Copyright: ® 1991-93 PROTEL TECHNOLOGY, INC


index
Advanced PCB 2.0 Help contents

To choose a topic, press [image] to select the underlined topic you want to view, and then Press [image]. With the mouse, point to the underlined topic you want to view, and then click the mouse button.

About Advanced PCB 2.0

Basic concepts

Commands

Tool bar shortcuts

Hot key shortcuts

Printing

Managing files

Screen regions

Reference

Questions and answers

After sales support

For information on how to use Help, choose [image] or choose Help-Using Help.


Copyright notice

Software and documentation (including this Help system)

© 1988-92 Protel Technology, Pty. Ltd.

© 1992-94 Protel Technology, Inc.

All rights reserved. Unauthorized duplication of the software, printed documentation, on-line help or related materials by any means, mechanical or electronic, including translation into another language is prohibited without the express written permission of Protel Technology.


Questions
Commonly asked questions

User interface, general matters

What causes slow screen re-draw?

Why has Advanced PCB slowed down during a sesson?

What causes low memory messages?

How are component Designators/Comments moved?

Why are some menu commands dimmed (gray)?

Why do polygon planes disappear after generation?

What causes errors when loading Tango or PADS files?

Why can't components be moved to the edge of the workspace?

How do I highlight connections?

How do I use internal plane layers for more than one net?

Netlists and autorouting

Why are existing components reported as missing?

How are missing (netlist) components loaded?

How is the ratsnest (connection) display updated?

What are validation errors?

Why does the autorouter cross over existing tracks?

What causes slow or unsatisfactory routing?

Why are there extra unconnected ratsnest nodes?

Why doesn't Unroute work on connections?

How do I edit or add ratsnest connections?

Design Rule Checking

Why does DRC generate false errors?

How are DRC (design rule check) highlights reset?

Printing and plotting

Why is pen plot quality poor?

Why does printer output run to several pages?

Why was no legend included in the Drill Drawing plot?

How do I generate alignment targets for plots?

What are the NC drill file extension names?

Gerber plot files

What version of the Gerber (RS-274) format is supported?

What limits are placed on Gerber files?

What apertures should be used for thermal reliefs?

What causes gaps inside Gerber fills?

How are apertures auto-generated

Why are unused apertures generated?


Redraw_Speed
Why is screen re-draw slow?

Because use of the workspace involves interacting with Windows graphics routines, these processes can be markedly slower than in systems which allow direct access to the video hardware (as in Protel Autotrax). It is also useful to consider than many users will be working on higher resolution graphics systems (e.g. 1024x768 or higher) where screen redraw is inherently slower. There are several factors that can effect the redraw speed of Advanced PCB. Versions 1.12 and 2.0 make extensive use of floating point calculations when calculating screen redraw or when placing objects with 32 bit precision (DRC, array placement and external polygon planes, for example).

Processor and numeric co-processor

The processor type and clock speed are the most important elements of redraw performance. We strongly recommend a 486DX processor, which has an internal floating point co-processor. If you are using a 386 or 486SX-based system, we recommend that you add a floating point co-processor to your system.

Fast graphics

Two types of acceleration are used to improve Windows graphics performance. The most common is "bit blitter" acceleration, which speeds the display of bitmap objects (including text). Other acceleration routines concentrate on vector calculations. Many "Windows accelerator" cards speed-up bitmap rendering and some types (e.g. S3 chipset cards) speed-up vector rendering. Because Advanced PCB is a vector drawing environment, cards that improve vector redraw provide the best overall performance. Protel is exploring Display List Processing  and other specialized technologies to enhance redraw performance. The popularity of Windows has already created a wide demand for better graphics performance, particularly for demanding CAD and other graphically oriented systems so we believe that the problem is a short term situation.

A number of users with "local bus" 486DX2 (66MHz) systems and Windows "accelerator" graphics cards report that this hardware provides satisfactory re-draw performance.

Tips and shortcuts for improving productivity

Preview mode minimizes the amount of vector information which must be re-drawn as you change your view of the screen. To invoke this mode, choose Options-Layers then select the Current Layer Only or All Layers Off button. When active, this option displays one layer at a time.

When toggling layers (*, + or - key) only the current layer is displayed, with the following exceptions:

Signal layers are displayed with the Multi-layer (through-hole pads) visible.

Mechanical Layers are displayed with the current layer if they have been specified in the Output Options dialog box.

One of the best ways to overcome slow redraw performance is to avoid re-drawing the screen at all. This is one reason why we have included so many sophisticated automation tools. Once example is Advanced PCBs uniquely powerful global editing system, which can remove the need to make numerous individual edits of primitives. Experienced Advanced PCB users tell us that they make extensive use of the following techniques to maximize productivity:

Spacebar (and {BMC PGDN.BMP}, {BMC PGUP.BMP}, {BMC HOME.BMP}, etc.) to abort the redraw. This is particularly useful when moving object across large areas. As soon as you know you need to change you view again, press one of these keys to stop the re-draw, rather than waiting for the screen to refresh.

Zoom-Point command allows precise definition of the display area, minimizing the need to adjust the workspace several times.

{BMC CTRL.BMP}+{BMC PGUP.BMP} or {BMC PGDN.BMP} zooms to the highest (or lowest) zoom level in a single operation.

{BMC SHIFT.BMP} +{BMC PGUP.BMP} or {BMC PGDN.BMP} zooms in 1/10 normal increments for fine adjustment of the viewing area.

Draft Mode display can speed redraw, especially for text and arcs. Speed increase is especially noticeable at higher zoom levels. The Draft Tracks Threshold option (Options-Preferences command) allows the user to designate single pixel tracks (below the specified threshold) rather than the full outline of these tracks. This option will greatly speed re-draw and also makes it easier to edit the non-track primitives in the layout.

  while panning, increases panning increment to 1/2 (rather than 1/8) of screen.

Selection speed

Selection speed is not directly related to redraw speed, but like redraw is a function of the system speed. In Advanced PCB, the direct selection command ({BMC SHIFT.BMP}+{BMC LMOUSE.BMP}) has to recursively search the entire data structure, e.g. all layers, for the boundary of all primitives at a certain coordinate. This process can slow considerably if the amount of data (size of the file) is large. To overcome slow selection, the user can use the following options:

Toggle Selection command. This method of selection specifies the "target" primitive, simplifying (and speeding) the selection. This form of selection is virtually instantaneous.

Move command works similarly. Using Move-Track or Move-Pad make selection of the target instantaneous, unlike the {BMC CTRL.BMP}+{BMC LMOUSE.BMP} shortcut.

Change command allows you to globally toggle the selection status of all primitives of a type.

Remember, Advanced PCB provides many productivity benefits: virtual memory support, multiple applications and files, device independence, etc., so productivity must be measured across the complete design process, not just redraw speed.


Memory_problems
What causes low memory messages?

Many users will find that 4MB of memory may not go very far when running Windows. This is especially true when SmartDrive is activated (see your Windows documentation). SmartDrive (in its Default form) uses about half of the "available" memory after DOS and Windows are loaded. If memory is a problem, try allocating less for SmartDrive. If you run multiple instances of Advanced PCB, this will also grab a significant amount of the available memory. Advanced Place and Advanced Route use memory intensively. We recommend at least 8MB of RAM for these modules.


Move_Component_Text
How are Designators/Comments moved?

Component text strings (Designators or labels and Comments) can be moved independently of the component decal or footprint. You can use the Edit-Move-String command or the {BMC CTRL.BMP}+{BMC LMOUSE.BMP} shortcut to reposition the component text anywhere in the workspace. You can also use SPACEBAR to rotate text in 90 degree increments or press X or Y to flip the text orientation. The component text remains "associated" with the footprint and will move relative the component if you move the component.

Caution: the overall boundary of components includes their text strings. If you cannot position a component near the edge of the workspace, make sure that no (hidden) text is limiting the move.


Dimmed_Commands
Why are some menu commands dimmed (gray)?

Commands are dimmed when they are unavailable due to the access codes set for the system. Some commands are available only when an Advanced PCB, Advanced Place, Advanced Router or Advanced SB Route access code has been provided. See the Environment Guide for further information.


Execution_Speed
Why has Advanced PCB slowed down during a session?

When performing a series of complex operations or after a long period of editing, you may notice a gradual degradation of system performance. This can be caused by the accumulation of a large Undo/Redo memory "stack". To clear the Undo/Redo stack, simply use the File-Save As.. command.

Periodic use of this command also speeds operations which require file access, as it re-write fragmented files to a contiguous block of hard disk space.

Another cause of performance degradation is caused by running low on system resources. This can happen irrespective of the amount of RAM available, as a fixed amount of DOS memory is allocated by Windows to manage system resources. Try closing other applications first. If this doesnt remedy the problem, you may need to exit, then re-start Windows.


Dead_Copper
Why do polygon planes disappear after generation?

If you define a Polygon Plane (copper pour) and it disappears after being generated, you have chosen the Remove Dead Copper option in the Place-Polygon Plane dialog box without having specified the Connect to Net option. Dead copper is any portion of the auto-generated plane which is not connected to a net.

To avoid this, be sure to specify a net which is represented by a pad inside the fill area, or disable the Remove Dead Copper option.


File_Load_Errors
What causes errors when loading ASCII, Tango or PADS files?

All ASCII text format files are validated during loading (File-Open command). Most errors are caused by format incompatibilities or out-of range values in the data. Advanced PCB file integrity checking is described on page 65 of the Advanced PCB User Guide.

Note: PADS-PCB and PADS2000 files must be in .ASC format. After conversion, these files may still contain out of range data which cannot be handled by Advanced PCB. See the Advanced PCB User Guide for information regarding assignment of PADS files to Advanced PCB layers.

PADS-PCB and PADS2000 provide the user with many options when generating files in PADS .ASC format. Some of these options may yield a file that is incomplete or otherwise unreadable to Advanced PCB. If you experience difficulty in loading PADS files, try re-generating the file using the PADS default (include all) output options. Some problems are due to ambiguities in the .ASC format that cannot be resolved by Advanced PCB. For example, Advanced PCB cannot translate PAD-PCB files that contain numeric net labels of four or less characters, because there is no inherent identification of these strings as net labels. In this case, manual editing of the .ASC file allows Advanced PCB to resolve the nets.


Tango PCB Series II format is supported. PCB Plus and Tango Pro (Windows) files are not currently supported.


Component_Boundary
Why can't components be moved to the edge of the workspace?

Every component has a bounding box that is defined by its minimum and maximum x and y coordinates for every primitive, including the coordinates that describe component text strings (Designator and Comment) whether or not the primitive is hidden or displayed. Movement of components is restricted by the entire boundary for the component, not just the displayed portion. If you are unable to move a component to the edge of the workspace, unhidden and hidden text (or other primitives) and check for text which has been moved away from the displayed portion.

In some cases, the bounding box for a component may not match its orientation, and position will be restricted. In some cases, it may be necessary to define the board outline away from the absolute origin to accommodate these limits.

Warning: even "empty" Comment strings can be moved and/or hidden. To find these, first enter some text into the Comment field in the Change-Component dialog box.


Connections_Selecting
How do I highlight connections?

Unlike Protel Autotrax, Advanced PCB has no highlight command. Advanced PCB uses the Select command to perform many of the same functions, such as deleting, moving or duplicating complex groups of items. Use Edit-Select-Net or Edit-Select-Connection to perform these operations.

See also:	Selection for Autotrax Users

Selection and highlighting

Select and De-select commands


Split_Planes
How do I use internal plane layers for more than one net?

Any of the four internal plane layers can be directly manipulated by the user. Objects placed on these layers become voids in the solid plane, when plotted. For example, you can place tracks to "cut" the solid copper into split planes. However, this approach will not allow more than one net to be assigned to a single plane layer.

Version 2.0 allows users to define split power planes, with full preservation of design rule checking and net integrity. To define a split plane:

1.	Make a power plane layer the current active layer.

2.	Choose the Edit-Place-Polygon command.

3.	Define the polygon for one part of the split plane. When the Polygon Plane dialog box opens, disable both the Horizontal and Vertical Hatching options so that an un-filled plane (outline) will be generated (the Horizontal and Vertical boxes should be unticked).

4.	In the Polygon Plane dialog box, assign the desired net to the plane.

5.	Repeat steps 3 and 4 to define polygons for all other nets to be connected on this split plane layer. Ideally, the entire plane will be divided into two or more unfilled polygon planes. This assures that all connected/relieved pins will be inside a polygon.

One polygon may be enclosed inside another. Polygon perimeters must not overlap (or cross).

6.	Once all polygons have been defined, direct connections or thermal reliefs can be created for each pin connected to the plane. This is done when nets are assiged to the plane layer (Netlist-Power Planes command) or when editing the plane connections for individual pins.

This feature is supported by clearance and DRC checking.


Missing_Components
Why are existing components (or pins) reported as missing?

There are two reasons why components will be listed as missing when a netlist is loaded, despite being present in the netlist file:

1. 	There is no footprint description that matches the literal package description in the netlist (e.g. DIP 14).

2. 	The netlist has more than one instance of a pin identifier (e.g. U1:A). Some netlist formats allow duplicate pin names (i.e. same component listed in two nets. using the same designator). In Advanced PCB, each instance of a pin, must be unique. Edit the netlist to resolve these duplications prior to loading in Advanced PCB.

Missing pins: Pins are reported missing when the schematic pin ID and PCB pad ID cannot be reconciled. See page 142 in the User Guide.


Placing_Multiple_Libraries
How are missing (netlist) components loaded?

To automatically place components, the netlist must include a package description which matches one of the available pattern names in a Advanced PCB library. Special consideration must be made for generic devices which may lack a specific package description in schematic sheets, such as transistors, resistors or capacitors. It is possible to load a netlist with multiple footprint libraries (see Loading Netlists) in the Reference Manual.

Missing components can also be a problem with netlists from some environments, where there is no ready method for performing this footprint assignment. Special support is provided in version 1.12 and 2.0 for OrCAD netlists. See page 142 in the User Guide.


Reload_Netlist
How is the ratsnest (connection) display updated?

To update the ratsnest display, go the Auto-Setup Auto Route and enable the Pre-router (Routing Passes). Be sure to disable all other passes. Use the Auto-Auto Route-All command to run the Pre-router pass only (this will take a few moments). When the pre-router is finished, press the {BMC END.BMP} key to refresh the display. The ratsnest will now reflect the physical connections present in the layout.

There are a number of instances when the Pre-Router should be run to update the relationship between the netlist and the physical layout:

1.	After using Place-Track to route connections (as opposed to using the Auto-Manual Route command to route using the ratsnest).

2.	After using Delete-Track (or the [image] key shortcuts) to change the connections (as opposed to using the Auto-Un-Route commands).

Note: In version 2.0, the Pre-Router pass will properly recognize and re-optimize partially routed nets.


Validation_Errors
What are validation errors?

All ASCII text format files are validated during loading (File-Open command). Most errors are caused by format incompatibilities or out-of range values in the data.

Note: PADS 2000 files cannot be successfully loaded, unless they are first converted to the text (.ASC) format..


Track_Violations
Why does the autorouter cross over existing tracks?

There is no inherent restriction regarding tracks crossing on the same layer, assuming the tracks belong to the same net. This is usually the result of component placement changes, prior to routing the board.

To eliminate this effect, use the Netlist-Optimize command before routing to reset the connection order.


Router_Problems
Why is routing slow or results unsatisfactory?

Autorouting speed and the quality of the routing result are the functions of several variables. It is important to understand that the time to taken to route a board increases with the square of the grid pitch. In other words, having the routing grid, e.g. from 20 mil to 10 mil means that the router has to work with 4X the number of routing points, and the time to route increases proportionally.

Measuring the quality of autorouter results is more difficult. Generally, it has to be conceded that the current routers do not yield a "hand routed" result. With optimum placement (using Advanced Place), Advanced Route can produce higher completion rates than hand placement, especially on complex through-hole boards. SMD or mixed boards are much more difficult to autoroute and the results are often less satisfactory.

If the track width + clearance are less than (or equal to) the routing grid, then routing will be faster. For example 8 mil tracks and 6 mil clearances (12 mil air gap) will route much faster on a grid of at least 20 mils.

Significant improvements will be noted when the Smoothing pass(es) are completed. These passes remove vias (by swapping track layers) and replace multiple track segments with single segments, where possible. Smoothing is applied progressively with each router pass. For example, if 5 passes are set, the first pass will result in minimal improvements and each subsequent pass will apply higher costs for undesirable conditions. It's preferable to choose 1 pass only than to choose 5 passes and stop the smoother after one pass. When smoothing, patience will be rewarded with a greatly improved result, with lower vias, direct routes, bussing (if allowed) and copper sharing.

Version 2 adds new smoothing options: two types of corner mitering are now provided: 45 degree lines or 90 degree arcs. The user can specifiy the corner radii (minimum and maximum) for these passes. Choosing the same value for both options will make all corners the same radius, however this may cause some corners to remain un-mitred, due to clearance restrictions.


Extra_Nodes
Why are there extra unconnected ratsnest nodes?

When connections are partially routed, the ratsnest remains terminated to track end. If this track is deleted, the ratsnest is left hanging at the termination point. Normally, it is preferable to use the Auto-Un-Route command, rather than the Delete command to delete track segments, preserving the integrity of the current netlist.

To correct this problem, re-load the netlist, then run the Pre-Router pass to re-synchronize the netlist and physical PCB. The Pre-Router updates the net i.d. information for each primitive.


Unroute_Limits
Why doesn't Un-Route work on connections?

In order to "unroute" a connection (and restore the unrouted ratsnest connection) the netlist information has to be present. This is maintained ONLY when the prior routing of the connection was performed by an autorouter or the Auto-Route Manual command -- not by manually placing tracks. Running the Pre-Router pass (Auto-Autoroute-All) can be used to update the net information for tracks which may have "lost" their net identity, due to manual editing.


Ratsnest Changes
How do I edit or add ratsnest connections?

In previous versions of Advanced PCB, there was no provision to "edit" or add nets. Version 2.0 adds full net editing capability to the PCB environment. Use the Netlist-Add Nodes,  and Delete Nodes commands to add pads to existing nets or remove pads from existing nets. Use the Add and Delete Connections commands to modify the ratsnest, such as changing the connection order within a net. The Netlist-Add Nets command can be used to add new nets to the PCB. These commands update the internal netlist for the current design, allowing the user to sucessfully autoroute and design rule check the project. Care must be taken when graphically editing nets from inside the PCB system, as this feature allows you to change nets. However, the Design Rule Check system will report violations of the original (loaded) netlist.

Version 2.0 support forward annotation from an updated schematic netlist, if you prefer to make netlist level changes from inside the schematic. Forward annotation compares the new version of the netlist with the internal PCB connection list and updates the PCB components and connections, even if the design is already routed or partially routed. Advanced PCB version 2.0 also provides links for back annotation of schematic sheets, using a .WAS file, generated when you use the File-ReAnnotate command.


DRC_Errors
Why does DRC generate false errors?

Version 2.0 of Advanced PCB features an enhanced Design Rule Check system featuring improved accuracy when processing complex board geometry. DRC false errors are usually the result of netlist problems. For example, check the netlist for extra pins, etc. when erroneous reports of missing pins are generated. DRC is extremely memory intensive and Windows errors may occur if the available resources are insufficient. If problems occur, try minimizing resource use prior to running DRC. Consider adding memory to your system, if you are consistently generating Windows error messages when running DRC.


DRC_Reset
How are DRC (design rule check) Error Markers reset?

DRC error markers are presented on a dedicated display layer (DRC Errors). The layer can be toggled off or on from the Options-Layers dialog box. The layer is reset whenever DRC is run with the Generate Markers option enabled. We have added an option to the version 2.0 Netlist menu to Reset DRC errors.


Plot_Problems
Why is pen plot quality poor?

Previous versions of Advanced PCB used the Windows pen plotter drivers. These drivers treat pen plotters as though they are RASTER devices, rather than VECTOR devices, resulting in poor plot quality and inefficiency. Versions 1.5 and 2.0 includes a File-Pen Plot command, which bypasses the Windows pen plotter drivers (and their many limitation and problems). See Printing for details


Print_Margins
Why does printer output run to several pages?

If you print runs (unexpectedly) to several pages, this may be the result of a conflict between the calculated print area and the area available in the target device. For example, many laser printers have a minimum margin area. Depending upon the options selected, Advanced PCB will tile your output across as many pages as needed. This can be a particular problem with drill drawings, which auto generate a legend outside the artwork area.

Versions 1.5 and 2.0 features a new pen plotting command, which bypasses the Windows pen plotter drivers (and their many limitation and problems). See Printing for details


Drill_Legend
Why was no legend included in the Drill Drawing plot?

The size, position and orientation of the legend is determined by the .LEGEND string placed in this layer. The following restrictions currently exist for drill drawing legends:

Graphics Symbol markers are limited to a maximum of 8 different hole sizes;

Character markers are limited to a maximum of 26 different hole sizes;

Size of Hole String markers are limited to a maximum of 8 different hole sizes.

See page 198 of the User Guide for details.


Alignment_Targets
How do I generate alignment targets for plots?

Unlike Autotrax, Advanced PCB does not provide specific target and moiré pads which can be placed as entities in the workspace. You must build these items using tracks and/or arcs on the mechanical layers. For convenience, save your targets as components in the footprint library. If your target photoplotter provides specific target apertures, you can manually edit the aperture tables to force this aperture code to any unique pad.


Drill_Extensions
What are the NC drill file extension names?

Three files are produced when generating an NC drill file:

The .DRL file (The binary Excellon format file, read by the N/C machinery).

The .TXT file (An ASCII version of Excellon file, which can be checked)

The .DRR file (An ASCII text report including the tool table, count, etc.)


Gerber_format
What version of the Gerber (RS-274) format is supported?

The Gerber standard has evolved over several years and, therefore, has many implementations. Protel uses a generalized subset of the format, to insure compatibility with the greatest possible number of software and hardware interfaces. The following specifications apply to Advanced PCB version 2.0:

Numeric formats: 2.3 (e.g. 12.899), 2.4 and 2.5;

Leading Zero Suppression: optional;

Trailing Zero Suppression: not allowed.

A (Protel format) aperture file (.APT) must be provided to the plotting bureau along with the Gerber plot files for each layer.


Gerber_limits
What limits are placed on Gerber files?

The following limits define the limits of Protels Gerber file implementation:

Maximum number of Apertures in an .APT file: 1000

Maximum size of any single aperture (manually created): 1000 mils

Maximum size of any auto generated aperture: 250 mils (default). This can be designated by the user (Library-Apertures dialog box).


Relief_Apertures
What apertures should be used for thermal reliefs?

Advanced PCB allows the user to generate apertures automatically for a design by choosing the Generate List from PCB button in the Library-Apertures dialog box..

If the target photoplotter does not support Relief type apertures, generate the aperture list with the Generate Relief Shapes option enabled. Otherwise a "Relief" shape will be assumed and generated. These relief type apertures will be used to "flash" each pin location where a connection is made to the internal plane. These "flashed" reliefs will reflect the shape generated by the plotter.

A "draw" (or "stroke") use aperture will then be assigned for generating the relieved pads (as specified by the user when defining the Reliefs in Gerber output options) and will be automatically assigned. These relief shapes will be painted or drawn when the file is generated.

"Painted" thermal reliefs on Advanced PCB are drawn with "conductors" at 45 degree angles. This will keep these conductors as isolated as possible from one pad to the next.

See also: How are apertures auto-generated?


Fill_Problems
What causes gaps inside Gerber fills?

Manual filling of complex shapes must be performed with care. Small placement errors may not be apparent at higher zoom levels. The smallest gaps will be visible when photoplotting. Normally, a small amount of overlay will insure that the area is covered. Use the File-Gerber-In command to view generated Gerber files (and make corrections) prior to plotting.


Auto_Apertures
How are apertures auto-generated?

The following descriptions indicate the calculation method used for all auto generated aperture shapes.

This method of aperture generation is ideally suited to users who are targeting raster Gerber plotters. Vector plotters require a custom aperture table. Please consult your bureau for requirements prior to generating plot files.

All apertures shapes except Relief shape are Multi-use (Flash or Stroke). Relief Shape are always Flash. Some plotting software/equipment cannot accept the Multi use description. Contact your plotting bureau to determine these restrictions prior to generating aperture files and plot files.

Apertures are clipped at a maximum size of 250x250 mils.

APERTURES AT PAD LOCATIONS

Apertures generated for Copper layer

X	=	XSize

Y	=	YSize

Shape	=	Pad Shape

Apertures generated for Thermal Reliefs (internal Power Plane layers)

X	=	Hole Diameter = (2*PwrGndExpand)

Y	=	Hole Diameter = (2*PwrGndExpand)

Shape	=	ReliefShape

Draw Apertures generated for Thermal Reliefs (internal Power Plane layers)

X	=	Relief Air Gap

Y	=	Relief Air Gap

Shape	=	Rounded

Apertures generated for Power Plane layers (provide pin-to-plane clearance)

X	=	Hole Diameter = (2xPwrGndExpand)

Y	=	Hole Diameter = (2xPwrGndExpand)

Shape	=	Rounded

Apertures generated for Solder Mask layers

X	=	XSize = (2xSolder Mask Expansion)

Y	=	YSize = (2xSolder Mask Expansion)

Shape	=	Pad Shape

Apertures generated for Paste Mask layers

X	=	XSize = (2xPasteMaskExpansion)

Y	=	YSize = (2xPasteMaskExpansion)

Shape	=	Pad Shape

APERTURES AT VIA LOCATIONS

Apertures generated for Via (Copper layers)

X	=	Via Diameter

Y	=	Via Diameter

 	Shape 	=	Rounded

Apertures generated for Solder Mask

X	=	Via Diameter = (2*Solder Mask Expansion)

 	Y	=	Via Diameter = (2*Solder Mask Expansion)

Shape 	=	Rounded

Apertures generated for Power Planes (provide pin-to-plane clearance)

X	=	Hole Diameter = (2*PwrGndExpand)

Y	=	Hole Diameter = (2*PwrGndExpand)

Shape 	=	Rounded

ARCS

X	=	Line Width

Y	=	Line Width

Shape	=	Rounded

TRACKS

X	=	Width

Y	=	Width

Shape 	=	Rounded

FILL

 	X	=	X2-X1 (yields width of fill)

 	Y	=	Y2-Y1 (yields height of fill)

Shape	=	Rectangular

TEXT

X	=	Line Width

 	Y	=	Line Width

Shape	=	Rounded

DRILL SYMBOL

An aperture is always automatically generated for Drill Drawing symbols (and text), per the current Drill Symbol Size setting (stroke width, assigned for symbol size automatically - 50 mil symbol yields 7 mil aperture).


Unused_Apertures
Why are unused apertures generated?

Users may find that auto-generated aperture files contain one or more apertures that are not present in the Gerber plot file(s). This is because the program creates a general set of apertures based upon the requirements to generate ALL Gerber layers for the file, not just the specific layer being generated at any given time. These apertures will include apertures for generating text, solder/paste masks, thermal reliefs, etc.

For example, an aperture is always automatically generated for Drill Drawing symbols (and text), per the current Drill Symbol Size setting (stroke width, assigned for symbol size automatically - 50 mil symbol yields 7 mil aperture). The same holds true for any text in the PCB.

If desired, you can manually delete any apertures which are not required for a given plot, when submitting the files to your bureau.


After sales support

If this package is an upgrade to an earlier verson of Advanced PCB, your software is already registered. You will receive diskettes and updated documentation for version 2. The new version will use your existing Hardlock (software protection device) mounted on your computers parallel port. A new access code will be supplied which enables the version 2 software. This will be supplied in a letter, which accompanies the upgrade, or under separate cover. If you do not recieve the required version 2 access code, please contact your Protel dealer for assistance.

If this is your first purchase of Advanced PCB, please sign and return the enclosed License Registration Card. By returning this card, you acknowledge that you have accepted the terms of the license. You should also notify Protel (or your local dealer or distributor) if your address changes.

Maintaining your registration ensures on-going access to technical support, upgrade notices and other important product information.

Your Protel Design System License Number is stamped on the Hardlock device. This single device (and serial number) is used to support several Protel Design System modules. Some modules may require a separate hardware lock. Others may not require either a hardware lock or access code. In any case, the Protel Design System license number identifies you as a user, so we recommend that you record this number in a convenient location, so that you can refer to it when making any inquiries about the software.

Always refer to this serial number when making any inquiries regarding Advanced PCB and other Protel Design System (for Windows) products. Protel products are supported by an international network of distributors and dealers. When you register your software you become eligible for technical support.

Support policies and procedures vary from country to country. If you have questions about your software, please direct your initial inquiry to your Protel dealer.

When inquiring about your Protel software, always quote your software license registration number. The license number for this package appears on the registration card shipped with your Advanced PCB software.


About Version 2.0
About Advanced PCB 2.0

User Interface changes (version 1.5 and 2.0)

The user interface of the software has been updated in version 1.5 and 2.0 from earlier releases.

The Toolbar has been re-designed and now includes buttons for 28 commands. A De-Select All button, Route Manual button, Add Connection button and Align Components button have been added to the toolbar for version 2.0

When the cursor moves over a tool button, its function is displayed on the Status Line at the bottom of the workspace window:

We have re-designed the Status bar to include the Layer selector button and layer name / color. This allows the toolbar to be "hidden" without losing access to the Layer button.

The color palette system in this version, provides 233 pre-defined colors. An additional palette of 16 user-defined custom colors is also provided. If you have 8-bit or 24-bit color graphics, a wide range of solid color values will be displayed. This system by-passes the standard Windows Palette Manager, but is fully compatible with other applications which use the Palette Manager.

The Current menu has been changed slightly from previous versions (as illustrated on page 169 in the Reference).  Commands for Via Diameter, Via Hole, Via Layer Pair and Free Text have re-organized so that no option is more than two layers deep in the menu structure.  The hot key shortcuts for these commands have been changed to reflect the new menu structure (see Current menu).

32-bit precision

Advanced PCB versions 1.5 and 2.0 add 32-bit database and output capabilities to the design system. Dimensions (for all entities) and grids can be specified to .000001 inch accuracy. As in version 1.12, angular resolution is to .001 degree for either arcs or circular arrays. Coordinates are displayed in mil (.001 in) or metric units in the following formats: imperial (0-100,000.000mils) or metric (0-2540.0000mm). The unit of measure, either mils or mm is displayed on the Status line at all times.

The number of decimal places displayed in the Status line is dependent upon the current Snap grid, cursor position and zoom settings. For example, setting a Snap grid of .05mils will display 20, 20.05, 20.1, etc. as the cursor is moved. Values are rounded off to the nearest significant unit, with trailing zeros removed. Use the Current-Shap Grid command (or press the Grid button on the toolbar) to change the grid.

Change between metric and imperial measure by choosing the Options-Toggle Units command, changing the Snap Grid units to mil or mm or by pressing the Q key.

See also:	Version 2.0 Features


Version 2.0 Features
Verson 2.0 features

Over 100 refinements, improvements and new features have been added to version 2.0. Most of these changes are described in the new documentation set which now includes an Environment Guide, User Guide and separate Advanced PCB Reference. This On-line Help file includes descriptions of the complete Advanced PCB 2.0 system, including those changes which were implemented after the manuals were printed. For a quick review of all version 2.0 changes, see the README.TXT file.

Click to review these featured new or revised capabilities:

Advanced Route Improvement

Advanced SB Route option

Aperture files

Array placement

ASCII file format changes

Autotrax moire and target pads

Cross Probing Advanced Schematic

Draft Tracks Threshold option

ECO (Engineering Change Order) system

Forward Annotation

Gerber files

Hardlock and Access file support

Links to Advanced Schematic

Loading pad and component libraries

Manual routing improvements

Net and connection editing

On-line DRC system

Pad stacks

PADS 2000 support

PADS and PCAD files

Pen plotting changes

Polygon Plane improvements

ReAnnotation options

Report generation

Rotation Step option

Selection rule changes

Split power plane capabilities


Selection rule changes

In version 2.0, when using selection commands (Edit-Select-All, Edit-Select-Inside Area), free primitives will not be included in the selection if they are hidden (Options-Display command). Also, free primitives will be selected only if their layer is active (Options-Layers command). This change in selection rules for version 2.0 allows the user more control over free primitives that are included in a selection by hiding specific primitives or by turning off specific layers. These changes apply only to free primitives, not components. Other selection rules are unchanged.

See also:	Selection


Pad stacks

Users can now define pad stacks for all multi-layer pads. Separate pad size and shape attributes can be defined for the Top layer, Mid 1-14 layers and Bottom layer. When printing mid-layers, unconnected pads are now automatically removed from the artwork (optional).

Protel uses the Multi-layer to display through-hole pads and vias. When a pad or via is assigned to this layer, it is automatically deemed to be present on each physical layer of the design. Automation features such as autorouting and DRC work transparently with Multi-layer data. Similarly, printing and plotting includes Multi-layer data when generating output.

A new feature allows you to define the shape and size of multi-layer pads independently on the Top, Mid1-14 and Bottom layers to create pad stacks.

If you require layer-by-layer control of pad/via entities beyond this new feature, there are two options:

You can edit the Gerber data directly (this is generally not recommended);

You can place single layer pads on other physical layers at the same location as the multilayer pads.

This option allows you to save the customization in the PCB file and allows Design Rule Checking.

Note: When placing these pads, be sure to set the designator to "empty" - not "zero" (0), or DRC will report errors at each pad location.

Note: When exporting files in Autotrax format, the Top layer pad description is used to define the pads.


PADS 2000 file support

ASCII (.ASC) versions of PADS2000 files are now  loaded, using the same method applied to PADS-PCB files. Users must assign numbered PADS layers to the appropriate Advanced PCB layer during the initial load sequence. Earlier problems with loading PADS files have been corrected for version 2.0


Engineering Change Order (ECO) system

ECO system: An engineering change order system has been added to version 2.0 of Advanced PCB. This system (enabled under the Options-Preferences command) records physical changes to the design and generates an ASCII report file (filename.ECO). This file conforms to the PADS ECO format. This system also supports updating of the design.

Specific netlist level changes that are supported by the system include:

Adding or deleting a pin to a net

Adding, deleting or renaming a net

Adding or deleting or renaming a component

Changing a components footprint field (pattern).

Opening or closing a file (recorded in .ECO file).

A Netlist-Run ECO File command will process these changes in the PCB. Users can externally modify the .ECO file to update the PCB. This feature is documented in the User Guide and Reference.


PCB net editing

Users can now graphically edit ratsnest connections from inside Advanced PCB. This is supported by 5 new Netlist menu commands: Add Nodes (to net), Delete Nodes (from net), Add/Modify Connections and Add Nets. This feature is partially documented in the User Guide and Reference. However, the Add/Modify Connections and Delete Connections commands have been added since the manual was printed.

See also:	Netlists

Netlist-Add Nets

Netlist-Add Nodes

Add/Modify Connections

Delete Nodes

Delete Connections


Advanced SB Route
Advanced SB (shape-based) Route

A new product, Advanced  SB Route, provides a high-end autorouting solution for Advanced PCB users. Advanced SB Route provides shape-based (or gridless routing and uses technology, based on the Specctra SP-10 router from Cooper and Chyan Technology, Inc. This router will generate higher completion rates, using fewer layer, with a more manufacturable result, especially for mixed pitch or SMD designs. Options are available for advanced design rules, design for manufacture/test and hybrid design. Contact your dealer, or Protel for details.


Polygon Plane improvements

The Polygon Plane feature now makes full use of Advanced PCBs 32-bit placement accuracy, resulting in improved pour quality. Copper pours are now fully editable after placement. Users can move, add or delete vertices and there is an option to fill pours with area fills, as well as with horizonatal and/or vertical tracks. Fills will now regard and automatically connect to primitives that belong to the same net (optional feature). These features are documented in the User Guide and Reference.

The Edit-Change-Repour Polygon is used to update a selected polygon at any time. This is especially useful when you need to move or place a primitive inside the polygon area. After making the changes, choose the Repour Polygon command and then click to select the polygon. The Edit-Polygon dialog box will open. You can change any attributes (e.g. polygon grid and polygon track sizes, net assignment, etc.) at this time, if desired. Click Place and the polygon will be re-generated using the original vertices (corners).

The Edit-Change-Edit Polygon Vertices command allows you to alter the shape of a copper pour, without re-generating the polygon. Vertices can be moved, added or deleted graphically. The [image] and [image] keys are used to add or remove vertices from outline segments. When editing vertices, pressing [image] will convert a track segment into an arc and pressing [image] will convert an arc segment into a track.

You can also specify fills (rather than tracks) to fill the polygon shape. Additionally, an Edit-Change-Replace Selection with Fills command has been added. This command will remove a selection, replacing solid areas (in polygons, typically) with area fills which will print more efficiently.

The Pour Over Same Net option will flood the copper over the top of exisiting tracks, fills or vias associated with the assigned net, when the Connect to Net option is enabled. When this option is not enabled, the pour area will avoid touching these same net primitives, observing the air gaps specified for these items under the Netlist-Clearances command.

Edit-Toggle Selection-Polygon and Edit-Move-Polygon commands have been added to the Edit menu. When a polygon is moved, the user will have the opportunity to change the polygon design rules, as when editing an existing polygon pour. Polygons can be copied (Edit-Copy command) to the clipboard and pasted (Edit-Paste command) to a new location. As when using the move command, the Place-Polygon Plane dialog box opens, allowing the user to change the design rules, prior to repouring the copper. The clipboard now fully-supports polygons. Users can Cut or Copy polygons and Paste them into PCB docuements. As when moving or re-pouring polygons, the Place Polygon dialog box will open, allowing the user to re-define the polygon design rules prior to generation.

An Edit-Delete-Polygon Plane command has also been added, to simplify  removal of copper pours.

In previous versions, DRC reported numerous false errors inside legally constructed Polygon Planes. This problem has been corrected in version 2.0 and DRC can be successfully run at any time.

Using polygon planes to define split planes

In previous version of Advanced PCB, each internal plane layer (1-4) was restricted to a single net assignment. Version 2.0 allows users to define split power planes, with full preservation of design rule checking and net integrity. To define a split plane:

1.	Make a power plane layer the current active layer.

2.	Choose the Edit-Place-Polygon command.

3.	Define the polygon for one part of the split plane. When the Polygon Plane dialog box opens, disable both the Horizontal and Vertical Hatching options so that an un-filled plane (outline) will be generated (the Horizontal and Vertical boxes should be unticked).

4.	In the Polygon Plane dialog box, assign the desired net to the plane.

5.	Repeat steps 3 and 4 to define polygons for all other nets to be connected on this split plane layer. Ideally, the entire plane will be divided into two or more unfilled polygon planes. This assures that all connected/relieved pins will be inside a polygon.

One polygon may be enclosed inside another. Polygon perimeters must not overlap (or cross).

6.	Once all polygons have been defined, direct connections or thermal reliefs can be created for each pin connected to the plane. This is done when nets are assiged to the plane layer (Netlist-Power Planes) or when editing the plane connections for individual pins.

This feature is supported by clearance and DRC checking.


ReAnnotation options

Re-annotation of the board now includes options to re-annotate for right-to-left, left-to-right , top-to-bottom, bottom-to-top and by position coordinates.


Forward annotation

Netlist-level changes (from schematics or other utilities) will now be automatically updated in the physical layout when the new netlist is loaded. This powerful new feature will handle component additions/deletions, net additions/deletions, split nets, joined nets, re-named components, re-named nets, etc. Routed PCB connections will be returned to an un-routed condition  and ratsnest connections will be moved or deleted to reflect connectivity changes. This feature is documented in the User Guide and Reference.


Rotation shortcut

User can now define the rotation step used when the Spacebar shortcut is available, as when moving selections or placing primitives. The amount of rotation for each keystroke is set using the Rotation Step Size option (Options-Preferences command).


Cross probing Advanced Schematic

Advaned PCB can now cross probe Advanced Schematic parts, pins and nets. This feature is documented in the User Guide and Reference.


Advanced Route improvements

Auto-Manual Route has been improved to allow interactive re-routing of routed connections with automated removal of "obsolete" track loops. To use this new facility, choose the command and click on any track segment. A ratsnest connection will "guide" you to the next pad in the net. The new route can be terminated at the pad or an any track segment between the starting point and the pad. The "disused" placed tracks will be removed automatically, once you click to end the re-route. This improved version of Manual Route is now supported by a button on the toolbar. Remember, Manual Route works only with netlisted connections or connections created with the new Netlist-Add Nets, Add Nodes or Add/Modify Connections commands. Two new hot keys assignments support manual routing: press [image] to add a via when manually routing; press [image] to place a pad. Pads automatically inherit any power plane assignment associated with the current net.

A new command, Auto-Route-Advanced Route Connections, has been added. This command will route a single connection, using Advanced Route passes. Numerous refinements have been made to Advanced Route routines and most users will notice improved router performance over earler releases. Most of these features are documented in the User Guide and Reference, although some enhancements have been added since the manuals were printed:

Auto-Auto Route-Advanced Route Connections command

This command is used for interactively routing individual connections, like the Auto-Auto Route-Connection command. Unlike Route-Connection, Advanced Route Connections initializes the Maze Router passes, bypassing the Memory and Line Probe passes for efficiency when routing more difficult connectons. When the command is chosen, a cell map will be created for the board, then the user will be prompted to choose the first connection to be routed, etc. Pressing ESC will abort the command.

Setup Autorouter options

A new set of options supports corner mitering during the Advanced Route Clean-up passes. Users can specify either 45 degree re-corner or arc replacement. The radius for either option can be defined by the user. A Fixed Radius option forces the miter/arc replacer to use the specified size. Mitering and arc replacement is performed for each existing 90 degree corner, where clearances permit. The replacer will start with the specified radius. If insufficient clearance blocks replacement, the radius is halved and the replacer attempts to place the arc or mitre a second time, and so on.

Manual routing

If you use the Auto-Manual Route command, the size of the tracks and vias used will be those set in the Auto-Setup Auto Route dialog box, not the settings in the Current menu.

You can backtrack from the current routed position by pressing [image] as you route. Each press of [image] will remove one segment, restoring the ratsnest for that connection.

New Net Editing options allow the user to re-define the connections (ratsnest). The user can also specify Dynamic Reconnect (Options-Preferences) which guides the user when manually routing netlisted connections by re-connecting the ratsnest to the nearest pad as the user manually routes the net. The Loop Removal option (also Options-Preferences) will automatically remove duplicated track connections during manual routes.

Notes on Unrouting (Advanced PCB)

You cannot use the Auto-Un-route command to remove placed tracks from the board unless they were routed from the current netlist (routed using either the autorouter or the Auto-Manual Route command).

If you load files created in Protel Autotrax, these cannot be unrouted, as there is insufficient information in the Autotrax file format.

If you wish to unroute all of the tracks and vias on an Autotrax board, use the Auto-Unroute All command which will convert all of the connections on the board to unrouted, then use the Select commands to delete all the free primitives.

Route priority, Route Class and Layout Directives (Advanced PCB)

The route priority field (part of the attached netlist portion of a .PCB file) is now implemented in this version of Advanced PCB. You can assign route priority from the Netlist-Edit-Net command. You can view .PCB files after saving them using the Protel Text format option (Save; Save As... command).

Layout Directive information from Advanced Schematic is recognized when you use the Protel 2.0 netlist format. PCB nets can now have routing classes assigned (Netlist-Edit-Net command) for use with Advanced SB Route (which recognizes classes for nets).

Use Of "Edit-Set Origin" When autorouting/ auto placing (Advanced PCB and Advanced Route)

Using "Edit-Set Origin" could result in poor autorouter performance in earlier versions. This was due to the absolute coordinate system used by the Auto place and Autoroute systems.

This problem has been corrected for version 2.0. It is now possible to leave the board contents and origin at any point inside the workspace and Advanced PCB will calculate the correct cell map for the design.

It is still important that the routing grid and component pad placements are compatible, however.

The "Auto-Move to Grid" command is not a practical solution if the board is partially routed. Only one option exists when free primitives must also be aligned to the absolute grid. In this situation the entire design must be shifted to obtain alignment. This can easily be performed using "Edit-Select-All" and "Edit-Move-Move Selection" commands. Before this is done, the absolute origin must be restored so that the coordinate display can be used as an aid for alignment. To restore the absolute origin, set the snap grid to 1 mil and choose

"Edit-Jump-Absolute Origin" then "Edit-Set Origin". This must done using the keyboard (without the mouse) if "Options-Preferences-Lock Cursor" is enabled.

The relative and absolute origins are now aligned and the coordinate display on the status line can now be used as reference for realigning the components and primitives to the absolute grid. Choose "Edit-Select-All" then "Edit-Move-Move Selection". Be sure that the snap grid is still set to 1 mil then select the center of one of the pads as the "Reference Point". Now move the selection until the status line indicates X and Y coordinates that are a multiple of the routing grid (Ex: if the routing grid is 20 then the last 2 digits of the X and Y coordinate display should read 00, 20, 40, 60, or 80), and choose that location.

Hint: The center of a pad can easily be located if the cross of a relief pad is used as an alignment target. Another method is to click on the pad for editing which will cause the cursor to jump to the center of the pad if the snap grid is set to 1 mil and the "Options-Preferences-Snap to Center" option is enabled.

The relative origin can now be restored without compromise to router performance.

Version 2.0 creates a "cell map" of the entire board from the current Relative (0,0) origin to the Maximum X and Y coordinates of the PCB file and moves the board (temporarily) to this origin for routing. This is unlike previous versions which used the absolute origin (lower left limit of workspace) to determine the cell map size. If the board was placed away from the absolute origin, the cell map would needlessly include the empty area, increasing the memory allocation.

Fractional Routing Models (Advanced PCB + Advanced Route)

Two of the sample routing models (in the Reference Manual) refer to fractional grids. It was not possible to define fractional grids in previous versions Advanced PCB. Fractional grids are fully supported in version 2.0.

Hint: Using rounded settings of x.750, x.666*, x.500, x.333*, x.250. for fractional routing grids helps to keep the memory requirements reasonable, while providing additional flexibility in routing -- particularly for SMD and single sided routing.

*These settings will provide even multiples for routing 25 mil and 50 mil pin spacings, allowing 2 or 3 tracks to pass between pads.

Router performance

Version 2.0 features improved router performance -- particularly for SMD and single-sided routing. It is now possible to define fractional grids (this feature was not supported in previous versions). Fractional grids allows you to define routing models which support multiple tracks between pads and tracks between SMD pads. Tracks are kept clear of SMD pads during the early stages of routing, if the Hug Before 100% is enabled. This helps to preserve sufficient space for a via -- so that the pad can gain access to another layer for routing. During Smoothing passes, this will be ignored.  A special Fan Out pass can be used to generate fan out patterns around SMD components.

Pre-Router pass

The Pre-Router pass is used to update the internal routing connection list, whenever physical changes have been made to the PCB, independent of the netlist. This prevents the router from re-routing a previously routed connection, for example. In previous versions (version 1.12 or earlier), this pass was not properly recognizing (previously) partially routed nets and duplicate connections would be autorouted or unrouted connections would be missed. Versions 1.5 and 2.0 correct this problem and partially routed nets will be properly re-optimized.


Draft tracks display

Users can now specify a Draft Tracks Threshold. This option will allow draft mode (outline) tracks to be displayed as single pixel width lines, below a pre-defined width. This option will greatly speed screen re-draw when users dont require the full outline track display. The user can also specify Clean Redraw (Options-Preferences command). This option will redraw the display more frequently when moving or deleting object. Leaving this option disabled speeds up system response, when a neat and tidy display is not required.


On-line Design Rule Checks

In versions 1.5 and 2.0, an on-line DRC system detects clearance violations (including logical violations) while you manually edit your board, when a netlist is loaded. The system uses the clearances set under the Netlist-Clearances command. When you place an item that violates the minimum air gap (track-to-track, track-to-pad, etc.) the placed (or moved) item and at least one of the violated items will flagged as a DRC error (an outline of the primitive violation zone will be displayed on the DRC Errors layer). Clearing the collision(s) will re-set the flags back to off. The system recognizes the net attributes of items and will not highlight items that belong to the same net.

When this option is enabled, the DRC layer (Options-Layers dialog box) is automatically activated. The flags for offending items are displayed using the color assigned to this layer. De-activating this layer will disable the display of DRC error flags. In version 2.0 the "flag" shows the clearance zone around the primitive. This feature provides visual feedback as you manually move offending items to remove the violation.

This feature can be toggled on or off from the Options-Preferences dialog box.

The Netlist-Clearance Check command provides a way to check the whole project for clearance violations any time a netlist is loaded. Any violations will be flagged, as described above. If no violations are detected, the system will beep.

Another new command that supports DRC is Edit-Jump-Design Rule Violations. This command will place the cursor over a flagged violation. Once the have corrected the clearance problem, the DRC flag will be re-set (turned off). Choosing the Edit-Jump-Design Rule Violations command will move the cursor to the next clearance error, etc.

A count of (current) clearance violations is displayed in the PCB Information dialog box, accessed from the Info-PCB Status command.


Pen plotting changes

A new command, Pen Plot, included in the File menu in versions 1.5 and 2.0. This command provides an independent pen plotting system which bypasses the standard Windows plot drivers (and their associated problems and limitations). Although it is still possible to use the Windows plot drivers, we recommend that you use the new Pen Plot option when using HPGL and DMPL compatible vector plotters.

Note: Protel does not develop or maintain Windows print/plot or display drivers. To obtain information about current drivers, please contact the hardware manufacturer or Microsoft Corp. directly.

See also:	Introduction to Printing


Links to Advanced Schematic

A number of special features and "links" have been provided to enhance the interoperability of Advanced Schematic and the Advanced PCB layout system:

Re-annotation and Back Annotation

ReAnnotation refers to re-labeling the component designators, based upon their physical location in the PCB layout. BackAnnotation refers to updating schematic sheet file component labels, based upon changes in the PCB layout.

ReAnnotation of the PCB:

Versions 1.5 and 2.0 add a ReAnnotate command to the File menu.  See the Advanced PCB User Guide and Reference for details.

Forward annotation from schematic netlists

Advanced PCB now updates PCB component and connection information when a new netlist is loaded for the current layout. The supported changes are documented in the User Guide and Reference.

Cross Probing between PCB and Schematic:

Cross Probing refers to on-line "links" between Advanced PCB and Advanced Schematic. These links are available when running the two packages with a circuit design (sheet or project) and board layout file open at the same time. Advanced PCB version 2.0 supports cross probing back to Advance Schematic (version 2, or later).


Hardlock and access code support

Advanced PCB access codes for each software module are stored in files identified by the extension ACCESS.CDE, located in the Windows directory, either on a server (if running the software over a network) or on an individual machine. This CDE file can contain access codes for any number of products or hardlock serial numbers

Versions 1,5 and 2.0 supports multiple hardlocks. All CDE codes are scanned when the software is run.

In the Set Access Codes dialog box, only the first instance of each license is displayed. Duplicate codes will not have their license types listed. In other words, if you have entered two valid codes for Advanced PCB, Advanced PCB will only be displayed once.


Report generation

When you choose the File-Report command, or click the Report button  from the Library-Components dialog box, or load a netlist, you will be presented with two options for the report format:

The first is standard Protel output and the second is in the CSV output. CSV stands for Comma Separated Values. This is a file format that can be loaded into most spreadsheets and databases. Both options generate reports in ASCII text format.

For example Microsoft Excel will open a CSV format text file, when the Text option in the File-Open dialog box is selected Change the Column Delimiter Value option in the dialog box to "Comma".

Version 2.0 featues enhancements to some of the existing report formats. For example, the (autorouter) .LOG file and .DRC file now include setup information that provides a more complete description of the board file when the report was generated.

Pick and Place report

A new report (File-Reports-Pick And Place) generates a new support file for programming Pick and Place equipment. An ASCII report file (.PIK) is generated. This feature is described on page 224 of the Advanced PCB Reference.


Gerber files

Using "File-Gerber-Gerber In" and "File-Gerber-Batch Load" (Advanced PCB)

The Gerber loader now recognizes Gerber 2:3, 2:4 and 2:5 numeric formats. You now have the option to specify the numeric format when generating Gerber files in version 2.0.

The "File-Gerber-Gerber In" and "File-Gerber-Batch Load" commands do not incorporate file integrity checking. This enables Gerber files to be viewed without modification. However this may lead to difficulties if non Advanced PCB Gerber files are saved without taking a few precautions.

If the workspace appears empty after opening a Gerber file, the data may exist beyond the legal boundaries (the Advanced PCB environment allows data within X:0-100,000.000 and Y:0-100,000.000 coordinates). This situation can be confirmed by viewing the "PCB Information" dialog box (Choose "Info-Board Status..."). "Board Dimensions" beyond the 0 to 100,000.000 range and quantities greater than zero for "Physical Items on PCB" are indications that data exists beyond the workspace boundaries.

Data can be moved within the borders of the workspace by using the following method:

Choose "Edit-Select-All".

Choose "Edit-Move-Move Selection".

Select a Reference Point near the upper right corner of the workspace.

Place the selection near the lower right corner.

If this procedure was successful the screen will redraw with the data in view. If not, try moving the selection in another direction.

When this is complete, save the document using the text format then open this file. Integrity checking will take place as the text format file is opened. Integrity checking ensures that invalid data can not cause application or system errors.

Note: When re-generating edited Gerber files, Solder Mask expansions, Paste Mask expansions and Thermal Relief expansions are re-applied to the CURRENT data. Be sure that you re-set these values to zero before regenerating the Gerbers.


Aperture files

Manual aperture file generation

A special aperture type must be included in the current aperture list, whenever the PCB includes pad or via holes. This is because Advanced PCB needs to provide an aperture for stroking Drill Drawing symbols and/or text, when these layers are generated as Gerber files. Advanced PCB looks for this aperture, even if you are not generating a Drill Drawing plot. If no holes are in the file (no vias, all pad holes defined as zero, for example), the aperture is not required.

If using automatic aperture generation, see below. The required apertures for Drill Drawing symbols and other text is automatically provided with the stroke width being proportional to the text height. For example, the default 50 mil Drill Drawing symbol size yields a 7 mil aperture for stroking the symbols. 60 mil text height yields 8 mils stroke width. Users should take care in defining text sizes for Silkscreen (or Overlay) layers, as very fine strokes may not be successfully screened onto the board.

Automatic aperture file generation

If Advanced PCB is used to automatically generate an aperture table, this should be done after setting all output options and Gerber setup parameters. This is because some options change the aperture use requirments for the file.


Autotrax moire and target pads
Autotrax moiré and target pads

If you load and Autotrax board which has a moiré or target pad then these pads will be converted to free primitives of arcs and tracks. These items will be painted when generating Gerber plots and not be converted back into special moiré or target apertures.


Manual routing improvements

The Auto-Manual Route command has been upgraded significantly for version 2.0. This command now allows the user to re-route previously routed connections as well as routing the un-routed ratsnest connections. Re-routing can only be performed on netlisted connections. (Netlist connections can now be created or changed from inside Advanced PCB. See the Netlist Add Nodes, etc. commands.)

Re-routing is performed by choosing the command (shortcut:   then clicking on any routed track segment. This action "breaks" the attaches a new segment at the cursor location. You can procede to re-route from that point, guided by a ratsnest to the nearest pad in the net. The ratsnest will continuously change to the closest pad in the net as you route. You can either continue to route all the way to the pad, our route back to any track segment in the net. Once the net is re-joined, the obsolete track will be automatically removed.


Loading pad and component librarie
Loading pad and component libraries

When Advanced PCB is started, the library files Advanced PCB.PAD (containing pad descriptions) and PFW.LIB (standard footprint library) are automatically loaded. You can re-name a custom library as PFW.LIB, and this will become the (automatically loaded) default. If you choose to do this, remember to first save the standard library under another name, or it may be overwritten and lost. Library and pad files from previous versions (prior to version 1.5) of Advanced PCB are automatically converted to 32-bit format when loaded and saved in version 2.0.


Array placement
Array placement (Advanced PCB)

Negative Offset values are now permitted. Enter positive or negative numbers in the Place-Array dialog box. Indicate negative numbers by typing - (dash), then the digit, for example: -3.333, etc.


PADS and PCAD files

Opening PADS-PCB and PADS 2000 files

Users may experience problems loading some PADS-PCB files. This is due to ambiguities in the .ASC format that cannot be resolved by Advanced PCB. For example, Advanced PCB cannot translate PADS-PCB files that contain numeric net labels of four or less characters, because there is no inherent identification of these strings as net labels.

PADS-PCB provides the user with many options when generating files in PADS .ASC format. Some of these options may yield a file that is incomplete or otherwise unreadable to Advanced PCB. If you experience difficulty in loading PADS-PCB files, try re-generating the file using the PADS default (include all) output options.

Problems can also occur when PADS 2000 files are imported into PADS-PCB, then re-exported in .ASC format.

Opening PCAD files

Version 2.0 loads PCAD files, using the File-Open command. The translator handles PDIF version 5 and 6 format files. Boards should be 100.000 x 100.000 inches or smaller, to fit within the Advanced PCB workspace. Some limitations may be encountered with (through hole) pad stacks -- as Advanced PCB limits pads to a single description placed on Multi layer. PCAD pads assigned as multi-layer require no special handling. If a pad stack exists, the top layer shape is assigned to the Advanced PCB Multi layer. The PDIF Void primitive is not supported by the current translator.


PCB capabilities
Advanced PCB 2.0 capabilities

Advanced PCB is a complete PCB layout environment with many attractive features for productive design work. You can use Advanced PCB as a stand-alone manual board layout. When combined with a schematic capture package, Advanced PCB becomes the backbone of a fully-automated, end-to-end design system that features a high degree of design automation and integration. However you use Advanced PCB, you'll appreciate its ease-of-use and the high degree of flexibility built into this proven PCB design system.

Advanced PCB generates through-hole and SMD designs of up to sixteen signal layers, plus four mid-layer power planes and four mechanical drawing layers. Board size can be as big as 100 inches (or 254 cm) square. Placement accuracy is to 1/1,000,000 inch (.001 mil or .00025 mm). A metric/imperial grid system allows you to work accurately in both measurement systems and the grid can be "toggled" between metric and imperial modes as you design by pressing Q.

Full support is included for popular netlist formats. Importing a schematic netlist allows you to take full advantage of Advanced PCB's auto component placement, autorouting and design rule checking facilities. Windows 3 features support for many output devices including printers, PostScript  printers and imagesetters, and pen plotters. PCB also includes Gerber plot and Excellon  NC drill file capabilities.


Windows applications
Advanced PCB compared to other Windows applications

The way Advanced PCB uses tools, menu commands and shortcuts will already be familiar to experienced Windows users - such as using combinations of [image] and other keys to execute menu commands.

In short, Advanced PCB looks and runs like other Windows applications - and it's as flexible as you are. However you should be aware that Advanced PCB is different from other Windows "drawing" applications in some of its fundamentals.

A PCB design is a series of layers - layers which correspond to the individual "tools" used to create the board such as the Top and Bottom signal layers or the silkscreen Overlay layer. PCB displays and manages these layers independently and some operations, such as track placement are layer dependent - you must first select the layer, then place the track. PCB print/plot options also reflect this requirement for "layered" design.

PCB design differs from other drawing tasks in its requirement for extreme precision. As a result, PCB is more of a "placing" environment than a freehand "drawing" environment. Another fundamental difference is connectivity - PCB's ability to recognize connections between track segments, tracks and component pads, etc. For example, PCB allows you to move a component without breaking its track-to-pad connections. You will be using connectivity on several levels as you design with PCB.


Keyboard
Mouse and keyboard shortcuts

Advanced PCB supports several mouse and keyboard shortcuts that are used to speed-up or simplify frequently performed operations, commands and options.

For example, pressing [image] [image] allows you to choose a new Pad Type without having to go to the Current menu and choosing the Pad Type command.

Using the [image] button for {BMC ENTER.BMP} and the [image] button for {BMC ESC.BMP} will allow you to perform many operations without using the keyboard.

Some keyboard commands provide the only practical way of performing an operation when you don't wish to move the mouse in the workspace such as setting a new grid or zoom level while moving a selection.

If you double-click on any placed item, the Change dialog box for that item will be opened, allowing you to edit its attributes. Double-clicking can take slightly longer than using the Edit-Change command.

To move an item, hold down [image] click on the item you wish to move. If you wish to delete an item from the printed circuit board then hold down the [image] key and click on the item you wish to delete.

Many shortcuts are part of the standard Windows interface, such as pressing [image] [image] to close the application window. Other "hot keys" have been added that are specific to Advanced PCB.

Some shortcuts that were part of the Protel Autotrax default key macro set have been retained in Advanced PCB, for the convenience of experienced Protel DOS system users.

See also: Hot Keys

Windows allows you to assign operations to specific key combinations by using the Recorder feature. See you Microsoft Windows Users Guide for details.

There are also a number of third party Windows-compatible macro editors available, which allow users to define keystrokes.


Hot Keys
Hot key shortcuts

Key combination	Command or action

Delete menu

Change menu

Jump menu

Move menu

Place menu

Select menu

Toggle Select menu

Autoplace Tools menu

DeSelect menu

Zoom menu

 + [image] or 	Auto menu

 + [image] or 	Current menu

 + 	Edit menu

 + [image] or 	File menu

 + [image] or 	Help menu

 + [image] or 	Info menu

 + [image] or 	Library menu

 + [image] or 	NetList menu

 + [image] or 	Options menu

 + [image] or 	Window menu

 + 	Place-Single Arc By Center command

 + 	Set Snap Grid aize command

 + 	Select-Physical Net command

 + 	Set Current layer command

 + 	Measure distance command

 + 	Set Current-Pad Type command

 + 	Set Current-String Height command

 + 	Set Current-Track Width command

 + 	Undo command

 + 	Set Current-Via Size command

 + 	Zoom-Window command

Help-Index command

 + 	Cascade Windows command

 + 	Tile Windows command

Zoom-Expand command

Zoom-Contract command

 + 	Zoom-In maximum command

 + 	Zoom-All command

Toggle next active Signal layer

Toggle next active layer

Toggle to previous active layer

Zoom-Pan command

Zoom-Redraw command

Toggle imperial/metric measure units

 + 	Jump-Absolute Origin command

 + 	Jump-Relative Origin command

   	Move one Grid point

 +    	Move ten Grid points

 + 	Cut command

 + 	Copy command

+ 	Paste command

 + 	Clear command

Special mode depending shortcuts

Opens Current menu option for item during placement

Aborts screen redraw, cancels current operation

Pans at 5X rate when moving or placing items

Aborts screen redraw, toggles track placement mode, rotates component or pad during placement

, 	Flip or mirror item during move or place

Access Options-Display dialog box while editing

Swap component layer during move or place

Convert polygon perimeter track to arc; toggles arc direction

Convert polygon perimeter arc to track

Places via during Auto-Manual Route command

Places pad during Auto-Manual Route command

Add vertex to polygon perimeter segment

Remove vertex from polygon perimeter

, [image], [image],	Toggles Align Component mode

, [image].

Undo last segment when placing or manually routing tracks

 + [image] + 	Break track at cursor location

 + 	Move primitive at cursor location


Reference

Keyboard

Messages

Special files

Photoplotter output files


Basic concepts

Advanced PCB design environment

Advanced PCB capabilities

Compared to other Windows applications

System options

Navigating Advanced PCB

Mouse and keyboard shortcuts

Searching for workspace objects

Making selections

Component libraries

Pad types

Design automation

Printing and plotting artwork


Design environment

PCB layers

Metric and imperial units

PCB primitives


System options

Changing system defaults

Setting user preferences

Assigning display colors

Using the grid system


Introduction to grids

Advanced PCB supports two different grids which work completely independently of one another. The first is the snap grid and the second is the visible grid. Both grids can be set using through the Options menu. Both grids are relative to some point (the current origin), and can have a value between 1 and 1000 mil.

See also:	The Snap Grid

The Visible Grid


Snap Grid

The snap grid is an array of points on the screen to which cursor movement is restricted. Whenever the cursor keys or the mouse are used to move the cursor around the screen the cursor follows (snaps) from one grid position to the next. For example, setting the snap grid to 100 mils will mean the cursor can only be on points, 0.0 inch 0.1 inch 0.2 inch etc. If you are using the cursor keys to move the cursor, you will find that Choosing [image] and a cursor key makes the cursor jump move 10 times the current setting of the snap grid. To view fractional coordinates, use a snap grid value less then 1 mil. For example, setting a snap grid of .05mil will display: 23.00mil, 23.05mil, 23.10mil, etc. on the Status line.

This grid also controls the default display of measurements. If it is set to Imperial then measurements will be display as mils (.001 inch). If it is Metric then measurements will be display as metric.

Shortcut: Press Q to toggle between imperial (mils) and metric (mm) units.

See also:	Metric and imperial units

Current-Snap Grid


About the visible grid system

This is a system of lines (or dots) displayed in the workspace and used for alignment of placed primitives.

The visible grids are tools to assist in accurate placement and alignment. On the Options-Layers dialogue box, there are two separate Colors for these grids. If the grid lines will be closer than 5 pixels apart on the screen, then these grids will not be displayed. Dots can be substituted for solid lines for these grids from the Options-Preferences command.

See also:	Metric and imperial

Current-Visible Grid 1

Current-Visible Grid 2


Automatic Tools
Design automation features

The level of design automation features available in Advanced PCB depends upon the options that have been purchased. Users of the basic 32-bit version will not have access to some of the automation tools displayed in menus or dialog boxes. Purchasers of the full Advanced PCB system gain access to features like Gerber-Batch Load, array placement, global editing, local auto placement and the Line Probe autorouter. Advanced Place, Advanced Route and Advanced SB Route are additonal options that further extend the Advaned PCB feature set. If you have questions about the options available, please contact your Protel representative.

Array placement

Global editing

Netlists

Auto placement

Autorouting


Output

Printing and plotting

Photoplotting

NC drilling


Autorouting

Note: 	The level of autorouting available in Advanced PCB depends upon the license: in the basic Advanced PCB package (formerly Professional PCB), no router is available; in the full Advanced PCB version, a Line Probe router is provided; if you have purchased the Advanced Route option, the Maze (Rip-up/Retry) router is available; purchasers of Advanced SB Route receive a gridless, shape-based routing system for high-density, SMD or mixed technololgy layouts.

The process of converting a "from-to" connection to a collection of tracks and vias that from an electrical connection, is referred to as routing. When this process is performed automatically by a computer program, it is referred to autorouting.

Advanced PCB contains a collection of autorouters which can be run separately or together, to perform this task. The successful use of autorouters is dependent on a number of different parameters. The quality of the component placement, the density of the PCB, the number of copper layers that can be used, not to mention the aesthetic requirements of individual designer. A basic introduction to autorouting technology will help you to get the most from the autorouter in Advanced PCB.

See also:

To learn more about general autorouting topics:

Judging autorouters

Layer bias

Autorouter types

Protel autorouter

Autorouter setup

Autorouting models

To learn more about specific autorouter commands:

Auto Route-All

Auto Route-Net

Auto Route-Connection

Auto Route-On Component

Auto Route-Selected Components

Auto Route-Pad to Pad

Auto Route-Advanced Route Connections


Judging autorouters

The success of an autorouter, is usually judged primarily by the percentage of the board that it can autoroute. As a designer you have to consider a number of other success measurements, depending on the design problem. If the board is a standard digital board with two signal layers, to be manufactured as a plated through board, then completion percentage may be your only requirement. If the board is mainly analog, RF, or power supply, then completion percentage may not be as important as 'star pointing', connection lengths, shielding etc.

For mixed analog and digital boards, you should consider manually routing the analog section, using the powerful editing tools in Advanced PCB, and then autorouting the remaining digital sections.

For digital boards that have large and complex bussing structures, consider manually routing the bussing on one or two layers, and then autorouting the remaining random logic. If the board has high speed ECL circuits, then the trace length and termination requirements will put it beyond the reach of standard autorouters. Power supply and power control boards, particularly those that use switching technology, need attention to star pointing and overall track shape, length and width.

Adding extra layers will allow greater component densities. Hand routing buses and other difficult connections will allow successful routing on much high density boards.


Layer Biasing
Layer bias

Multilayer board manufacturing technology enables you to route connections across two or more layers, separated by a dielectric (usually fiberglass).

Placing parallel tracks on adjacent layers will result in an increased capacitance between the layers, and will block track placement in the opposite direction across the board.

In Advanced PCB, each layer can be set as horizontal, vertical, both (for single layer routing) or turned off altogether.

For this reason, layer biasing is commonly used in designing boards with two or more layers. That is, placing predominantly vertical tracks on one layer, horizontal on the next, vertical on the next and so on. This does not mean that routing is restricted entirely to this direction, but rather, that the majority of tracks on a given layer will travel in the same direction.


Autorouter types

Basic classes of gridded routers

There are two main classes of autorouter, those that work through the board, one connection at a time until finished, and those that, after finishing, modify the design in some way, to get the failed connections in, repeating this process as many times as possible until the board is routed. These "iterative routers" (sometimes referred to as "100% routers") fall into two main sections, "rip-up" and "shove aside".

Within both classes of router, there are a number of different techniques used to actually find a path between two points on a partially routed board.

Gridless routers

A distinct third class of routers includes so-called gridless or shape-based routers. This type of router uses board primitive (track, pad, etc.) geometry to describe the board, rather than a series of cartesian coordinates which are either occupied or unoccupied. Gridded routers fail when the routing grid becomes too fine, because memory requirements grow exponentially. Because gridless routers do not have to build an internal map of the routing grid, they can perform more complex routing solutions using less memory. This makes gridless routers the preferred solution for surface mount or mixed technology layouts.

See also:	Pattern routers

Line Probe routers

Wave Expansion routers

Shape-based routers


Pattern routers

Sometimes referred to as heuristic routers look for a known commonly occurring pattern of pins, and try to [image] a standard pattern of tracks and vias to complete the connection. For example, memory bussing is a common pattern, usually solved with the characteristic wave pattern. Simple L patterns, formed from a horizontal and vertical track segment (one on each layer) connected by a via, is another common pattern.

Pattern routers are usually very fast, produce very high quality routes, but will only get a small percentage of all but the most simple boards. For these reasons, pattern routers are usually run first, to pick up the easy connections, and provide a high quality solution to them.


Line Probe routers

These routers move a test track from both ends of a connection until an obstacle is encountered. They move sideways until the obstacle is not there and then continue on there way. When they meet, the connection is complete. There is usually a limit to how far sideways they can go. Line probe routers are reasonably fast and provide high quality routes with low via counts, but suffer from a major problem. They are prone to run into blind alleys and fail to solve what would appear to be very simple problems, and as a result, they tend to slow down and fail as the board gets fuller. This is because they are not evaluating all possibility, but simply following the best one.

When combined with a heuristically guided route shape, such as a Z shaped route (two vias, two verticals an one horizontal track etc.) they can provide very high quality solutions to fairly difficult routing problems.


Wave Expansion routers

Commonly referred to as "flood", "maze" or "Lee" routers. These routers use an exhaustive search to find a solution to a connection if one exists. The flooding process is a metaphor for pouring water from one end of the proposed connection, over the board, where all free spaces are considered as channels for the water, and all obstacles are considered as islands. The water will spread out in all directions until, eventually, if at all possible, the water will get to the other end of the connection. This type of router can be enhanced in a number of ways.

The quality of the route can be enhanced by setting a cost for changes in direction, swapping layers and moving in the wrong biasing direction. The final solution will then be a balance of these parameters, controlled by the size of the various costs. Expanding points on the wave front that are closer to the target and in the same direction as the target, before others, will speed up the search.

There are two basic kinds of wave router, gridded and gridless.

In the grid type, each point of space on the board is represented as a point in a two dimensional array, either filled or empty. The problem here is that the memory requirements go up as the square of the grid resolution.

In the gridless type of wave router, the expansion is performed by expanding the current point as rectangle that fits over the current point and goes in all directions until obstacles are hit. When an obstacle is hit, the intersection of the obstacle and the rectangle is calculated and another rectangle is expanded from the free section of the edge of rectangle. This is very processor intensive, but completely grid independent due to the polygon calculations (as opposed to point calculations).

Although tremendously powerful and flexible, generally, all wave type routers are slow and memory hungry.


Protel autorouter

The Advanced PCB autorouter is a multi-algorithm router. It works with up to 16 signal layers plus power and ground planes with grid sizes of 5-100 mil. The passes include various pattern, line probe and a maze router. You can control all clearances (air gaps) and, track and via sizes. You can specify which passes are used and what layers and directions are used for tracks. The autorouter passes are:

Pre-router

SMT Stringers

Memory router

Pattern routers

Line Probe router

Maze router

Smoothing passes

Mitre/Add arcs pass


Autorouter Pre-Router
Pre-Router pass

If you place some items on the board to complete connections (pre-routing) then set this pass on. It will check all the connections and make sure that the router will only attempt to route the unrouted ones. If you have used the Auto-Manual Route option to complete some connections, then this option is not needed for those connections.


Autorouter SMT Stringers
SMT Stringers pass

If you are using power and ground planes with SMT components, use this option to route those pins that need to connected to the planes (with a short track segment and a thermal relieved pad).


Autorouter Memory Router
Memory router

This is a very fast heuristic pattern router to put in the classic wave structure for memory busses.


Autorouter Pattern Routers
Pattern router

These are very fast simple pattern routers which allow zero, one or two vias, and up to three track segments. They will stick rigidly to the layer biasing rules and will never travel in the "other" direction on any given layer.


Autorouter Line Probe
Line Probe router

These are combination line probe and pattern routers. They use a basic L, C or Z shape, with the separate sections completed by a line probe router.


Autorouter Maze Router
Maze router

This is a gridded wave expansion router. This pass is used after all the others have failed. It copies a description of the board into a cell map and then attempts to route un-routed connections. The amount of memory required by this router is determined by the board size and layers. Basically, one byte for each layer at each grid point, plus, if hugging is on, one byte for each layer at each grid point. For example, on a 25 mil grid, a 4 inch x 5 inch board with 4 signal layers, will require 4 x 5 x 40 (point per inch) x 40 x 4 (layers) = 64000 bytes, or 128K if hugging is turned on.


Autorouter Smoothing
Maze router Smoothing passes

After all routing is completed, this pass checks the board for vias that can be removed by swapping tracks from one side of the board to the other, and resolves loops into direct connections by using copper sharing. Smoothing can result in very significant improvements to the router result, but completion can take a fair amount of time. If multiple smoothing passes are enabled, each pass will run with increasing thoroughness as the cost for undesirable conditions (e.g. extra via, etc.) increases with each subsequent pass. For this reason, it is preferable to enable one smoothing pass, rather than to set the smoother for five passes, then stop it at one pass. Smoothing should be normally be disabled until the board is routed (either automatically or manually) to 100% completion. It is also possible to apply Hugging or Spreading when smoothing.


Autorouter Add arcs
Maze router Mitre/Add Arcs pass

If you wish to use 45 degree mitres or curved tracks, then enable this Advanced Route clean-up pass. It will attempt to replace corners on tracks with mitres or arcs. Normally, you should use this pass only after finishing board routing. This makes it easy to discard the result, set new maximum and minimum radii and re-run the clean-up routine, if you are not satisfied with the initial results.

See also: Router performance.


Autorouter setup

All the values described below should be set after consultation with your board manufacturer to make sure he can work to the tolerances you require.

Autorouter grid size

Autorouter track width

Autorouter via size.

Clearances


Autorouter grid size

The autorouter grid can be different from the snap grid. All tracks, vias or arcs placed by the autorouter, will be on this grid. It can have any value from 5 to 100 mils. For all the routing passes, decreasing the grid size will slow the program down. For the maze router, the memory requirements, for storing the grid model of the board, go up as a square of the grid resolution, so a 25 mil grid will use four times as much memory to model the board, as 50 mil grid. Making the grid smaller will. You should make sure that most of your pads are on the currently set router grid. Use the command Netlist-Router Off Grid to highlight any off grid pads. Use the command Netlist-Auto place Move to grid to move components to the nearest grid point. Autorouter speed improves when the routing grid is greater than (or equal to) the track width + router clearance. For example, when routing 8 mil tracks with 6 mil clearances (yields a total clearance or air gap of 12 mils), a routing grid of at least 20 mils will improve speed.


Autorouter track width

This is the width of any tracks, straight or curved, put in by the autorouter. Enter any value from 1 to 255 mils. This value should be set in conjunction with the grid size and clearances to allow successful routing.


Autorouter via size

The diameter of any vias place by the autorouter. Enter any value from 1 to 255.000 mils


Autorouting models

To get the most from the router, you must select a combination of clearances, track size, via size and routing grid that will allow the router to work. Note: the fractional grids referenced in the Manual are now supported in version 2.0.

The following fractional values are available. If you enter another value, the grid will be rounded to the nearest of these settings: x.75, x.67, x.50, x.33, x.25. These restrictions keep the memory requirements reasonable, while providing additional flexibility in routing. Use the following examples as guidelines for autorouting design rules. See page 182 of the User Guide for additional models.

See also:	Single Density 100

Single Density SMT 50

Double Density SMT 50


Single Density 100 mil pad centers

Track size	12 mil

Via size	50 mil  (or 62 mil if you like)

Clearances	12 mil

Grid size	25 mil

To use this model, the majority of your pads should be 62 mil or less in diameter. This will enable a single track, maintaining clearances, to pass between two pads 100 mil apart.


Single Density Routing (SMT 50 mil pad centers)
Single Density SMT 50 mil pad centers

Track size	8 mil

Via size	40 mil

Clearances	8 mil

Grid size	25 mil

To use this model, the majority of your pads should be 26 mil or less wide (in one axis), to leave a gap of 24 mils between pads. This will enable one track, maintaining clearances, to pass between a pair of pads 50 mil apart. The via size can be varied as required.

Check with you board manufacturer before giving him this board to make. This a fairly standard SMT board.


Double Density SMT 50 mil pad centers

Track size	6 mil

Via size	26 mil

Clearances	4 mil

Grid size	10 mil

To use this model, the majority of your pads should be 24 mil or less wide (in one axis), to leave a gap of 26 mils between pads. This will enable two 5 mil tracks, maintaining clearances, to pass between a pair of pads 50 mil apart. The via size can be varied as required.

Check with you board manufacturer before giving him this board to make. This is a very demanding level of technology.


PCB Layers

Copper trace layers

Silkscreen overlays

SMT Paste Mask layers

Solder Mask layers

Post-processed Power Plane layers

Keep Out layer

Mechanical layers

Drill Drawing layer

Drill Guide layer


Copper trace layers

There are 16 layers for track routing. Anything placed on these layers will appear as copper on the final PCB.

Top Layer 	Sometimes referred to as the component side of the PCB. For boards with components on one side only, this is the side for component placement.

Bottom Layer	In conventional through hole boards this is referred to as the solder side.

Mid Layers  1 to 14	These are only used for track routing in multilayer boards.


Silkscreen overlays

Two Overlay layers are provided (Top and Bottom). These layers are used to display and print/plot component outlines and component text strings (Designator or label and Comment).


SMT Paste Mask layers

Two Paste Mask layers are provided (Top and Bottom). These tools provide a photo mask or silkscreen mask of solder paste locations. Used in the manufacture of boards with surface mount devices.


Solder Mask layers

Two Solder Mask layers are provided (Top and Bottom) for photo mask or silkscreen solder mask. This tool is used to apply a mask for wave soldering (usually only on components).

Solder Mask layers are auto generated during plotting. Users can customize these layers by placing tracks or fills directly on these layers from the editor. Any primitive placed on a Mask layer will be plotted in the reverse. In other words, placing a fill creates a hole in the solid mask.


Post Processed Power Planes
Post-processed Power Plane layers

Up to four (4) special midlayer planes can be specified. These planes are auto-generated during printing and plotting, using the Power Plane attribute of through hole pads is used to generate these layers.

Tracks, arcs, fills, etc. can be placed on power plane layers, but they are displayed and plotted as negatives, so any placed primitive becomes a break (or void) in the solid copper area when artwork is crated. Entities placed on these planes can be viewed and edited directly in Advanced PCB. The layer must be turned "on" (Options-Display) and the layer must be assigned a color other than the background.

Split planes can be created by placing polygons on internal plane layers, with full preservation of net integrity and DRC functions.


Keep Out layer

Specify multilayer keep outs.

The Keep Out layer is used to define the physical limits for both automatic component placement and autorouting.

This is achieved by placing a rectangular perimeter of tracks or by placing (solid) area fills to define any "no-go" areas. No-go areas must be defined with fills, not tracks. If the board shape is non-rectangular, first define its outer dimensions with a perimeter of tracks, then use fills to define the shape of the board, inside the perimeter.


Mechanical layers

Four reference special layers are provided for design documentation. These layers are typically used to place dimensions and instructions for fabrication and assembly of the board. The Print, Pen Plot and Gerber commands support plotting of mechanical layer data in combination with other layers.


Drill Drawing layer

The Drill Drawing is a reference plot, used as an aid in setting up and programming NC Drill equipment. The plot includes graphical symbols that identify each hole by size, tool assignment and location.


Drill Guide layer

The Drill hole guide is a plot of all the holes in your design. The plot includes all multi-layer pads and vias. You can specify a guide hole, which locates the hole center, from Output Options dialog box)


Metric and imperial units

Resolution: The metric resolution of the program is 0.0000254 mm.

All measurements can be entered in metric or imperial. To enter in imperial (mils or 0.001 inch units) just type the number. Fractional values to .001 mil are allowed. To enter in metric, type the number in millimeters with the unit designator mm (e.g. 0.10mm). Most measurement entry menus have both metric and imperial selections or you can select the "other" option and enter any value. To toggle the current unit of measure between imperial and metric press the Q key.


PCB Primitives

Arcs

Tracks

Vias

Pads

Fills

Text strings

Components


Arcs

Arcs are essentially circular curved tracks. They can be placed on any layer with any radius and any line width from .001 to 1000.000 mils wide. The angular resolution is .001 degree. The number of arcs is limited by memory only. Arcs can be placed using the place arc commands or as tracks using the place track command.


Tracks

Tracks can be placed on any layer with any width from .001 to 999.999 mils wide. The number of tracks is limited by memory only. Tracks can be placed using the place track command or by the autorouter.


Vias

Vias are always multi layer and can be any diameter from 1 to 500.000 mils wide. The number of vias is limited by memory only. Vias can be placed using the place vias command  or by the autorouter. The hole size of vias can be set from 1 to 500.000 mil.


Pads

Pads can be rectangular, rounded or octagonal with Y and Y size specified. Circular is rounded with the same X and Y value.

Pads can be place on any layer or made multi layer in which case they are copper on all layers.

Sizes can be from 1 to 500.000 mils on both axis with the hole size from 1 (SMT) to 500.000 mils. Pads which are to be used in components can be identified with a 4 character designator.

When a pad is first placed, its designator is empty. If the pad is to remain as a free pad, then leave it like this. If the Pad is to be a mounting hole, then leaving its designator as empty allows the DRC to ignore it (i.e. not report it as an empty pad).


Fills

Rectangular fills are simply rectangular areas of any size on any layer, representing solid copper areas of the manufactured board. Fills are also placed inside the Keep Out layer perimeter -- to define no go areas for both auto placement and autorouting. On Power Plane, Paste Mask and Solder Mask layers, fills are placed to define voids (or empty areas) in the artwork -- as these layers are plotted as negative (or reversed) artwork.


Text strings

Text strings can be placed on any layer with any height and can be any one of system Fonts. The number of text strings is limited by memory only. Strings can placed using the place string command.


Fonts

The Advanced PCB system is delivered with three fonts that are specially designed to support vector plotting, including both pen plotters and Gerber plots: Default (plain); San Serif and Serif. Fonts for Free String placement are selected from the Current-Free Text Font command. Component text fonts are selected from the Current-Component Text dialog boxes.

All fonts, being line vector fonts can be plotted and photoplotted and will appear the same as on the screen. All fonts have the full IBM extended ASCII character set that supports European languages other than English.

The default font supplied with the system is built into the software and cannot be unloaded). To load or unload fonts use the Library-Fonts command.

The size of the text is controlled from the Current-Free Text Height command and Current-Component Text dialog boxes. Height can be set in either mils (.001 in) or in millimeters. Text can be placed on any layer. Once placed, Free Text strings can be moved or edited like other primitives. Component text can be moved independently of the component (Move-String command). If the component is moved, component text will move relative its current position.

Strings from converted Autotrax files will be converted to the Default font.

When performing a Design Rule Check, checks are made for collisions with text strings. The size of the string is calculated using the default font, even if the some other font is used in the string. This only affects the length of the string as the user controls the height and this is independent of the font.


Components

Components consist of any number of the above items to any size grouped together. Both through-hole and SMT components can be placed on either side of the board.

The number of components is limited by memory only.

The component designator can be up to 12 characters and can be placed anywhere relative to the component on either copper or overlay. The comment field, which is used to store the type or value of the component can be up to 32 characters and can be placed anywhere relative to the component on either copper or overlay. Both comment and designator can be hidden from view and set to any size and font.


Netlists

Netlists Defined

A net, in electronic design, is a collection of component pins (nodes on the net) which are electrically connected. For example, all the pins connect to +5v on a PCB are connected together and hence constitute a net. (The term "net" is shortened from "network", but is now standard). Each net is given a name (+5v , VCC or GND for example) . A netlist is the collection of nets that define all the electrical connections in a design. A netlist file is the list of nets (the netlist) stored in a disk file.

Advanced PCB Nets

Each net has a name (up to 20 characters long) and each node consists of a component designator and a pad designator, separated by a hyphen. For example U23-16 refers to pin 16 on component U23.

Loading	After a netlist has been loaded to a PCB, the program converts each net to a series of logical connections. These connections are simply two of the nodes from the net and have no physical existence. This process is referred to as "optimizing" and the basic idea of this is to produce the series of connections that will complete the net with the shortest track length. The display of all the connections is referred to as a rats nest).

When a connection is converted to tracks and vias (i.e. when it is routed), then logical connection is no longer displayed. When all the connections in a net are routed, then all the nodes in the net will be physically connected together. When all the nets are routed, the PCB design is complete.

See also:	Netlist Commands


Optimize Methods

Optimization is a process for re-ordering the connections within a net. The order of connections after optimization is a function of the optimization method applied, the order of nodes in the netlist file and the physical location of any nodes (i.e. component placement) after components are loaded. Optimization is performed whenever a netlist is loaded. Once a netlist is loaded, optimization can be applied to any individual nets or groups of nets.

Use the Edit-Net command to assign a new optimization method to a single net. You can also define the Source Node and Terminal Node within a net. These are used to identify the starting and ending nodes within a net, regardless of the optimization method. For example, the Source Node will be the center (or hub) in a Star Point  topology.

Use the Netlist-Optimize commands to optimize nets.

The list of optimization methods will appear. The  options are

Shortest	This simply looks for the set of connections (with any topology) that connects all the nodes together.

X Bias	Looks for the set of connections (with any topology) that connects all the nodes together. The program will prefer horizontal shortness five times more than vertical shortness. Use this to force routing strictly in the horizontal direction.

Y Bias	Looks for the set of connections (with any topology) that connects all the nodes together. The program will prefer vertical shortness five times more than horizontal shortness. Use this to force routing strictly in the vertical direction.

Daisy Chain	This uses the order of the nodes in the net from the netlist file and connects them as one wire with the nodes strung along it. They will appear in the connection list in exactly the same order as the order of the nodes in the original netlist file. Each node will have two connections to it, except the first and last which will have only one. No minimization is performed. This option may be used for highly critical ECL designs.

Minimum Daisy Chain	Using this method, the nodes in the net will appear as nodes strung along one wire which threads its way around the board. Each node will have two connections to it, except the first and last which will have only one. Minimization is performed, within the limits of the daisy chain topology, to reduce the total connection length.

Start End Daisy Chain	Using this method, the connections in the net will appear as nodes strung along one wire which threads around the board. Each node will have two connections, except the first and last connection, which will have a single connection. Minization is performed within this topology to reduce the total connection length. The first and last nodes in the net (from the order of nodes in the original netlist) will be the two end nodes in the daisy chain. Use this option for nets which have termination components on the ends of the nets, as in high speed circuits.

Star Point	This method orders connections into a star configuration, with minization of each node radiating from the central node.


Command Reference

File

Edit

Library

Netlist

Auto

Current

Options

Zoom

Info

Window

Help


Gerber menu

Gerber In

Batch Load

Gerber Output


Reports menu

Bill of Material

Board Specifications

Netlist Status

Pick and Place


File menu

New

Open

Close

Restore Backup

Save

Save As

Save All

Shape Based Router

Output Options

Gerber

Print

Pen Plot

NC Drill

DXF

Export Selection

Reports

ReAnnotate

Run Schematic Capture

Exit


Select menu

Inside Area

Outside Area

All

Free Prims

All on Layer

Physical Net

Physical Connection

Hole Size

Off Grid Pads


De-Select menu

Inside Area

Outside Area

All

Free Prims

All on Layer


Toggle menu
Toggle Selection menu

Arcs

Components

Fills

Pads

Polygons

Strings

Tracks

Vias

See also:	Toggling the selection


Delete menu

Arc

Component

Fill

Pad

Polygon

String

Track

Via


Change menu

Arc

Component

Fill

Pad

String

Track

Via

Repour Polygon

Edit Polygon Vertices

Convert Selection to Fills

Convert Selected Vias to Pads

See also:

Making Changes


Move menu

Move-Selection

Flip Selection

Rotate Selection

Break Track

Drag End

Whole Track

Re-Route

Arc

Component

Fill

Pad

Polygon

String

Via


Place menu

Arc (Center)

Arc (Edge)

Component

Fill

Pad

String

Track

Via

Polygon Plane

Outline Selected Items

Coordinate

Dimension

Array


Jump menu

Absolute Origin

Current-Origin

New Location

Component

Net

Pad

String

Design Rule Violation


Edit menu

Undo

Redo

Cut

Copy

Paste

Clear

Select

De-Select

Toggle Selection

Delete

Change

Move

Place

Jump

Set Origin

Reset Origin

Cross Probe Part On Schematic

Cross Probe Pin On Schematic

Cross Probe Net On Schematic


Library menu

Components

Un-Group

Pad Types

Apertures


Optimize menu

Net

On Component

All


Show Connections menu

Net

On Component

All


Hide Connections menu

Connection

Net

On Component

All


Netlist menu

Load

Clear

Optimize

Show Connections

Hide Connections

Edit-Net

Identify

Length

Add Nodes

Add/Modify Connections

Delete Nodes

Delete Connections

Add Nets

Export

Run ECO File

Generate

Design Rule Check

Clearance Check

Reset DRC Error Markers

Clearances

Power Planes

Compare


Autoroute menu

All

Net

Connection

On Component

Selected Components

Pad to Pad

Advanced Route Connections


Un-Route menu

All

Net

Connection

Track

On Component

Selected Components


Auto menu

Auto Place

Placement Tools

Move to Grid

Density

Manual Route

Auto Route

Setup Auto Route

Un-Route


Current menu

Pad Type

Track

Via Diameter

Via Hole Diameter

Via Type

Component Text-Comments

Component Text-Designators

Free Text Height

Free Text Font

Snap Grid

Visible Grid 1

Visible Grid 2

Layer


Track Mode menu

Any Angle

90/90 Line

45/90 Line

90 Arc/Line


Options menu

Layers

Preferences

Display

Track Mode

Tool Bar

Status

Scroll Bars

Toggle Units

Memory Monitor


Zoom menu

Window

Point

Select

All

In

Out

Pan

Redraw


Info Power Planes menu

Plane 1

Plane 2

Plane 3

Plane 4


Info menu

System Status

Board Status

Components On PCB

Selected Pins

Nets

Measure Distance

Length of Selection

Power Planes


Window menu

Tile

Cascade

Arrange Icons

Close All


Help menu

Index

Using Help

Basic Concepts

Commands

Printing

Managing Files

Screen Regions

Reference

About


File New

Shortcut keys:

Summary:	Displays a new document window with the title "PCB_#".

Procedure:	Choose File-New. A new document window becomes the current window.


File Open
File-Open

Shortcut keys:

Summary:	This will open a new document window with the contents of the selected file.

Procedure:	Choose File-Open. The file may be of any type supported by Advanced PCB.

When you start PCB, The Load PCB File dialog box is opened. The menu bar displays three options: File, Info and Help. The Tool bar buttons (if displayed) are dimmed. This dialog box will display the current directory and any files that include the extension .PCB which is reserved for Protel PCB workfiles. To open a new (empty) document window:

1.	Type the filename (include the full path, if different from the path listed after Directory;

2.	Click OK to open the files.

You can also double-click on the desired filename in the Files window, if any. To change directories, click under any of the options listed in the Directories window.

The selected file will load into the active PCB document window. This may take a few moments. to draw the PCB layers in the window.

You can abort the drawing (or redraw) of the document window, at any time, by pressing [image]. This allows you to move directly to another menu command or Tool button without waiting for the entire screen redraw to be completed.

See also:	File-Open Dialog Box

File-Save

File-Save As

File-Formats


File Close
File-Close

Shortcut keys:

Summary:	Closes the current document window.

Procedure:	Choose a document window, then choose File-Close. If modifications have been made to the contents of the document window, a message is displayed that prompts to save, discard, or cancel.

See also:	File-Exit

File-Save

File-Save As


File Open dialog box
File-Open dialog box

Open File-Name	Type a PCB file name or select a name from the Files box. Select the name of the PCB Window. This box lists files with .PCB extensions.

Directories	Select the drive and directory where the PCB Window is stored. Choose OK to see a list of PCB Windows in the selected directory that have the extension specified in the Open File Name box. Default is current drive and directory.

See also:	File-Open

File-Save

File-Save As

File Formats


File Restore
File-Restore Backup

Shortcut keys:

Summary:	Overwrites the current board window with the last created autobackup version of the file (if any). Auto backups are labeled: <filename>.AB0, .AB1, etc up to .AB9, then back through .AB0, .AB1, again. Restore Backup uses the creation date for the autobackup file, not the numeric extension, to determine the restored version.

Procedure:	Select a document window, then choose File-Restore Backup.

Warning:	You cannot Undo this command. This command will overwrite the current window contents with the backup version. Make sure that you save the file with a new name if you wish to recover the data later.


File Save
File-Save

Shortcut keys:

Summary:	Saves the contents of the current document window in Protel Binary format using the existing path and filename.

Procedure:	Select a document window, then choose File-Save.

See also:	Save As Dialog Box

File-Save As


File Save As;Save As
File-Save As

Shortcut keys:

Summary:	Save the contents of the current document window to a new path, filename, and file format.

Procedure:	Select a document window, then choose File-Save As.

See also:	File-Open

File-Save

File Formats


Save As dialog box
File-Save As dialog box

Save File Name	Type a new file name to save in a different file or leave the current name to save with the same name.

Directories	Select the disk drive and directory where you want the PCB Window stored. Default is current drive and directory.

See also:	File-Open

File-Save

File Formats


File Save All
File-Save All

Shortcut keys:

Summary:	Saves the contents of all the document windows to the Protel Binary file format using the existing paths and filenames.

Procedure:	Choose File-Save All.

See also:	File-Save

File-Save As

File Formats


File Shape
File-Shape Based Router

Shortcut keys:

Summary:	Used to export design files and .DO files to Advanced SB Route, import SB Route files (.RTE) files back into Advanced PCB and run the Advanced SB Route application (or the Specctra SP-10 router) from inside Advanced PCB.

Procedure:	Choose File-Shape Based Router, then choose Export Design, Import Routes or Run.

See also:	Setup Auto Route


Output Options
File-Output Options

Shortcut keys:

Summary:	Used to setup output options for printing or plotting (including Gerber plot files). Settings in the Output Options dialog box effect the display of Power Plane layers, Paste Mask layers and Solder Mask layers. For example, enlargements applied these layers will be displayed when the layers are visible (Options-Layers command).

Procedure:	Choose File-Output Options. Assign the desired attributes in the dialog box, then click OK. Changes will be reflected, where applicable, in the display and in any arwork generated.


Gerber In

Shortcut keys:

Summary:	Loads a Gerber file into the current document window. During loading, flashes are converted to free pads and lines are converted to free tracks.

Note:	Leave the Center Plots on Film option disabled (default is enabled) to superimpose the Gerber layer(s) directly over the (previously opened) PCB file.

Gerber Formats

Advanced PCB loads files in 2:3 (nn.nnn) 2:4 and 2:5 numeric formats. When there is no file header, the system will assume 2:3. If the format is 2:4 or 2:5, a file header must be present.  A typical format statement looks like:

*%FSLX24Y24%*

Format statements can be more complicated, but this is all Advanced PCB requires in order to interpret the Gerber file. The syntax is:

*%..%* 	delimits the statement as a comment

FS	labels a format statement

L	Indicates that leading zeroes are suppressed

Xnm	specifies numeric format for the X coords

Ynm	specifiesnumeric format for the Y coords (nearly always same as X)

See also:	Gerber-Batch Load

Library-Apertures


Gerber Batch Load
Gerber-Batch Load

Shortcut keys:

Summary:	Loads all Gerber files that match the filename into the current document window. During loading, flashes are converted to free pads and lines are converted to free tracks. Each file will automatically be assigned to a layer determined by its file extension (see filename conventions)

Procedure:	Select a document window. Open an aperture table using the Library-Apertures

Choose File-Gerber-Batch Load,

During the Gerber loading process, lines will be converted to free tracks and flashes converted to free pads.

Note:	Leave the Center Plots on Film option disabled (default is enabled) to superimpose the Gerber layer(s) directly over the (previously opened) PCB file.

Gerber Formats

Advanced PCB loads files in 2:3 (nn.nnn) 2:4 and 2:5 numeric formats. When there is no file header, the system will assume 2:3. If the format is 2:4 or 2:5, a file header must be present.  A typical format statement looks like:

*%FSLX24Y24%*

Format statements can be more complicated, but this is all Advanced PCB requires in order to interpret the Gerber file. The syntax is:

*%..%* 	delimits the statement as a comment

FS	labels a format statement

L	Indicates that leading zeroes are suppressed

Xnm	specifies numeric format for the X coords

Ynm	specifiesnumeric format for the Y coords (nearly always same as X)

See also:	Gerber In

Library-Apertures


Gerber Output

Shortcut keys:

Summary:	Generates Gerber files from the current document window. Gerber files can be single layer or composite, automatic panelization and batch plotting are supported. All layers and primitives that are displayed will be plotted. Output in the following formats is supported: 2:3, 2:4 and 2:5.

Procedure:	Choose the File-Gerber-Gerber Output command and select the appropriate options in the Photoplotter and Output Options for Final Artwork Plots dialog boxes. Draft mode is not supported during photoplotting. You have the option of using a pre-defined aperture table (appropriate for vector-type plotters) or allowing the system to generate an aperture table automatically, based on the primitives in the current PCB document.

Note:	An option in the Photoplotter setup dialog box allows the user to Center Plots on Film. Users should be aware that choosing this option does not change the N/C drill coordinates for the file. If N/C drill file and plot file coordinates must match, do not choose this option. If you do not choose this option, Gerber-In will superimpose the Gerber layer(s) directly over the (open) PCB file.

See also:	Options-Layers

Options-Display

Library-Apertures


File Plot/Print
File-Print

Shortcut keys:

Summary:	Generate Printer (or raster pen plotter) output. Draft outline and final quality modes are supported.

Procedure:	Choose File-Print-Composite (multiple layer) or Final Artwork commands. Each command provides access to the appropriate Setup dialog box to determine the contents of the output. After these settings are complete click the Print button.

See also:	File-Plot command

Printing


File Plot
File-Plot

Shortcut keys:

Summary:	Generate Pen plotter (vector) output for HP-GL (Hewlett Packard) or DM-PL (Houston Instruments) or compatible devices. Draft outline and final quality modes are supported. Multiple pen support allows you to assign individual pens to each plot layer, when producing composite check plots.

Procedure:	Choose File-Plot-Composite (multiple layer) or Final Artwork commands. Each command provides access to the appropriate Setup dialog box to determine the contents of the output. After these settings are complete click the Plot button.

See also:	File-Print command

Printing

 	About Version 2.0


File NC Drill
File-NC Drill

Shortcut keys:

Summary:	Generates binary and ASCII NC Drill files.

Procedure:	Choose a document window, then choose File-NC Drill.

See also:	Introduction to NC-Drilling

Generating NC Drill files


File DXF
File-DXF

Shortcut keys:

Summary:	Generates a DXF format file.

Procedure:	Choose a document window and use Edit-Select. A composite of all board layers is generated as a .DXF (AutoCAD) file. Tracks will be rendered in individual polyline segments.


File ReAnnotate
File-Re-Annotate

Summary:	Updates all component designators (labels), based upon their physical position in the PCB. Generates a <filename>.WAS text file, used to back-annotate the source schematic sheet file (Protel Advanced Schematic).

Procedure:	Choose a document window and the File-Re-Annotate command. Three options are available: X then Y, Y then X, Name from Position. Choose the desired method, then click OK.

See also:	About Version 2.0


File Run_Schematic
File-Run Schematic

Shortcut keys:

Summary:	Launches Advanced PCB Advanced Schematic application.

Procedure:	Choose File-Run Schematic. If the Advanced Schematic executable (.EXE file) is in the current PATH statement (AUTOEXEC.BAT file), the application will be launched.

See also:	Your DOS and Windows user documentation for information about the PATH statement.


Export Selection

Shortcut keys:

Summary:	Generate a Protel format .PCB file containing the current selection.

Procedure:	First choose a document window and use Edit-Select and Edit-De-Select to select the primitives and components to include in the file.

When you use this option you are creating a binary file which can be opened in a new Protel document window at any time. This provides a convenient way to store modular design elements for future use. You can use the Copy and Paste commands to import these files into any other PCB document. To use this feature:

1.	Make sure that  the current selection includes only those items you wish to save;

2.	Choose File-Export Selection

This command opens the Export Selection File Name dialog box.

3.	Type a filename for the selection at the prompt;

You can include a new path in the file name or change the directory by clicking in the Directories box.

4.	Click OK.

The file will be generated. This may take a few moments if the selection is large.

If a netlist is attached to the current file, the netlist information is not attached to the exported selection.

See also:	Edit-Select

Edit-De-Select

Selection


Bill of Materials
Bill Of Material

Shortcut keys:

Summary:	Generates an ASCII parts list file.

Procedure:	Choose File-Reports-Bill of Materials, enter a filename and the bill of materials will be written to the file. The extension will be forced to BOM.

An example of the format used is

Bill of Material for F:\BOARDS\DEMO.PCB

On 10-Nov-1991 at 17:44:01

Comment	Pattern	Quantity	Components

--------------------------------------------------------------------------------------------

0.1uF	RAD0.2	7	C4, C5, C6, C3, C9, C10, C1

100uF	RB.2/.4	1	C7

10uF	RB.2/.4	1	C8

1488	DIP14	1	U11

1489	DIP14	1	U10

330R	AXIAL0.4	1	R5

4.00 MHz	XTAL1	1	XTAL1

4.7K	AXIAL0.4	1	R6

4.915 MHz	XTAL1	1	XTAL2

4040	DIP16	1	U12

470R	AXIAL0.4	4	R2, R3, R4, R1

4k7	AXIAL0.4	1	R7

6264/2764	DIP28	4	U2, U1, U4, U3


Board Specifications

Shortcut keys:

Summary:	Generates an ASCII report file that lists of primitives and components on the board, together with holes counts, copper areas and layers used.

Procedure:	Choose File-Reports-Board Specifications, this will generate a report of the following format.

Specifications for F:\BOARDS\DEMO.PCB

On 10-Nov-1991 at 17:44:15

Size of board	5.912 x 5.012 sq in

Equivilent 14 pin components: 0.98 sq in/14 pin component

Components on board	36

Layer	Route	Pads	Tracks	Fills	Text	Arcs

---------------------------------------------------------------------------------------------------------------------------------

Top Layer	Vert	0	427	0	4	0

Bottom Layer	Horiz	0	924	0	1	0

Top Overlay	-	0	203	0	0	15

Multi-Layer	-	435	0	0	0	0

---------------------------------------------------------------------------------------------------------------------------------

Total	435	1554	0	5	15

Layer Pair Vias

---------------------------------------------------------------------------------------------------------------------------------

Top Layer - Bottom Layer	85

---------------------------------------------------------------------------------------------------------------------------------

Total	85

Hole	Size	Pads	Vias

---------------------------------------------------------------------------------------------------------------------------------

28 Mil (0.700mm)	0	85

30 Mil (0.750mm)	435	0

---------------------------------------------------------------------------------------------------------------------------------

Total	435	85


Netlist Status
Netlist-Status

Shortcut keys:

Summary:	Generates and ASCII file that lists the routed/unrouted status of the board together with the names of nets loaded.

Procedure:	Choose File-Reports-Netlist-Status, this will generate a file of the following format

Nets report for D:\GEMINI\TPU\READY50.PCB

On 10-Nov-1991 at 17:44:50

+12

J1-3 to U11-14	Unrouted

-12

J1-4 to U11-1	Unrouted

BAUDCLK

U6-27 to U6-14	Unrouted

U6-14 to U6-13	Unrouted

U6-13 to SW1-9	Unrouted

SW1-16 to SW1-15	Unrouted


Pick and Place

Shortcut keys:

Summary:	Generates a Pick and Place report in Protel (text) or CSV (comma separated value) format. This report lists all component coordinates, rotation and layer status. It can be used as an aid in programming component insertion (pick and place) equipment.

Procedure:	Load all component libraries used to create the layout. Choose File-Reports-Pick and Place. You will be prompted to choose either Protel or CSV format for the report. The default (filename).PIK will be supplied or the user can supply another name and extension. Use the Notepad utility to view the report. The report format is described on page 224 of the User Guide. Since publication of the manual, the report format has been modified slightly and now includes coordinates for both the component center and the center of pin 1 (or A1), as required for some types of insertion equipment. Each column in the report is identifed by a header.


File Exit
File-Exit

Shortcut keys:

Summary:	Quits the current session of Advanced PCB and prompts to save modified files.

Procedure:	Choose File-Exit, if the physical contents of any document window has been modified since the last File-Sale or File-Save As, a Confirm dialog box will prompt the user to save the changes and exit (Yes), discard the changes and close (No) or Cancel the exit.


Edit Undo
Edit-Undo

Shortcut keys:

Summary:	Restores the contents of the current document window to its state prior to the previous command. Multiple level Undo is supported back to the previous File-Open or File-Save As command.

Note:	If system performance degrades, the Undo-Redo stack may be consuming a large proportion of available memory. Choose the File-Save As command to clear the stack and performance will return to normal.

Procedure:	Choose Edit-Undo

See also:	Edit-Redo


Edit Redo
Edit-Redo

Summary:	Restores the previous changes made by the Edit-Undo

Procedure:	Choose Edit-Redo.

See also:	Edit-Undo


Edit Cut
Edit-Cut

Shortcut keys:	+

Summary:	Removes the selected items form the current document window and places them into the Advanced PCB clipboard.

Procedure:	Use Edit-De-Select to de-select objects that are not to be removed. Use Edit-Select to select the objects that will be removed. Choose Edit-Cut. Move the cursor to a reference location, the direction keys may be used to precisely align the cursor with the snap grid, and click or press [image].

See also:	Selection

Edit-Paste

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Edit Copy
Edit-Copy

Shortcut keys:	+

Summary:	Copies the selected items from the current document window to the Advanced PCB clipboard.

Procedure:	Use Edit-De-Select to deselect objects that are not to be copied. Use Edit-Select to select the objects that will be copied. Choose Edit-Copy. Move the cursor to a reference location, the direction keys may be used to precisely align the cursor with the snap grid, and click or press [image].

See also:	Selection

Edit-Paste

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Edit Paste
Edit-Paste

Shortcut keys:	+

Summary:	Copies the items from the Advanced PCB clipboard into the current document window.

Procedure:	Choose a document window, then choose Edit-Paste. The same contents of the clipboard may be pasted multiple times. The cursor will align with the reference point designated when the selection was Cut or Copied to the clipboard.

See also:	Edit-Copy

Edit-Cut


Edit Clear
Edit-Clear

Shortcut keys:	+

Summary:	Removes the selected items from the current document window. Items in the clipboard are not affected.

Procedure:	Choose a document window. Use Edit-De-Select to deselect objects that should not be cleared. Use Edit-Select to select the objects that will be cleared. Choose Edit-Clear.

See also:	Selection

Edit-Paste

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Select Inside Area
Select-Inside Area

Shortcut keys:

Summary:	Selects primitives and components within a rectangular region.

Procedure:	Choose a document window. Choose Edit-Select-Inside Area, then click [image] to define two opposite corners of a selection rectangle. All primitives or components that fall completely inside the rectangle will be included in the selection and will be displayed using the color assigned to selections in the Setup Layers dialog box (Options-Layers command).

When using selection commands (Edit-Select-All, Edit-Select-Inside Area), free primitives will not be included in the selection if they are hidden (Options-Display command). Also, free primitives will be selected only if their layer is active (Options-Layers command). This allows the user to control which free primitives are included in a selection by hiding specific primitives or by turning off specific layers. This applies only to free primitives, not components.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Select Outside Area
Select-Outside Area

Shortcut keys:

Summary:	Selects primitives and components outside a rectangular region.

Procedure:	Choose a document window. Choose Edit-Select-Outside Area, then choose two opposite corners of a region.

All primitives or components that fall completely outside the rectangle will be included in the current selection and will be displayed using the color assigned to selections in the Setup Layers dialog box (Options-Layers command).

When using selection commands (Edit-Select-All, Edit-Select-Inside Area), free primitives will not be included in the selection if they are hidden (Options-Display command). Also, free primitives will be selected only if their layer is active (Options-Layers command). This allows the user to control which free primitives are included in a selection by hiding specific primitives or by turning off specific layers. This applies only to free primitives, not components.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Select All
Select-All

Shortcut keys:

Summary:	Adds all primitives and components within the current document window to the current selection.

Procedure:	Choose a document window, then choose Edit-Select-All.

When using selection commands (Edit-Select-All, Edit-Select-Inside Area), free primitives will not be included in the selection if they are hidden (Options-Display command). Also, free primitives will be selected only if their layer is active (Options-Layers command). This allows the user to control which free primitives are included in a selection by hiding specific primitives or by turning off specific layers. This applies only to free primitives, not components.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Select Free Primitives
Select-Free Primitives

Shortcut keys:

Summary:	Selects all free primitives within the current document window.

Procedure:	Choose a document window, then choose Edit-Select-Free Primitives. Free primitives include pads, vias, tracks, area fills, arecs and text which are not associated with any placed components. This procedure provides a way to completely unroute a board in a single operation.

When using selection commands (Edit-Select-All, Edit-Select-Inside Area), free primitives will not be included in the selection if they are hidden (Options-Display command). Also, free primitives will be selected only if their layer is active (Options-Layers command). This allows the user to control which free primitives are included in a selection by hiding specific primitives or by turning off specific layers. This applies only to free primitives, not components.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Select All On Layer
Select-All On Layer

Shortcut keys:

Summary:	All items on the Current Layer within the current document window become selected.

Procedure:	Choose a document window, then use Current Layer to choose the layer that will be selected. Choose Edit-Select-All On Layer.

When using selection commands (Edit-Select-All, Edit-Select-Inside Area), free primitives will not be included in the selection if they are hidden (Options-Display command). Also, free primitives will be selected only if their layer is active (Options-Layers command). This allows the user to control which free primitives are included in a selection by hiding specific primitives or by turning off specific layers. This applies only to free primitives, not components.

See also:	Selection

Edit-Paste

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Select Physical Net
Select-Physical Net

Shortcut keys:

Summary:	This command selects all free primitives (tracks, vias, fills) that connect a physical net within the current document window.

Procedure:	Choose a document window, choose Select-Physical Net, then choose any primitive on a copper trace layer. All primitives that touch will be selected.

To use this feature:

1.	Choose Edit-Select-Physical Net;

You will be prompted "Select Pad."

2.	Position the cursor over a component pad within the desired net and press [image] or [image].

The continuous physical net extending from the selected pad will highlight with the selection color.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Select Hole Size
Select-Hole Size

Shortcut keys:

Summary:	Selects all pads with a common hole size definition.

Procedure:	Choose a document window. Choose Select-Hole Size, then type a Hole size value into the dialog box and press OK.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Select Physical Connection
Select-Physical Connection

Shortcut keys:

Summary:	Selects all primitives on a physical connection.

Procedure:	Choose a document window. Choose Select-Physical Connection, then choose any non-pad primitive on a physical connection.

To use this feature:

1.	Choose Edit-Select-Physical Net;

You will be prompted "Select Pad."

2.	Position the cursor over a component pad within the desired net and press [image] or [image].

The continuous physical net extending from the selected pad to other pads (but not beyond) will highlight with the selection color.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Off Grid Pads
Select-Off Grid Pads

Shortcut keys:

Summary:	Adds all pads which are not centered on the current snap grid to the selection.

Procedure:	Choose a document window. Choose Edit-Select-Off Grid Pads. All pads which are not centered on the current snap grid will be displayed in the selection color and added to the current selection.


De-Select Inside Area
DeSelect-Inside Area

Summary:	De-selects all primitives and components within a rectangular region.

Procedure:	Choose a document window. Choose Edit-DeSelect-Inside Area, then choose two opposite corners of the region to be de-selected.

See also:	Selection

Edit-Paste

Edit-Select

Edit-De-Select

Edit-Toggle Selection


De-Select Outside Area
DeSelect-Outside Area

Summary:	De-selects all primitives and components outside a rectangular region.

Procedure:	Choose a document window. Choose Edit-DeSelect-Outside Area, then choose two opposite corners of a region. The area outside the region will be de-selected.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


De-Select All
DeSelect-All

Summary:	De-selects all primitives and components within the current document window.

Procedure:	Choose a document window, then choose Edit-DeSelect-All.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


De-Select Free Primitives
DeSelect-Free Primitives

Summary:	De-selects all free primitives within the current document window.

Procedure:	Choose a document window, then choose Edit-DeSelect-Free Primitives.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


De-Select All on Layer
DeSelect-All on Layer

Summary:	De-selects all primitives and components on the Current Layer within the current document window.

Procedure:	Choose a document window. Choose a layer, then use Current-Layer to choose the layer that will be de-selected. Choose Edit-DeSelect-All on Layer.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Toggle Selection


Toggle Arc
Toggle Arcs

Summary:	Selects all arcs were not previously selected within the document window, and de-selects all arcs that were previously selected within the document window.

Procedure:	Choose a document window, then choose Edit-Toggle Selection-Arcs.

See also:	Selection

Edit-Select

Edit-De-Select


Toggle Component
Toggle Components

Summary:	Selects all components that were not previously selected within the document window, and de-selects all components that were previously selected within the document window.

Procedure:	Choose a document window, then choose Edit-Toggle Selection-Components.

See also:	Selection

Edit-Select

Edit-De-Select


Toggle Fill
Toggle Fills

Summary:	Selects all fills that were not previously selected within the document window, and de-selects all fills that were previously selected within the document window.

Procedure:	Choose a document window, then choose Edit-Toggle Selection-Fills.

See also:	Selection

Edit-Select

Edit-De-Select


Toggle Pad
Toggle Pads

Summary:	Selects all pads that were not previously selected within the document window, and de-selects all pads that were previously selected within the document window.

Procedure:	Choose a document window, then choose Edit-Toggle Selection-Pads.

See also:	Selection

Edit-Select

Edit-De-Select


Toggle Polygon
Toggle Polygons

Summary:	Selects all polygons that were not previously selected within the document window, and de-selects all polygons that were previously selected within the document window.

Procedure:	Choose a document window, then choose Edit-Toggle Selection-Polygons.

See also:	Selection

Edit-Select

Edit-De-Select


Toggle String
Toggle Strings

Summary:	Selects all text that was not previously selected within the document window, and de-selects all text that was previously selected within the document window.

Procedure:	Choose a document window, then choose Edit-Toggle Selection-Strings.

See also:	Selection

Edit-Select

Edit-De-Select


Toggle Track
Toggle Tracks

Summary:	Selects all tracks that were not previously selected within the document window, and de-selects all tracks that were previously selected within the document window.

Procedure:	Choose a document window, then choose Edit-Toggle Selection-Tracks.

See also:	Selection

Edit-Select

Edit-De-Select


Toggle Via
Toggle Vias

Summary:	Selects all vias that were not previously selected within the document window, and de-selects all vias that were previously selected within the document window.

Procedure:	Choose a document window, then choose Edit-Toggle Selection-Vias.

See also:	Selection

Edit-Select

Edit-De-Select


Delete Arc
Delete-Arcs

Shortcut keys:

Summary:	Removes an arc.

Procedure:	Choose a document window. If the arc is not on the Current Layer and is below other arcs, then use Current-Layer to choose the layer that contains the arc. Now choose Edit-Delete-Arc and choose the arc.


Delete Component
Delete-Components

Shortcut keys:

Summary:	Removes a component.

Procedure:	Choose a document window. If the component is not on the Current Layer and is below other components, then use Current-Layer  to choose the layer that contains the component. Now choose Edit-Delete-component and choose the component.


Delete Fill
Delete-Fills

Shortcut keys:

Summary:	Removes a fill.

Procedure:	Choose a document window. If the fill is not on the Current Layer and is below other fills, then use Current-Layer to choose the layer that contains the fill. Now choose Edit-Delete-Fill and choose the fill.


Delete Pad
Delete-Pads

Shortcut keys:

Summary:	Removes a pad.

Procedure:	Choose a document window. If the pad is not on the Current Layer and is below other pads, then use Current-Layer to choose the layer that contains the pad. Now choose Edit-Delete-Pad and choose the pad.


Delete String
Delete-Strings

Shortcut keys:

Summary:	Removes text.

Procedure:	Choose a document window. If the string is not on the Current Layer and is below other strings, then use Current-Layer to choose the layer that contains the string. Now choose Edit-Delete-String and choose the string.


Delete Track
Delete-Tracks

Shortcut keys:

Summary:	Removes a track.

Procedure:	Choose a document window. If the track is not on the Current Layer and is below other tracks, then use Current-Layer to choose the layer that contains the track. Now choose Edit-Delete-Track and choose the track.


Delete Via
Delete-Vias

Shortcut keys:

Summary:	Removes a via.

Procedure:	Choose a document window. If the via is not on the Current Layer and is below other vias, then use Current-Layer to choose the layer that contains the via. Now choose Edit-Delete-Via and choose the via.


Delete Polygon
Delete-Polygon

Shortcut keys:

Summary:	Removes a (copper pour) polygon.

Procedure:	Choose a document window. If the via is not on the Current Layer and is below other vias, then use Current-Layer to choose the layer that contains the via. Now choose Edit-Delete-Polygon and choose the polygon.


Change Arc
Change-Arc

Shortcut keys:	  or double-click on any arc segment.

Summary:	Modifies any attribute of an arc. The modifications can be applied globally to other arcs.

Procedure:	Choose a window. If the arc is not on the Current Layer and is below other arcs, then use Current-Layer to choose the layer that contains the arc. Now choose Edit-Change-Arc and choose the arc. Use the options button if the changes should also be applied to other arcs.

See also:	Changing Arcs

Making Changes

Selection


Change Component
Change-Component

Shortcut keys:	  or double-click on any component.

Summary:	Modifies any attribute of a component. The modifications can be applied globally to other components.

Procedure:	Choose a document window. If the component is not on the Current Layer and is below other components, then use Current-Layer to choose the layer that contains the component. Now choose Edit-Change-Component and choose the component. Use the options button if the changes should also be applied to other components.

See also:	Changing Components

Making Changes

Selection


Change Fill
Change-Fill

Shortcut keys:	  or double-click on any area fill.

Summary:	Modifies any attribute of a fill. The modifications can be applied globally to other fills.

Procedure:	Choose a document window. If the fill is not on the Current Layer and is below other fills, then use Current-Layer to choose the layer that contains the fill. Now choose Edit-Change-Fill and choose the fill. Use the options button if the changes should also be applied to other fills.

See also:	Changing Fills

Making Changes

Selection


Change Pad
Change-Pad

Shortcut keys:	   or double-click on any free or component pad.

Summary:	Modifies any attribute of a pad. The modifications can be applied globally to other pads.

Procedure:	Choose a document window. If the pad is not on the Current Layer and is below other pads, then use Current-Layer to choose the layer that contains the pad. Now choose Edit-Change-Pad and choose the pad. Use the options button if the changes should also be applied to other pads.

See also:	Changing Pads

Making Changes

Selection


Change String
Change-String

Shortcut keys:	  or double-click on any free text string.

Summary:	Modifies any attribute of text. The modifications can be applied globally to other text.

Procedure:	Choose a document window. If the string is not on the Current Layer and is below other strings, then use Current-Layer to choose the layer that contains the string. Now choose Edit-Change-String and choose the string. Use the options button if the changes should also be applied to other strings.

See also:	Changing Strings

Making Changes

Selection


Change Repour
Change-Repour Polygon

Shortcut keys:

Summary:	Repours an existing polygon (copper pour) without changing its vertices.

Procedure:	Choose a document window. If the polygon plane is not on the Current Layer use Current-Layer to choose the layer that contains the polygon plane. Now choose Edit-Change-Repour Polygon and choose the polygon plane. The Place-Polygon Plane dialog box opens. You can change any attribute of the polygon at this time:

Editable attributes of polygons include:

Connect to Net	Specifies a Net. Pads that are associated with the net will be automatically connected to planes (on the same layer) using thermal relief type conductors.

Remove Dead Copper	Removes any islands of unconnected copper, when the Connect to Net option is specified. Warning: If the plane is unable to connect to a primitive for the specified net, the entire plane will be removed when this option is enabled.

Pour Over Same Net	Includes any tracks, fills or vias connected to the specified net, when Connect to Net is enabled. Copper pours over the top of these primitives.

Horizontal and/or Vertical Hatching	Specifies the track orientation used to fill the polygon. Choosing one orientation only may limit the resolution of the fill for complex shapes.

Fills or Tracks	Allows the user to specify area fills, rather than tracks for solid (rather than latticed) pours. Users can also substitute fills for tracks after the pour is generated by using the Edit-Change-Convert Selection to Fills command.

Surround Pads with Arcs or Octagons	Specifies the method used to surround pads inside the copper pour area.

Layer	Allows the user to re-assign the pour to a new layer.

Track and grid	Specifies the track and grid size for generating the fill. When these two values are the same, a solid copper pour results. Coarse grid and track assignments result in faster pour generation. Finer settings increase the resolution of the pour. Clearances for pours are determined by the Netlist-Clearances dialog box settings. These clearances are additive. In other words, track clearance settings of 6 mils results in a 12 mil air gap between any two tracks.

When all options have been selected. Click OK to repour the polygon. The polygon will repour. This may take a few moments, if the polygon is large or complex.

See also:	Edit-Delete-Polygon

Edit Polygon Vertices

About PCB version 2.0


Edit Polygon Vertices

Shortcut keys:

Summary:	Graphically edits the perimeter of a placed polygon plane.

Procedure:	Choose a document window. If the polygon plane is not on the Current Layer use Current-Layer to choose the layer that contains the polygon plane. Now choose Edit-Change-Edit Polygon Vertices and click inside the polygon. The perimeter tracks will be highlighted.

1.	Click on any perimeter track segment and the cursor will jump to the nearest vertex. Move the vertex and click.

2.	Position the cursor over another perimeter track and click again to move another vertex. Press {BMC INS.BMP} or [image] keys to add or remove vertices. Press [image] to convert a perimeter track into an arc segment and press [image] to convert a perimeter arc into a track segment.

3.	Press {BMC ESC.BMP} or {BMC LMOUSE.BMP} to re-open the Place-Polygon Plane dialog box.

4.	You can re-define the design rules for the polygon. Click OK.

The polygon will repour. This may take a few moments, if the polygon is large or complex. Choose another polygon to edit or press {BMC ESC.BMP} or {BMC LMOUSE.BMP} to exit this command.

See also:	Delete-Polygon

Repour Polygon


Convert Selection to Fills

Shortcut keys:

Summary:	Recalculates the selection area and replaces track segments with area fills. Automates simplification of complex polygon plane geometry and other filled areas on the board.

Procedure:	Choose a document window. Use any combination of the Edit-Select and -De Select commands (or shortcuts) to add items to the current selection. Selected items will be displayed using the selection color (Options-Layers command). When the desired items are selected, choose the Edit-Change-Convert Selection to Fills command and click inside any continuous selection. The .

See also:	Delete-Polygon

Repour Polygon

Edit Polygon Vertices


Change Track
Change-Track

Shortcut keys:

Summary:	Modifies any attribute of a track. The modifications can be applied globally to other tracks.

Procedure:	Choose a document window. If the track is not on the Current Layer and is below other tracks, then use Current-Layer to choose the layer that contains the track. Now choose Edit-Change-Track and choose the track. Use the options button if the changes should also be applied to other tracks.

See also:	Changing Tracks

Making Changes

Selection


Change Via
Change-Via

Shortcut keys:

Summary:	Modifies any attribute of a via. The modifications can be applied globally to other vias.

Procedure:	Choose a document window. If the via is not on the Current Layer and is below other vias, then use Current-Layer to choose the layer that contains the via. Now choose Edit-Change-Via and choose the via. Use the options button if the changes should also be applied to other vias.

See also:	Changing Vias

Making Changes

Selection


Change Selected Vias to Pads
Change-Convert Selected Vias To Pads

Summary:	Changes selected vias to pads. This command supports conversion of PADS-PCB and PADS 2000 files where vias are used to connect to power and ground layers. Allows proper connection to internal power and ground planes using editable pads.

Procedure:	Use the Edit-Select commands (or SHIFT+LEFT MOUSE shortcut) to select the desired vias. Then, use the Edit-Change Selected Vias To Pads command to convert these vias into pads. Power and ground plane assignments will be inherited from the net assignments associated with the vias.

See also:	Selection


Move Selection
Move-Selection

Shortcut keys:

Summary:	Moves all selected items within a document window.

Procedure:	Choose a document window. Position the cursor at the location that will be used as reference, the direction keys can be used to precisely align the cursor to the snap grid. If cursor is not locked (see Options-Preferences), click at this location then choose Edit-Move-Move Selection. If the cursor is locked, leave the cursor at this position until the keyboard is used to choose Edit-Move-Move Selection.

Note: Moving a selection will not drag tracks which are connected inside the selection area, irrespective of whether the Drag Tracks option is enabled or disabled (Options-Preferences dialog box).

See also:	Selection

Edit-Select

Edit-De-Select


Flip Selection
Move-Flip Selection

Shortcut keys:

Summary:	Mirrors the orientation of all selected items within the current document window.

Procedure:	Choose a document window. Use Edit-Select and Edit-De-select as needed, then choose Edit-Move-Flip Selection.

See also:	Selection

Edit-Select

Edit-De-Select


Rotate Selection

Shortcut keys:

Summary:	Rotates all selected components within the current document window. The degree and center of rotation may be defined.

Procedure:	Choose a document window. Use Edit-Select and Edit-De-select as needed, then choose Edit-Move-Rotate Selection.

The selection becomes free to rotate in .001 degree increments.

When you choose this command Advanced PCB will prompt for a reference mark and for the amount of rotation in degrees (to 0.001 degree). This command has a one degree resolution. As with other Move commands, the current cursor position becomes the reference point for the selection, in this case the reference point serves as the axis for the rotation.

When you rotate selections there are a number of limitations that you should be aware of. For example, rectangular pads and rectangular fills will have their position rotated but their sides will remain parallel to the X or Y axis. You may wish to change component pad shapes to round before rotating, unless you are rotating in increments of ninety degrees.

See also:	Selection

Edit-Select

Edit-De-Select


Break Track

Shortcut keys:

Summary:	Creates a vertex in a track at the chosen location. The vertex may be moved to a new location.

Procedure:	Choose a document window. If the track is not on the Current Layer and is below other tracks, use Current-Layer to choose the layer that contains the track. Now choose Edit-Move-Break Track and choose the track.

See also:	Move track shortcuts


Move Drag End
Move-Drag End

Shortcut keys:

Summary:	Moves the end point of a track to a new location.

Procedure:

1.	Choose Edit-Move-Drag End.

You will be prompted "Select track." If the track is not on the Current Layer and is below other tracks, use Current-Layer to choose the layer that contains the track.

2.	Position the cursor over the track segment and click once or press [image];

The cursor will jump to the nearest end of the track segment. The selected segment and any intersecting segments connected to the end will be highlighted.

The prompt "Dragging track end" will be displayed on the Status line.

3.	Drag the track end to the new location and press [image] or [image] again.

"Select track" will be displayed on the Status line. If a via is part of the highlighted intersection, it will move along with the intersecting tracks.

4.	Select another track or press [image] or [image] to cancel the move.

See also:	Move track shortcuts


Move Whole Track
Move-Whole Track

Shortcut keys:

Summary:	Moves an entire track (and all connecting track ends and vias). The track retains its orientation.

Procedure:	If the track is not on the Current Layer and is below other tracks, use Current-Layer to choose the layer that contains the track.

1.	Choose Edit-Move-Whole Track;

You will be prompted "Select track."

2.	Position the cursor over the track segment and click [image] or press [image];

The selection will highlight, including all connected track segments and vias. The prompt changes to "Moving track."

3.	Move the cursor to drag the track to the new location and press [image] or click [image] again;

"Select track" will be displayed on the Status line.

4.	Select another track or press [image] or [image] to cancel the move.

See also:	Move track shortcuts


Move track shortcuts

To select and move a track:

Hold down [image] and click [image] once on a segment.

One of two different move commands will be executed. If you are within 25% of the track end, then the end will be moved as though you had chosen the Drag End command. If you select the middle 50% of the track then the whole track will be moved together with any tracks or vias that are attached to the ends of the track.

To "break" a track (convert it into two joined segments);

Hold down [image] [image] together and click on the track.

The track will be broken and you can drag the segments to a new location.


Move Re-Route
Move-Re-Route

Shortcut keys:

Summary:	Creates and moves a vertex in a track. The vertex may be placed in a new location. This sequence will continue as new vertices form after each placement.

Procedure:	This feature is similar to the Break Track command. When re-routing, the cursor jumps to the nearest pad on the physical connection and the selected segment highlights. Each time you press [image] or [image], the highlighted track segment is terminated and a new segment is started.

To re-route a track:

1.	Choose Edit-Move-Reroute

You will be prompted "Select Track."

2.	Position the cursor over the track segment and press [image] or [image] to select a track;

The track will break at the cursor position and the two created track sections will rubber band with the cursor.

3.	Drag the highlighted segments to a new location and press [image] or [image] again;

One end becomes a "placed" track segment (and the highlight is removed). Two highlighted segments are now displayed from the end of the newly placed segment.

4.	Continue to move and press [image] or [image] to reroute the track segment-by-segment;

5.	When finished, press [image] or [image] and a track segment will be placed between the end of the last segment and the end of the originally selected track.

You will then be prompted "Select  Track."

To finish Re-routing tracks, press [image] or [image].

You can change layers at any time during this operation with [image], [image] or [image] keys. If you specify two consecutive track segments, and change layers between, then a via will be place at their intersection. (This Auto Via feature can be disabled).

To move both the complete track segment (and all connecting track ends and vias), choose a document window. If the track is not on the Current Layer and is below other tracks, use Current-Layer to choose the layer that contains the track. Now choose Edit-Move-Re-Route and choose the track.


Move Arc
Move-Arc

Shortcut keys:

Summary:	Moves an arc to a new location.

Procedure:	Choose a document window. If the arc is not on the Current Layer and is below other arcs, use Current-Layer to choose the layer that contains the arc. Now choose Edit-Move-Arc and choose the arc.


Move Component
Move-Component

Shortcut keys:

Summary:	Moves a component to a new location.

Procedure:	Choose a document window. Now choose Edit-Move-Component and choose the component.

For SMD components, the component will be placed on the Top Layer, unless the Current Layer is specifically set to the Bottom Layer.

While moving a component, you can also rotate it around the cursor and flip it in the x and y axis about the cursor using the following keys

Rotates the component 90 degrees clockwise. Choose repeatedly to continue the rotation.

Flip the component in the X axis.

Flip the component in the Y axis


Move Fill
Move-Fill

Shortcut keys:

Summary:	Moves a fill to a new location.

Procedure:	Choose a document window. If the fill is not on the current layer and is below other fills, use Current Layer to choose the layer that contains the fill. Now choose Edit-Move-Fill and choose the fill.

If you select the edge of a fill, then it can be resized in the X or Y axis. If you select the corner, then the fill by resized in X and Y at the same time.


Move Pad
Move-Pad

Shortcut keys:

Summary:	Moves a pad to a new location.

Procedure:	Choose a document window. If the pad is not on the Current Layer and is below other pads, use Current-Layer to choose the layer that contains the pad. Now choose Edit-Move-Pad and choose the pad.


Move Polygon
Move-Polygon

Shortcut keys:

Summary:	Moves a pad to a new location.

Procedure:	Choose a document window. If the polygon is not on the Current Layer and is below other pads, use Current-Layer to choose the layer that contains the pad. Now choose Edit-Move-Polygon and click [image] anywhere inside the copper pour.

When you move the polygon to a new location, the Place-Polygon Plane dialog box will open, allowing you to accept the current polygon design rules, or assign new rules. The polygon will then be re-poured in the new location.


Move String
Move-String

Shortcut keys:

Summary:	Moves text to a new location.

Procedure:	Choose a document window. If the string is not on the Current Layer and is below other strings, use Current-Layer to choose the layer that contains the string. Now choose Edit-Move-String and choose the string. If you select a component's designator or comment string, its associated component will highlight during the move.


Move Via
Move-Via

Shortcut keys:

Summary:	Moves a via to a new location. No tracks are dragged.

Procedure:	Choose a document window. If the via is not on the Current Layer and is below other vias, use Current-Layer to choose the layer that contains the via. Now choose Edit-Move-Via and choose the via.


Place Arc By Center
Place-Arc By Center

Shortcut keys:

Summary:	Places an arc. Center, start angle, radius, and end angle are defined during placement.

Procedure:	Choose a document window and use the Current Layer to choose a layer for placement. Now choose Edit-Place-Arc (Center) and follow the prompts. The Current Track Width is used for the line width of the arc.

You can change layers with the [image], [image] or [image] keys.

This command can also be selected by pressing the Arc button on the Tool Bar.

Sets the default track width on the fly.


Place Arc By Edge
Place-Arc By Edge

Shortcut keys:

Summary:	Places of an arc. Start angle, radius, Center, and end angle are defined during placement.

Procedure:	Choose a document window and use the Current Layer to choose a layer for placement. Now choose Edit-Place-Arc (Edge) and follow the prompts. The Current Track Width is used for the line width of the arc.

You can change layers with the [image] , [image] or [image] keys.

Sets the default track width on the fly.


Place Component
Place-Component

Shortcut keys:

Summary:	Retrieves a library component for placement. During placement the component may be moved, rotated, or mirrored.

Procedure:	Choose a document window and use the Place-Component command. Enter a component pattern name, or enter a question mark to choose from a list of available component patterns. Follow the prompts.

When you choose this command you will be prompted for a component pattern. Enter a name (or ? to select from a displayed list). for example DIP16 or TO-3.

If the component you are placing is an SMT component, then the Current Layer should be the top or bottom layer. All components will be placed on the top of the board unless you go specifically to the bottom layer.

The program will now ask for the component designator. This is the actual name of the component, U1 for example. Note that this must be different from all other component designators current used in the design. If not, then an error  message will appear.

Designators can be up to 8 characters long and any alphanumeric character. It is suggested that you don't start designators with a number and that you do finish them with a number. This allows the auto numbering system to function at its best.

The program will supply you with a suggested designator based on the last component placed with the same pattern. If you wish you can enter [image]? or [image]?. The program will then supply the next available number for this designator.

For example, if the last designator starting with the letter [image] is U12 and you enter [image]?, then the program will assign U13 to the component. If you just enter ? then the program will use the lowest letter (starting at A) with the lowest number (starting at 1).

Now you will be asked for the component comment. This is the value or type of the component, 74LS123 or 100K for example.

Comments can be up to 32 characters long and any alphanumeric character. The program will supply you with a suggested comment based on the last component placed with the same pattern.

The component will now be loaded from the library and displayed on the screen.

Rotating:	Move it around with the cursor, rotate with [image] or mirror with [image] or [image]. This command can also be selected by pressing the COMP button on the Tool Bar.

See also:	Library-Components


Place Fill
Place-Fill

Shortcut keys:

Summary:	Places a rectangular fill region.

Procedure:	Choose a document window and use the Current Layer to choose a layer for placement. Now choose Edit-Place-Fill and follow the prompts.

You can change layers with the [image], [image] or [image] keys.

This command can also be selected by pressing the FILL button on the Tool Bar.


Place Pad
Place-Pad

Shortcut keys:

Summary:	Places a pad. Its attributes match those defined by the Current-Pad. The pad may be moved and rotated during placement.

Procedure:	Choose a document window and if placing a single layer pad, use the Current Layer  to choose a layer for placement. Now choose Edit-Place-Pad and follow the prompts.

Use [image] to rotate the pad.

 	If you are placing an SMT pad or an edge connector (a single sided pad), then the Current Layer should (normally) be top layer or bottom layer.

You can change layers with the [image], [image] or [image] keys.

Note that the designator of placed pads is set empty by default. To place multiple pads with incremental numbers, use the Edit-Change-Pad command to change the designator.

This command can also be selected by pressing the PAD button on the Tool Bar.

Sets the default pad type on the fly.


Place String
Place-String

Shortcut keys:

Summary:	Places a line of text. During placement, text can be moved, rotated, or mirrored.

Procedure:	Choose a document window and use the Current Layer to choose a layer for placement. Now choose Edit-Place-String and follow the prompts.

Change Layers:	You can change layers with the [image], [image] or [image] keys.

Size and Font:	The string will have size and font as defined by Current String.

Moving:	Move during placement with the cursor, rotate with [image] or mirror with [image] or [image].

This command can also be selected by pressing the STRING button on the Tool Bar.

Sets the default string height on the fly.

This command can also be selected by pressing the STRING button on the Tool Bar.

See also:	Special strings


Place Track
Special strings

Special strings are text strings that can be placed on any layer and printed (or plotted) with pre-defined contents. For example, placing the string .DATE_PRINT will generate a string with the current date (using the system clock) at the time the layer plot is generated. Special strings include:

.DATE_PRINT	Generates the current date when the layer is printed.

.TIME_PRINT	Generates the current time.

.LAYER_NAME	Generates the name of the layer.

.PLOT_FILE_NAME	Generates the plot filename.

.PCB_FILE_NAME	Generates the PCB filename.

.STRING_COUNT	Generates a count of the number of strings in the file.

.HOLE_COUNT	Generates a count of the number of holes in the file.

.TRACK_COUNT	Generates a count of the number of tracks in the file.

.PAD_COUNT	Generates a count of the number of pads in the file.

.VIA_COUNT	Generates a count of the number of vias in the file.

.FILL_COUNT	Generates a count of the number of area fills in the file.

.COMPONENT_COUNT	Generates a count of the number of components in the file.

.NET_COUNT	Generates a count of the number of nets in the file.

.LEGEND	Generates a drill symbol legend, when printing the Drill Guide layer.


Special strings
Place-Track

Shortcut keys:

Summary:	places tracks. During placement, each end point becomes a vertex and the starting point of a new track. Track width is predefined using the Current-Track.

Procedure:	Choose the document window and use the Current Layer to choose a layer for placement. Now choose Edit-Place-Track and follow the prompts.

The Track Place Mode can be changed on the fly with [image].

You can change layers with the [image], [image] or [image] keys. If the Auto Via Option is on, then when you change from one signal layer to another, a via will be inserted.

Sets the default track width on the fly.


Place Via
Place-Via

Shortcut keys:

Summary:	Places a via. The via can be moved during placement, its attributes are predefined using the Current Via.

Procedure:	Choose a document window and use the Current Layer to choose a layer for placement. Now choose Edit-Place-Via and follow the prompts.

The layer pair, diameter and hole size are setup using the Current Via Commands.

Sets the default diameter on the fly.


Place Polygon Plane
Place-Polygon Plane

Shortcut keys:

Summary:	Creates a plane of copper. clearances are maintained around all existing primitives and components and thermal ties are made to pads on a defined net.

Procedure:	Choose the document window and use the Current Layer to choose a layer for placement. Now choose Edit-Place-Polygon Plane.

Editable attributes of polygons include:

Connect to Net	Specifies a Net. Pads that are associated with the net will be automatically connected to planes (on the same layer) using thermal relief type conductors.

Remove Dead Copper	Removes any islands of unconnected copper, when the Connect to Net option is specified. Warning: If the plane is unable to connect to a primitive for the specified net, the entire plane will be removed when this option is enabled.

Pour Over Same Net	Includes any tracks, fills or vias connected to the specified net, when Connect to Net is enabled. Copper pours over the top of these primitives.

Horizontal and/or Vertical Hatching	Specifies the track orientation used to fill the polygon. Choosing one orientation only may limit the resolution of the fill for complex shapes.

Fills or Tracks	Allows the user to specify area fills, rather than tracks for solid (rather than latticed) pours. Users can also substitute fills for tracks after the pour is generated by using the Edit-Change-Convert Selection to Fills command.

Surround Pads with Arcs or Octagons	Specifies the method used to surround pads inside the copper pour area.

Layer	Allows the user to re-assign the pour to a new layer.

Track and grid	Specifies the track and grid size for generating the fill. When these two values are the same, a solid copper pour results. Coarse grid and track assignments result in faster pour generation. Finer settings increase the resolution of the pour. Clearances for pours are determined by the Netlist-Clearances dialog box settings. These clearances are additive. In other words, track clearance settings of 6 mils results in a 12 mil air gap between any two tracks.

About Polygon planes

The Polygon plane feature makes full use of Advanced PCBs 32-bit placement accuracy. Copper pours are  fully editable after placement. Users can move, add or delete vertices and there is an option to fill pours with area fills, as well as with horizonatal and/or vertical tracks. Copper will automatically flood over primitives that belong to the same net (when this option is enabled). These features are documented in the User Guide and Reference.

The Edit-Change-Repour Polygon is used to update a selected polygon at any time. This is especially useful when you need to move or place a primitive inside the polygon area. After making the changes, choose the Repour Polygon command and then click to select the polygon. The Edit-Polygon dialog box will open. You can change any attributes (e.g. polygon grid and polygon track sizes, net assignment, etc.) at this time, if desired. Click Place and the polygon will be re-generated using the original vertices (corners).

The Edit-Change-Edit-Polygon Vertices command allows you to alter the shape of a copper pour, without re-generating the polygon. Vertices can be moved, added or deleted graphically. The [image] and [image] keys are used to add or remove vertices from outline segments. When editing vertices, pressing [image] will convert a track segment into an arc and pressing [image] will convert an arc segment into a track.

You can also specify fills (rather than tracks) to fill the polygon shape. Additionally, an Edit-Change-Replace Selection with Fills command has been added. This command will remove a selection, replacing solid areas (in polygons, typically) with area fills which will print more efficiently.

The Pour Over Same Net option will flood the copper over the top of exisiting tracks, fills or vias associated with the assigned net, when the Connect to Net option is enabled. When this option is not enabled, the pour area will avoid touching these same net primitives, observing the air gaps specified for these items under the Netlist-Clearances command.

Toggle Selection-Polygon and Move-Polygon commands have been added to the Edit menu. When a polygon is moved, the user will have the opportunity to change the polygon design rules, as when editing an existing polygon pour.

An Edit-Delete-Polygon command has also been added, to simplify  removal of copper pours.


Outline Selected Items

Shortcut keys:

Summary:	Generates an outline of track and arc segments around a selection. This feature can be used to electrically isolate critical nets, by tying the outline to a ground source. The Current track width is used to define the outline tracks and arcs. Current primitive-to-primitive clearances (Netlist-Clearances command) are observed, but net assignment is not regarded. Net-to-net clearance violations will be highlighted when you run the Netlist-DRC command or if the online DRC system is active.

Procedure:	Use the Edit-Select commands to build a selection for outlining. Then, choose Edit-Place-Outline Selected Items.


Place Coordinate
Place-Coordinate

Shortcut keys:

Summary:	Places text that indicates the coordinates.

Procedure:	Choose a document window and use the Current Layer to choose a layer for placement. Now choose Edit-Place-Coordinate String and follow the prompts.


Place Dimension
Place-Dimension

Shortcut keys:

Summary:	Places a dimension line that indicates the length of the line.

Procedure:	Choose a document window and use the Current Layer to choose a layer for placement. Now choose Edit-Place-Dimension and follow the prompts.


Place Array
Place-Array

Shortcut keys:

Summary:	Generates a repeated placement of the contents of the clipboard. The placement can be defined as linear ( to 0.001 mil accuracy) or circular (to 0 .001 degree accuracy).

Procedure:	Choose a document window and select the primitives or components that will be placed in the array. Choose Edit-Copy or Edit-Cut to place the selection in the clipboard. Choose Edit-Place-Array, set the dialog box options and use the Place-Array button.

The options are:

Circular/Linear	Linear will place items in a straight line, circular will place in a circular array.

Count	The number of items to be placed by repeat command.

X-offset	The horizontal distance between the next placed and the last placed item.

Y-offset	The vertical distance between the next placed and the last placed item.

Increment	This is used for designators on pads. Setting this to 1 will give a series, for example A1, A2, A3 or 1, 2, 3. For example, to place a vertical row of pads for one half of DIP16 component, place the first pad manually. Edit the pad and set its designator to 1.

Cut the pad into the clipboard with the Edit-Cut Command. Now Select Place-Array, Set Y-offset to -100 mils X-offset to 0, text increment to 1, and linear. Set count to 8. Press the Place-Array button and a row of pads will appear, descending down from the manually placed pad. There designators will be 1,2,3,4,5,6,7,8 from top to bottom.

See also:	Selection

Edit-Select

Edit-De-Select

Edit-Paste

Edit-Copy

Edit-Cut

Edit-Toggle Selection


Jump Component
Jump-Component

Shortcut keys:

Summary:	Moves the cursor to the component's reference point.

Procedure:	Choose a document window. Use the Edit-Jump-Component. Enter a component designator, or enter a question mark to choose from a list.


Jump Net
Jump-Net

Shortcut keys:

Summary:	Moves the cursor to the nearest pad on a net.

Procedure:	Choose a document window. Use the Edit-Jump-Net and enter a net name or enter a question mark to choose from a list.


Jump Pad
Jump-Pad

Shortcut keys:

Summary:	Moves the cursor to a pad.

Procedure:	Choose a document window, then choose Edit-Jump-Pad. Type the component designator-pad number and click OK or press [image]. Select the component on which to search, then type a pin number.


Jump String
Jump-String

Shortcut keys:

Summary:	Moves the cursor to the text.

Procedure:	Choose a document window. Use the Edit-Jump-String then enter the text.

The program will perform three searches when jumping to a string.

1.	Firstly for a string that matches the specified string in case, characters and length.

1.	If not found then it searches for a string with same characters and length but ignoring case.

2.	If still not found then it searches for a string with same characters in it but perhaps having more characters (and ignoring case).

For Example:	Entering "Component" will find the string 'Component' first, if not found it will find the string COMPONENT and if still not found it would find the string 'COMPONENT LAYER'.


Jump Absolute Origin
Jump-Absolute Origin

Shortcut keys:

Summary:	Moves the cursor to the lower left corner of the work space.

Procedure:	Choose a document window, then choose Edit-Jump-Absolute Origin.


Jump Current Origin
Jump-Current Origin

Shortcut keys:

Summary:	Moves the cursor to the origin defined using the Edit-Set Origin command.

Procedure:	Choose a document window, then choose Edit-Jump-Current Origin.

See also:	Edit-Set Origin


Jump New Location
Jump-New Location

Shortcut keys:

Summary:	Moves the cursor to new X and Y coordinates.

Procedure:	Choose a document window, then choose Edit-Jump-New Location and follow the prompts.


Jump Design Rule Violation
Jump-Design Rule Violation

Shortcut keys:

Summary:	Moves the cursor to any clearance violation displayed on the DRC layer.

Procedure:	Make sure that the DRC layer is activated (Options-Layers command). Choose a document window, then choose Edit-Jump-Design Rule Violation and follow the prompts. Remove the violation and choose this command again to jump to another violation. If no violations are present the system will beep.


Set Origin

Summary:	Defines a location as the new origin and resets its coordinates to X0 Y0.

Procedure:	Choose a document window. Choose Edit-Set Origin, then choose the location for the new current origin.

See also:	Jump-Current Origin


Reset Origin

Summary:	Resets the default origin to the absolute 0, 0 coordinate at the extreme lower left corner of the workspace window.

Procedure:	Choose a document window. Choose Edit-Reset Origin.

See also:	Set Origin


Cross Probe Part On Schematic

Summary:	Moves the focus to the schematic sheet for the current PCB workfile and displays the part that corresponds to the designated PCB component.

Procedure:	Choose a document window. Choose Edit-Cross Probe Part On Schematic, then choose the component.

See also:	Jump-To Component


Cross Probe Pin On Schematic

Summary:	Moves the focus to the schematic sheet for the current PCB workfile and displays the part and pin that corresponds to the designated PCB component pad.

Procedure:	Choose a document window. Choose Edit-Cross Probe Pin On Schematic, then choose the component and pad.

See also:	Jump-To Pad


Cross Probe Net On Schematic

Summary:	Moves the focus to the schematic sheet for the current PCB workfile and displays a net identifier that corresponds to the designated PCB net.

Procedure:	Choose a document window. Choose Edit-Cross Probe Net On Schematic, then choose a pad connected to the desired net.

See also:	Jump-To Net


Component Libraries

Libraries in Advanced PCB, are collections of component foot prints (patterns). Each pattern is made up of a collection of items such as tracks, pads, fills etc. The process of creating a component is very simple.

First:	Place down all the items you want in the component, not forgetting to number any pads using the Change-Pad command.

Then:	Select all the primitives using the Select All command. Cut or Copy the selected items into the clip board.

Finally:	Choose  Library-Components, select the library you wish to add to, and choose new to Add the selected primitives  to the library.


Library Components
Library-Components

Shortcut keys:

Summary:	Allows creation, management, and browsing of pattern libraries.

Procedure:	Choose Library-Components. The Options are:

Add:	Adds an additional library to the current list. The library file extension will be forced to LIB.

Create:	Creates a new (and empty) library, When the command is complete, the new library will added to the current list.

Remove:	Removes the highlighted library from the current list of open libraries.

Compact:	When you delete a component from the library, a gap is left in the library file, fragmenting it. This gap is not closed after every deletion (this would make the process very slow). This command will sort the library and remove any fragmentation.

New:	Adds all selected primitives to the selected library as a new component.

Delete:	Deletes a component pattern stored in the library. (You cannot undo this).

Rename:	Changes the name of a component pattern stored in a library.

Place:	Places the highlighted component into the active PCB workspace.

Add All...	Adds all the component patterns in the current (active) PCB file to a selected library. This provides a convenient method of building libraries from PCB files imported from other systems.

Place Whole...	Places one copy of each component in the selected library into the current PCB file. This option allows users to build a catalog of pattern shapes or to quickly scan the patterns in the library. When placed, the components will be stacked at one board location. Use Auto Place (Local placer) to quickly distribute the components within a pre-defined board outline.

Close:	Exits the Library Components browser.

Report:	Generates a Library Components report for the highlighted library.

Display:	Choosing this command will expand the dialog box. A window for viewing the components is shown together with zoom control buttons. From now on, as you select a component from the components list box, it will be drawn. You can zoom in and out using the Expand and Contract buttons. The XY coordinates displayed are the position of the cross hair in the center of the view window relative the reference point of the component.

See also:	Place-Component


Library Un-Group
Library-Un-Group

Shortcut keys:

Summary:	Returns a component to its free primitives.

Procedure:	Choose a document window. If the component is not on the Current Layer and is below other components, use the Current-Layer to choose the layer that contains the component. Now choose Library-Un-Group and choose the component.


Library Pad Types
Library-Pad Types

Shortcut keys:

Summary:	Allows generation and management of pad libraries.

Procedure:	Choose Library-Pad Types.

See also:	Current Pad Type

Pad Types


Library Apertures
Library-Apertures

Shortcut keys:

Summary:	Allows generation and management of aperture tables.

Procedure:	Choose a document window, then choose Library-Apertures.

The Options Are:

New	The program will ask you for a new draft code. When you have entered a valid new draft code, the Edit Apertures dialog box will open, allowing the parameters of the aperture to be defined.

Delete	Removes an aperture from the current aperture list.

Rename	Allows you to change the current draft code for the highlighted aperture.

Edit	Allows you to re-define the aperture parameters. See Edit Aperture

Load APT...	Choose Library-Aperture Load to load an aperture file to the current list. When typing the file name you can use masks and select from a list. Aperture files always have the extension APT. If you have made any changes to your current aperture list then save it before loading another list or you changes will be lost.

Create List...	Generates a new aperture list from the current PCB. Apertures will be defined for all primitives on the PCB and special use apertures will be created for use in generating Solder Mask, Paste Mask, Power Plane Drill Drawing and Drill Guide artwork. These special apertures will be generated whether or not these layers are used in the design. Users can remove un-used apertures from the list prior to generating Gerbers, if desired.

Clear All 	Choose Library-Aperture Clear to remove any details of apertures currently stored in memory. If you have made any changes to these, then save your aperture list first. No changes or deletions are made to any aperture files on you disk.

Close	When finished editing the current aperture list, choose Close.

Users can also define the maximum allowable aperture in the file (some photoplotters have aperture size limitations). You can also specify Relief aperture types (used to flash thermal reliefs on internal power plane layers) is these are supported by the target photoplotter. Contact your plotting bureau for details.

See also:	Apertures


Aperture Edit

To modify an existing aperture Choose Library-Aperture Edit and select the aperture to be edited from the displayed list of all apertures in the current list. The aperture parameters which can be changed are

Draft Code	This is the aperture name. It can be any code from D04 to D999.

Hole Size	This is the size of the hole in the center of the aperture image. For no hole set this to zero.

Shape	The options for shape are, circular, rectangular, Octagonal, rounded rectangular, cross hair target or moiré target.

X Size	This is the horizontal size of the aperture in mils (or millimeters). Any value up to 100000 can be used for this.

Y Size	This is the vertical size of the aperture in mils (or millimeters). Any value up to 100000 can be used for this.

Use For	This specifies whether the aperture can be used to draw (as when stroking tracks, flash pads or both (Any). Relief-type pads are special assignments for flashing thermal relief shapes on internal power planes. These must be pre-defined for the target plotter. Contact your photoplotting bureau for details.


Netlist Load
Netlist-Load

Shortcut keys:

Summary:	Opens a netlist, retrieves missing components from the parts libraries, and assigns thermal relief connections to the plane layers.

Procedure:	Choose a document window, use the Netlist-Power Planes  to assign nets to the plane layers as needed. Choose Netlist-Load.

See also:	Library-Components

Netlist-Clear

Netlist-Power Planes

Netlists


Netlist Clear
Netlist-Clear

Shortcut keys:

Summary:	Removes the netlist from memory.

Procedure:	Choose a document Window, then choose Netlist-Clear.

See also:	Netlist-Load

Netlist-Power Planes

Netlists


Optimize Net
Optimize-Net

Shortcut keys:

Summary:	Reorders the all netlist connections on a net. The sorting method is predefined using Netlist-Edit-Net command.

Procedure:	Choose a document window, then choose Netlist-Optimize-Net. Enter the name of the net or enter a question mark to choose from a list.

See also:	Optimize Methods

Netlist-Edit-Net


Optimize On Component
Optimize-On Component

Shortcut keys:

Summary:	Reorders the netlist connections on a Component. The sorting method is predefined using Netlist-Edit-Net.

Procedure:	Choose a document window. If the component is not on the Current Layer and is behind other components, use the current layer to choose the layer that contains the component. Now choose Netlist-Optimize-On Component and choose the component.

See also:	Optimize Methods

Netlist-Edit-Net


Optimize All
Optimize-All

Shortcut keys:

Summary:	Reorders all the netlist connections within the current document window. The sorting method is predefined using the Netlist-Design Rules  or the Netlist-Edit-Net.

Procedure:	Choose a document window, then choose Netlist-Optimize-All.

See also:	Optimize Methods

Netlist-Edit-Net


Show Connections On Net
Show Connections-On Net

Shortcut keys:

Summary:	Displays the unrouted ratsnest connections on a named net (only if unrouted).

Procedure:	Choose a document window, then turn on the Rats Nest layer using the Options-Layers. Choose Netlist-Show Connections-Net, then enter a net name or enter a question mark to choose from a list.

See also:	Options-Layers

Netlists


Show Connections On Component
Show Connections-On Component

Shortcut keys:

Summary:	Displays the unrouted Ratsnest connections on a component (only if unrouted).

Procedure:	Choose a document window then turn on the Rats Nest layer using the Options-Layers. Choose Netlist-Show Connections-On Component, then choose a component.

See also:	Options-Layers

Netlists


Show All Connections

Shortcut keys:

Summary:	Displays all unrouted ratsnest connections on all nets within the current document window (only if unrouted).

Procedure:	Choose a document window then turn on the Rats Nest layer using the Options-Layers. Choose Netlist-Show Connections-All.

See also:	Options-Layers

Netlists


Hide Connection

Shortcut keys:

Summary:	Turns off the display of a ratsnest connection.

Procedure:	Choose a document window. Choose Netlist-Hide Connections-Connection and choose a ratsnest connection.

See also:	Options-Layers

Netlists


Hide Connections On Net
Hide Connections-On Net

Shortcut keys:

Summary:	Turns off the display of the ratsnest connections on a net.

Procedure:	Choose a document window then choose Netlist-Hide Connections-Net. Enter a net name or enter a question mark to choose from a list.

See also:	Options-Layers

Netlists


Hide Connections On Component
Hide Connections-On Component

Shortcut keys:

Summary:	Turns off the display of ratsnest connections on a component.

Procedure:	Choose a document window. If the component is not on the Current Layer and is behind other components, use the current layer  to choose the layer that contains the component. Now choose Netlist-Hide Connections-On Component and choose a component.

See also:	Options-Layers

Netlists


Hide All Connections

Shortcut keys:

Summary:	Turns off the display of ratsnests connections on all nets within the current document window.

Procedure:	Choose a document window then choose Netlist-Hide Connections-All.

See also:	Options-Layers

Netlists


Netlist Edit Net
Netlist-Edit Net

Shortcut keys:	  or

Summary:	Modifies the attributes assigned to a net. These include Net Name, Routing Track Width, Routing Via Diameter, Optimize Method, and Routing Priority. The modifications can by applied globally to all other nets.

Procedure:	Choose a document window then turn on the Rats Nest layer using the Options-Layers. Display the ratsnest using the Netlist-Show-All command. Choose Netlist-Edit-Net, then choose a ratsnest connection or pad within the desired net. If the cursor is not over a pad or connection (ratsnest), a dialog box opens, allowing the user to specify the desired net.

See also:	Options-Layers

Netlists

Netlist-Show

Netlist-Hide


Netlist Identify
Netlist-Identify

Shortcut keys:

Summary:	Displays the net name for a chosen ratsnest connection.

Procedure:	Choose a document window then turn on the Rats Nest layer using the Options-Layers. Display the ratsnest using the Netlist-Show. Choose Netlist-Identify, then choose a ratsnest connection.

See also:	Options-Layers

Netlists

Netlist-Show

Netlist-Hide


Netlist Length
Netlist-Length

Shortcut keys:

Summary:	Displays the total length of all ratsnest connections within the current document window.

Procedure:	Choose a document window, then choose Netlist-Length.

See also:	Netlists


Netlist Add Nodes
Netlist-Add Nodes

Shortcut keys:

Summary:	Interactively adds a pad to an existing net. Updates the ratsnest display. Any connections to other nets from the pad are removed.

Procedure:	Choose a document window, then choose Netlist-Add Nodes. You will be prompted to name the net. Type ? to choose from all nets. You will then be prompted to choose a pad to add to the net.

See also:	Netlists

Netlist-Add Nets

Netlist-Delete Nodes

Netlist-Add/Modify Connections


Netlist Delete Nodes
Netlist-Delete Nodes

Shortcut keys:

Summary:	Interactively removes a connected pad from an existing net. Updates the ratsnest display.

Procedure:	Choose a document window, then choose Netlist-Delete Nodes. You will be prompted to choose a pad to remove from the net.

See also:	Netlists

Netlist-Add Nodes

Netlist-Delete Connections


Netlist Add Connections
Netlist-Add/Modify Connections

Summary:	Interactively adds connections to pads assigned to the same net. Updates the ratsnest display.  Allows the user to change the connection order (net topology) by removing, moving or adding new connections within the net.

Procedure:	Choose a document window, then choose Netlist-Add/Modify Connections. You will be prompted to name the net. Type ? to choose from all nets. All pads associated with the net will be highlighted.

1.	To select an existing connection, position the cursor over the connection (ratsnest) and click [image].

2.	To move the connection to a new pad, drag the ratsnest to the desired pad and click [image]. The connection will now be routed to that pad, changing the topology (or connection order) within the net. To restore the connection back to its original state, press [image] or [image].

3.	To add a connection, click [image] over any pad in the net, then drag the new ratsnest connection to any highlighted pad within the net.

4.	To delete a connection, first select it as in step 1, then press [image].

Only pads which are currently assigned to the net can be connected. If you "split" the net, by removing a connection, the DRC system will flag the split by highlighting the net/pads using the DRC Errors layer color assignment. Reconnecting the split portion back to the net will clear the DRC flag, returning the display to normal.

See also:	Netlists

Netlist-Add Nets

Netlist-Add Nodes

Netlist-Delete Connections


Netlist Delete Connections
Netlist-Delete Connectionss

Summary:	Interactively removes connections from the ratsnest display.

Procedure:	Choose a document window, then choose Netlist-Delete Connections. You will be prompted to choose a conneciton to remove from the display. Click on the ratsnest to remove the connection. If the connection has been partially routed, these tracks and vias will be removed, along with the ratsnest.

See also:	Netlists

Netlist-Add/Modify Connections

Netlist-Delete Nodes


Netlist Add Nets
Netlist-Add Nets

Summary:	Adds a net to the current (internal) netlist.

Procedure:	Choose a document window, then choose Netlist-Add Nets. You will be prompted to name the net. You can then add component pads to this new net, using the Netlist-Add Nodes command.

See also:	Netlists

Netlist-Add Nodes


Netlist Run ECO File
Netlist-Run ECO File

Summary:	Updates the current PCB file and netlist per changes documented in an .ECO file.

Procedure:	Choose a document window, then choose Netlist-Run ECO FIle. You will be prompted to name the ECO file from files with the extension .ECO. Logical and physical changes documented in the ECO file will be used to update the layout. See page 140 of the Advanced PCB Reference for a list of ECO system parameters.

See also:	Engineering Change Orders

Netlists


Netlist Generate
Netlist-Generate

Shortcut keys:

Summary:	Produces a netlist from the current document window. The netlist produced by this method has no connection with the netlist loaded from a net file. It is purely based on the electrical connection between component pads, based on the physical layout of the board. You can use this method to get a netlist from a manually routed file (for later submission to an autorouter for example).

Procedure:	Choose a document window, then choose Netlist-Generate.


Netlist Export
Netlist-Export

Shortcut keys:

Summary:	Produces a netlist from the current document window. The netlist produced by this method is purely base on the loaded nets. Physical tracks, vias etc. are not considered. If you have deleted some components, then any nodes in a net that referred to that component, will not be written with the netlist.

Procedure:	Choose a document window, then choose Netlist-Generate.


Netlist Design Rule Check
Netlist-Design Rule Check

Shortcut keys:

Summary:	Produces a design rule check report and displays the areas of violation. The rules are predefined using the Netlist-Design Rules. The types of violations that are reported may be defined.

Procedure:	Choose a document window, then use the Netlist-Design Rules to set clearances. Choose Netlist-DRC, set the report options and use the OK button.

Notes regarding Design Rule Checks

DRC uses an external netlist. This means that changes made to the connectivity of the design, reflected in the current ratsnest display, are not regarded by DRC. DRC should be normally be regarded (see the exception below) as a final check of the design per the original (or updated) netlist.

DRCs can be used to document changes in an orderly way. Re-loading an earlier version of a netlist will generate a report of logical (not physical) changes to the design.

If you plan to place polygon planes (poured copper), you may wish to run DRC prior to generating these complex planes, which will slow down DRC. Because these planes are auto-generated, you do not have to worry about clearance violations.

Note: DRC use is particularly memory intensive. When Windows resources are limited, general memory errors can occur. We recommend that you maximize available resources prior to running DRC if you are experiencing Windows memory errors. Adding memory to your system should allow you to DRC larger designs without these problems.

See also:	Netlist-Clearances


Netlist Clearance Check
Netlist-Clearance Check

Shortcut keys:

Summary:	Displays any clearance violations on DRC layer.

Procedure:	Make sure that the netlist for the current project is loaded. Choose Netlist-Clearance Check. The DRC layer will be automatically activated and any violations will be displayed on this layer. Correcting the volations will remove the violation from the DRC layer. Use the Edit-Jump-Design Rule Violation command to toggle through all violations.

See also:	Netlist-Design Rule Check

 	Jump-Design Rule Violation

Netlist-Clearances


Netlist Reset DRC Error Markers
Netlist-Reset DRC Error Markers

Summary:	Removes DRC violations from DRC layer display.

Procedure:	Choose Netlist-Reset DRC Error Markers.

See also:	Netlist-Design Rule Check

 	Jump-Design Rule Violation


Netlist Clearances
Netlist-Clearances

Shortcut keys:

Summary:	Allows definition of clearances for routing and design rule checking.

Procedure:	Choose Netlist-Design Rules.

See also:	Netlist-Design Rule Check


Netlist Power Planes
Netlist-Power Planes

Shortcut keys:

Summary:	Removes or assigns nets to any of four internal power plane layers. Pins on these nets are automatically assigned to the plane, with the specified connection method, direct to the solid copper or relief connection, which thermally isolates the pin during wave soldering.

Procedure:	Choose a document window, then choose Netlist-Power Planes and Disconnect Net From Plane, Relief Connect to Plane 1, etc., Direct Connect to Plane 1, etc. You will be prompted to supply the net name. Pins for the specified plane are connected automatically and the display is updated to indicate these assignments. See pages 155 and 197 of the User Guide for more information about using power planes and plotting power plane artwork.

Split planes can be created by placing polygons on internal plane layers, with full preservation of net integrity and DRC functions.

See also:	Netlist-Load


Netlist Compare
Netlist-Compare

Shortcut keys:

Summary:	Prompts user to supply the name of two netlists. The netlists are compared and differences between the two nets are reported to the user.

Procedure:	Choose Netlist-Compare. You will be prompted to supply the name for two nets.


Auto Place

Shortcut keys:

Summary:	Arranges parts within an area outlined on the Keepout layer.

Procedure:	Choose a document window. Use the Netlist-Load to load the netlist and retrieve the components, then choose Auto-Auto Place.

See also:	Netlist-Load

Auto Placement


Auto Placement

Auto Placement Theory

Advanced Placer

Additional Comments on the Advanced Placer

Placement Tools


Auto Placement Theory

Placement is a critical process in manufacturing a PCB. The success in manufacturing is almost completely dependent on a good placement technique.

Placement involves specifying the exact location and orientation of each component on the PCB, given the board size and the area of the board on which placement is permissible.

The most important objective in placement, after the fitting of all the components on the board without violating any design rules, is to make the job of routing easier or, in most cases, possible.

There is also one more consideration which is not as critical as the others, and this is the aesthetics of the board.

In short, the main goals in placement of a PCB are :

Fitting all the components on the board.

Allowing no design rules violations.

Creating a routable board.

Creating a board with a good aesthetics.

See also:

Theory of optimization

Global and Local Optimizations

Optimization for Automatic Placement


Theory of optimization

Optimization is a formal technique used by mathematicians to find the extremes of a function. In mathematical terms this problem can be stated as follows:

Given the function f(x) with x belonging to the set s and s being the set of all the possible x's find a w from the set s for which f(w) is a maximum (or a minimum).

Solving this problem has turned out to be one of the most difficult areas in mathematics. The complexity of this problem is governed by the type of the function, and the size and dimension of s.

There are hosts of different techniques developed by mathematicians and other scientists to solve this problem. Most of them, however, only work on a small subset of the real-world problems.

If f(x) is an analytical function, using differential calculus maxima and minima of f(x) can be found. This method is the fastest in terms of the computational time required. Moreover it always guarantees a solution can be found. For most real-world problems f(x) is not an analytical function and consequently this method can not be used.

One optimization technique which is almost diametrically opposite to the analytical method, uses an exhaustive search to find the solution. What exhaustive search means, is to try all the possible x's and pick the one which gives the maximum for the function (or the minimum). This method also guarantees to produce the best solution. By contrast, it can be applied to any problem regardless of the type of the function with the heavy price of needing some geological time to carry out the computations involved for most of the real-world problems.

Although the real-world problems seem to be almost impractical for the optimization techniques to tackle they have, however, one major handy attribute which allows us to successfully apply an optimization technique to a real-world problem.

That attribute is that in a real-world problem, often we are not after the maximum or minimum, rather an approximation to them. In other words, we are not after the x which  gives the maximum (or the minimum), rather an x which produces a high enough (or low enough in case of minimization) value for f which can satisfy the problem in hand.

This aspect of the real-world problems has given rise to a spectrum of different techniques in between the two extremes, i.e. the analytical and the exhaustive search methods. Most techniques in that range make a compromise between the computational time and the quality of the approximation. they generally attempt to find a good solution by searching a very small subset of the set of all possible points in the solution space. The criteria by which a small subset is selected for search is the most intriguing part of optimization problem, and often the cause of diversity in the methods of optimization.


Global and Local Optimizations

Approximation of a solution is a very loose goal when we do not have any idea about the solution. How can we approximate a number when we do not know anything about the magnitude of that number? All we know is, "the higher the better"(or "the lower the better" in the case of minimization). The answer to this is that most of the optimization techniques only find the best out of the ones which have been tried, and that, they only try the ones which are expected to make an improvement . A method like this can, in no wise, claim to be able of  finding one of the best solutions. This problem is commonly known as the problem of Local Maxima  (or Local Minima in the case of minimization).

An analogy to this is the case of a blind man wanting to get to the highest point in a valley. Starting from a random point on the valley, he only moves to a direction where he can ascend. It is obvious that the chances for this poor man to get to the highest point in that valley is very small. In fact, a small hill which happens to be near his starting point can fool him and drag him to its top and making him believe he can not get any higher, as there is no point near by the top of that hill which is of a higher altitude. The techniques exhibiting this or similar kind of problems are commonly referred to as local optimization or greedy methods. By contrast the methods which find one of the best solutions are commonly referred to as global optimization methods.


Optimisation for Automatic Placement

Note: the level of auto placement available in Advanced PCB depends upon the license: in the standard (or Professional PCB) package, no placer is available; in Advanced PCB, the standard auto placer is available; if you have purchased the Advanced Place option, the intelligent placer can be activated.

Developing a Function for the Problem

Choosing an Optimization Technique

Simulated Annealing Method of Optimization


Placement Function
Developing a Function for the Problem

In order to apply optimization to the problem of automatic placement we first need to define a function which can measure the goodness of a placement job. In this case our variable x is a proposed placement job and s is the set of all the possible placements. It is obvious what the next move is.

We use a suitable optimization method to find the placement which gives us a high value of goodness.

This function, depending on a particular method of optimization employed, is referred to as the Cost Function, Objective function, evaluation function, fitness evaluator, etc. We have used the term Routing-Difficulty Function.

This function measures the following :

- Connection length.

- Connection density on the board.

- Component's alignment.

- Design rules violations.

Our goal is to minimize this function.

It is very important to realize that the overall success of an optimization technique is highly dependent on how good this function models the actual problem.


Optimization Techniques

Now we have to choose an optimization technique which results in success. Our policy is to find a global solution rather than a local one. In the context of that blind man we want to get to the highest point or some point very close to the highest. This means we have to employ a global optimization technique in order to minimize the Routing-Difficulty function.

There are only a few global optimization techniques and almost all of them have been developed very recently. Amongst them are the simulated annealing method, simulated evolution method and genetic algorithms. These methods all, have received inspiration from nature as their names suggest. In the annealing process of a metal, atoms array themselves in a way that crystals of low energy are formed. In natural evolution, only those species which are of better fitness survive and in genetics through cross-over and mutation, on average, better chromosome are produced from generation to generation.

The optimization technique which was chosen, was the Simulated Annealing method.


Simulated Annealing
Simulated Annealing Method of Optimization

In a metal raised to a temperature above its melting points, the atoms are in violent random motion. As with all physical systems, the atoms tend toward minimum energy state (a single crystal in this case), but at high temperatures the vigor of atomic motion prevents this. As the metal gradually cooled, lower and lower energy states are assumed until finally the lowest of all possible states, global minimum.

A simple way of describing the application of this to the PCB placement problem is to consider each component as a metallic atom during the annealing process. Now all we need is some artificial temperature, base on which, we can control the random movements of components. Starting at a high temperature, allowing components to move freely, we gradually drop the temperature and thereby applying some loose restriction on the moves. As the temperature drops lower we apply more restriction until we get close to the freezing point around which only moves which result in improvements are allowed.


Advanced Placer

The first thing that could be said, in describing the Advanced PCB advanced placer is that it is easy to use. Despite the underlying complexity, the Advanced PCB placer appears quite simple to the eyes of the user. All the user needs to know, before he or she runs the placer, is some very basic facts about the design. The user at no time needs to ever worry about configuring the placer. The placer has been finely tuned over a wide spectrum of boards for an optimal performance.

Setting Up the Advanced Placer

Pre-placing Components

Board Area for Placement

Advanced Placer Window

Advanced Placer Results

Background Running


Auto Place Setup

To set up the advanced placer, the user needs to run the Autoplace Set Up Command. Advanced PCB responds by displaying the Autoplacement Dialogue Box. The following information is needed by the placer:

- The Placement Grid Size.

- The allowable Clearance for small components.

- The allowable Clearance for large components.

- The names of the power and ground nets. (if used)

The power and ground nets are required by the placer in order to detect the by-pass capacitors. The by-pass capacitors are not directly placed by the advanced placer. The placer allows some space for the by-pass capacitors on top of each chip on the board.

There are four options in the Autoplace Set Up Dialogue Box, they are:

Local Placement

Global Placement

Component Rotation

Grouping


Local Placement

The Local Placement option is an independent greedy Auto placer. It is an improved version of the Protel Autotrax Auto placer.


Global Placement

The Global Placement option is the Advanced PCB advanced placer.


Auto Place Grouping

The Grouping option, if enabled, causes the placer to go through all the components on the board and group together all the components which are tightly connected. The placer then performs a relative placement on each group. These groups are treated by the placer as super components and their relative placement is kept untouched during the main placement cycle.

This option is generally useful. It could be counter productive if there is not going to be enough space on the board. This is so because the relative placement within each group is not changed during the main placement cycle and the placer might waste some space in order to accommodate the group.


Board Area for Placement

This can be done by putting tracks in the keep-out layer. If there is no track found in the keep-out layer, the entire area of the board is assumed. To disallow placement on any particular area on the board, area fills in the keep-out layer can be used.


Advanced Placer Window

The advanced placer has its own window. When running, it displays the current state of the board. It draws the rats nets, components and the keep-out areas (any of them can be set, using the display menu. ) The size of the components displayed includes the clearances specified in the Autoplace Dialogue Box. The main menu for the advanced placer is very short. The only specific options in the main menu are the Display and the Update PCB option in the File menu.

The advanced placer has its own data structure. This means the PCB is not changed normally during the placement. The user, however, can update the PCB to the most current state of the board by selecting the Update PCB option in the File menu.

The placement window has its own status bar, within which, the following information is available :

Elapsed time	Time since start of placement.

Optimization	There are a total of 70 cycles in any placement task. The first 40-50 cycles are very fast as most moves are accepted. However, as the temperature decreases, more and more moves are made in order to satisfy the requirements of a cycle. This means the cycles get slower towards the completion. Optimization refers to the percentage of completion toward an ideal set of costs.

Number of Moves	The Number of Moves, displayed in the status bar, is the total number of times that the placer has moved a component to a new position in order to improve the routability of the board.


Advanced Placer Results

Before the placer starts to run, the user is asked to provide a  name for the PCB file for saving the placement results. The placer, at the completion, updates the current PCB and saves the PCB in the file whose name was provided by the user at the start of the placement.


Auto Place Background Running

One interesting feature of the Advanced Placer is that it runs in the background. While placement is in progress, the user can work on another PCB or run another application. The user can not, however, run the placer for the second time in the same application. To have two placements running at the same time, the user needs to run a

second copy of the main application. The user, while the placer is in progress, can not close the PCB window or close the application. Once the placement is finished a dialogue box appears to inform the user of the completion of the placement.


Additional Comments on the Advanced Placer

The Advanced Placer is highly robust and generally does not require any special direction by the user. However, should any difficulty arise, the following points could provide useful information.

Pre-placing Components

Use of the keep-out Area Fills

Rotation Option

Grouping Option

Large nets slow down the placer


Preplacing Components
Pre-placing Components

The user can pre-place any component before running the Advanced Placer. The placer leaves untouched all the components that are specified by the user as being pre-placed. In order to specify that a component has been pre-placed, the Place Status of that component  needs to be set  to 'Locked in Place'. This can be done through the Change-Component Command. The Place Status for all the other components needs to be set to 'Free to Move'.

Apart from those components which have to be placed on certain locations on the board, such as edge connectors and heat sinks, etc., sometimes it is useful to pre-place a component which has no restriction on its placement. For example, it might be desirable to pre-place the memory chips. This could facilitate the placement of the other components. In the case of a group of analog components connected together, it again might be beneficial to pre-place them.


Auto Place Keep Outs
Use of the keep-out Area Fills when auto placing

This could be very useful when it comes to routing. It is advisable, in most cases, to put keep-out area fills all around the board. This will give some open space for the router to go around. It is also good to put keep-out area fills next to connectors and some pre-placed components.


Auto Place Rotation

The Component Rotation option only applies to the Global Placement, where as the Grouping option applies to the both Auto placers.

If component rotation is allowed, the Advanced Placer rotates components in order to find an optimal orientation. It only considers four orientations, namely, 90,180,270 and 360 degrees.

The Rotation option can sometimes make the placement task more difficult. Rotation in general requires more board space. Therefore, in those boards where there is not going to be a lot of open space, rotation could be counter-productive. On the other hand, if the board space is large the rotation option can be highly useful.


Auto Place Large Nets

Large nets slow down the placer. The reason for this is the computation involved with the rearranging of a net, is exponentially proportional to the net size. An interesting observation is the insignificant role of these large nets in the overall placement. Therefore it could be advantageous to hide the large nets from the placer. To do this one can either save the net-list, remove the large nets, run the placer and at the end reload the original net-list, or assign some of the large nets to the power and ground planes and thus hide them from the placer. When supplied by the user, the power and ground nets are not passed to the placer, as power and ground nets are usually connected to most of the components.


Placement Tools menu

Shortcut keys:	  or

Summary:	The outcome of the Advanced Placer is a board, in which, the relative positions of the components are optimal. Due to its global nature, the Advanced Placer often produces boards which are not entirely polished. For instance, there could still be some overlaps  after the placement is completed, or some components might not be aligned properly. These anomalies need to be removed. The placement tools are specifically designed to facilitate this phase.

Spread Horizontal

Spread Vertical

Align Left

Align Right

Align Top

Align Bottom

Center On Horizontal

Center On Vertical

Align Component

Expand Horizontal

Expand Vertical

Contract Horizontal

Contract Vertical

Shove

Set Shove Depth


Auto Place Spread Horizontal
Placement Tools-Spread Horizontal

Shortcut keys:

Summary:	Spread out selected components horizontally.

The Placement Grid can be set to a new value in the Autoplace Dialogue Box.

Procedure:	De-Select any selected components.

Select the components to spread and choose Auto-Placement Tools Spread Horizontal.

The selected components will be spread evenly horizontal.

See also:	Selection

Auto Placement


Auto Place Spread Vertical
Placement Tools-Spread Vertical

Shortcut keys:

Summary:	Spread out selected components vertically.

Procedure:	De-Select any selected components.

Select the components to spread and choose Auto-Placement Tools Spread Vertical.

The selected components will be spread evenly vertically.

See also:	Selection

Auto Placement


Auto Place Align Left
Placement Tools-Align Left

Shortcut keys:

Summary:	Move all selected components to align with the left hand side of a chosen component.

Procedure:	De-Select any selected components.

Select the components to align and choose Auto Placement Tools Align Left.

You will be asked to choose a component. The one you choose will be used as the reference and all the other selected components will be move to align with its left hand side. No Vertical movement will be made.

See also:	Selection

Auto Placement


Auto Place Align Right
Placement Tools-Align Right

Shortcut keys:

Summary:	Move all selected components to align with the right hand side of a chosen component.

Procedure:	De-Select any selected components.

Select the components to align and choose Auto Placement Tools Align Right.

You will be asked to choose a component. The one you choose will be used as the reference and all the other selected components will be move to align with its right hand side.

No Vertical movement will be made.

See also:	Selection

Auto Placement


Auto Place Align Top
Placement Tools-Align Top

Shortcut keys:

Summary:	Move all selected components to align with the top of a chosen component.

Procedure:	De-Select any selected components.

Select the components to align and choose Auto Placement Tools Align Top.

You will be asked to choose a component. The one you choose will be used as the reference and all the other selected components will be move to align with its top.

No horizontal movement will be made.

See also:	Selection

Auto Placement


Auto Place Align Bottom
Placement Tools-Align Bottom

Shortcut keys:

Summary:	Move all selected components to align with the bottom of a chosen component.

Procedure:	De-Select any selected components.

Select the components to align and choose Auto-Placement Tools Align bottom.

You will be asked to choose a component. The one you choose will be used as the reference and all the other selected components will be move to align with its left hand side.

No horizontal movement will be made.

See also:	Selection

Auto Placement


Auto Place Center On Horizontal
Placement Tools-Center On Horizontal

Shortcut keys:

Summary:	Move all selected components to align their centers on a horizontal line which passes through the center of a chosen component.

Procedure:	De-Select any selected components.

Select the components to align and choose Auto-Placement Tools Center On Horizontal.

You will be asked to choose a component. The one you choose will be used as the reference and all the other selected components will be moved so as to align their centers on a horizontal line which passes through the center of the reference.

See also:	Selection

Auto Placement


Auto Place Center On Vertical
Placement Tools-Center On Vertical

Shortcut keys:

Summary:	Move all selected components to align their centers on a vertical line which passes through the center of a chosen component.

Procedure:	De-Select any selected components.

Select the components to align and choose Auto-Placement Tools Center On Vertical.

You will be asked to choose a component. The one you choose will be used as the reference and all the other selected components will be moved so as to align their centers on a vertical line which passes through the center of the reference.

See also:	Selection

Auto Placement


Auto Place Align Component
Placement Tools-Align Component

Shortcut keys:

Summary:	Moves individual components to align relative a "master" component. Works independently of the current selection status of components.

Procedure:	1.	Choose Auto Placement Tools Align Component.

You will be prompted to choose a master component. The one you choose will be used as the reference and all the other selected components will be moved relative its position.

2.	Click to choose the master component. This component will now move freely  with the cursor.

3.	If desired, reposition the master component and click [image] once. To cancel the move click [image] once.

The status line prompt changes to, "Select a component to be aligned TOP (BOTTOM, VERTICAL, HORIZ., LEFT, RIGHT)."

4.	Choose a component to be aligned with the master. To change modes press T for Top, B for Bottom, V for Vertical Center, H for Horizontal center, L for Left or R for Right.

The target component will be aligned with the master component, per the current mode (Top, Bottom, etc.) In other words, if the alignment mode is Top, the component will move from its current position, to vertically align its top with the master.

This target component will now be free to move on the "unconstrained" axis. In the above example, where Top is the alignment mode, you will be able to move the component left or right, if desired, after the tops are aligned. If the mode is H (for horizontal center) the component will move freely up or down, while remaining at the horizontal center of the master.

Components will be aligned whether or not they are part of the current selection.

5.	When the desired components are aligned, press [image] or [image].

You will be prompted to select another master component, allowing you to repeat the process. Press  [image] or [image].again to cancel the procedure.

See also:	Selection

Auto Placement


Auto Place Expand Horizontal
Placement Tools-Expand Horizontal

Shortcut keys:

Summary:	Move selected components  apart horizontally so as to increase the spacing between them by one Autoplace grid point.

Procedure:	De-Select any selected components.

Select the components to expand and choose Auto-Placement Tools Expand Horizontal.

The selected components will be move apart horizontally so as to increase the spacing between them by one Autoplace grid point.

See also:	Selection

Auto Placement


Auto Place Expand Vertical
Placement Tools-Expand Vertical

Shortcut keys:

Summary:	Move selected components  apart vertically so as to increase the spacing between them by one Autoplace grid point.

Procedure:	De-Select any selected components.

Select the components to expand and choose Auto-Placement Tools Expand Vertical.

The selected components will be move apart vertically so as to increase the spacing between them by one Autoplace grid point.

See also:	Selection

Auto Placement


Auto Place Contract Horizontal
Placement Tools-Contract Horizontal

Shortcut keys:

Summary:	Move selected components closer together horizontally so as to decrease the spacing between them by one Autoplace grid point.

Procedure:	De-Select any selected components.

Select the components to expand and choose Auto-Placement Tools Contract Horizontal.

The selected components will be moved closer together horizontally so as to decrease the spacing between them by one Autoplace grid point.

See also:	Selection

Auto Placement


Auto Place Contract Vertical
Placement Tools-Contract Vertical

Shortcut keys:

Summary:	Move selected components closer together vertically so as to decrease the spacing between them by one Autoplace grid point.

Procedure:	De-Select any selected components.

Select the components to expand and choose Auto-Placement Tools Contract Vertical.

The selected components will be moved closer together vertically so as to decrease the spacing between them by one Autoplace grid point.

See also:	Selection

Auto Placement


Auto Place Shove
Placement Tools-Shove

Shortcut keys:

Summary:	Moves all components of a selected component. And then move components of the moved components.

Procedure:	The Shove command causes all the components which overlap the selected component to slide away and leave the selected component clear. It then attempts to shove all the slided components and so on.

It is not advisable to use the Shove command for intricate jobs as the 'Shove and Push' process involved could upset the overall placement. The scope of the Shove command, however, can be limited by setting the Shove Depth to a small value. Shove Depth can be set through the Set Shove Depth command.

For example, if the Shove Depth is set to 1, only the selected component is cleared - the components which were cleared off the selected components are not shoved again.

Although setting the Shove Depth high is dangerous to the layout, you can use the Undo and Redo commands to recover from any unintended result.


Auto Place Set Shove Depth
Placement Tools-Set Shove Depth

Shortcut keys:

Summary:	Used to limit the scope of the shove depth command.

Procedure:	Choose Auto-Auto Place Set Shove Depth. Enter a number greater or equal to 1. This is the depth of expansion. If this is set to 2 for example, the chosen component will move all the components on it. The moved components will move all the components on them.

See also:	Auto Place-Shove


Auto Move To Grid
Auto-Move To Grid

Shortcut keys:

Summary:	Moves each free to move component to the nearest location that will align its reference point with the grid.

Procedure:	Choose a document window. Choose Auto-Move To Grid, choose a grid, or choose other to enter another value.


Auto Density

Shortcut keys:

Summary:	Temporarily displays a map of the ratsnest connection density.

Procedure:	Choose a document window. If a netlist is not loaded, use Netlist-Load. Choose Auto-Density.

This is a relative color display. Red is the most dense area, and green is the least dense area.

See also:	Netlist-Load


Auto Manual Route
Manual Route

Shortcut keys:

Summary:	Places tracks interactively using a ratsnest connection or re-routes a previously routed connection, removing old tracks. A netlist must be loaded for the PCB in order to display the connections (Netlist-Show Connections command).

Procedure:	To manually convert a connection to a series of tracks and vias, choose Manual from the router command menu and select a connection to work on. The cursor will jump to the nearest end of the connection. Manual routing works in a very similar way to the Place-Track command, except that as you lay tracks you will see a rubber band line from the current cursor position to the other end of the connection.

You can use the [image] [image] and [image] keys to change layers and vias will be inserted automatically as you go.

Press [image] or [image] to place a track section. When you are ready to place the last section (and complete the connection), press [image] or [image] A track section will run from the current cursor position to the end of the connection.

You can manually route another, or Press  [image] or [image] to finish manual routing.

You can re-route an existing routed connection by clicking on any track segment. A ratsnest connection will be displayed from the cursor position to the next pad in the net. You can then route the remainder of the connection, as above. You can terminate the re-route either at the pad or at any track point between the current cursor position and the pad. If you terminate at any point on a track, the re-route will break, and connect to the track at that point. Any loop is "disused" track will be removed.

Vias will be placed automatically, if you toggle layers during the routing. If the cursor is on a multilayer pad and you toggle layers, the pad will be used to connect on the new layer and no via will be placed.


Autoroute All
Auto Route-All

Shortcut keys:

Summary:	Routes all connections on all nets within the current document window.

Procedure:	Select Auto-Autoroute All, the route status dialog will appear and the router will attempt to route all the unrouted connections on the board.

See also:	Autorouting


Autoroute Net
Auto Route-Net

Shortcut keys:

Summary:	Automatically routes a net.

Procedure:	To select a net and autoroute all the connections on it, choose Auto-Autoroute Net. Click directly on the ratsnest connection or a pad within the net to start routing from that point. If you click in a location that is not a connection or pad, you will be prompted to supply a net name. Type in the net name, or press [image] to select from the dialog box list. All currently selected routing passes will be tried on all the unrouted connections in the selected net.

See also:	Autorouting


Autoroute Connection
Auto Route-Connection

Shortcut keys:

Summary:	Automatically routes a ratsnest connection.

Procedure:	To select individual connections and autoroute them, choose Auto-Autoroute Connection. When prompted, select a connection. All currently selected routing passes will be tried on the connection.

See also:	Autorouting


Autoroute On Component
Auto Route-On Component

Shortcut keys:

Summary:	Automatically routes all ratsnest connections on a component.

Procedure:	To select a component and autoroute all the connections on it, choose Auto-Autoroute On Component Select a component. All currently selected routing passes will be tried on all the connections that go to that component (not nets, just individual connections).

See also:	Autorouting


Autoroute Selected_Components
Auto Route-Selected Components

Shortcut keys:

Summary:	Automatically routes all ratsnest connections on a group of selected components.

Procedure:	Select a group of components. Choose Auto-Autoroute Selected Components. All currently selected routing passes will be tried on all the connections that go to that component. Individual connections only are routed -- the balance of any nets will be left un-routed.

See also:	Autorouting


Autoroute Pad to Pad
Auto Route-Pad To Pad

Shortcut keys:

Summary:	Automatically routes tracks between two pads. This autorouting function does not require a netlist.

Procedure:	Choose Auto-Autoroute Pad to Pad. Select 2 pads and the router will attempt to route them. The maze router is not used by this pass.

See also:	Autorouting


Autoroute Advanced Route Connections

Shortcut keys:

Summary:	Automatically routes tracks in a connection using the Advanced Route passes. The Advanced Route option must be enabled to use this command.

Procedure:	Choose Auto-Autoroute-Advanced Route Connections. Select a connection and the Rip-up Maze router will attemp to complete the route.

See also:	Autorouting


Setup Auto Route

Shortcut keys:

Summary:	Defines use of autorouting algorithms and attributes.

Procedure:	Choose Auto-Setup Autorouter. The autorouter setup dialog box will appear. Use these options to set the routing layers, routing passes and router variables.

See also:	Autorouting


Un-Route All
Un-Route-All

Shortcut keys:

Summary:	Removes all tracks and vias on all valid netlist connections within the current document window.

Procedure:	Choose a document window, then choose Auto-Un-Route All.

See also:	Autorouting


Un-Route Net

Shortcut keys:

Summary:	Removes all free primitives on all valid netlist connections on a net.

Procedure:	To select a net and un-route all the connections on it, choose Auto-Un-Route Net. Click directly on the ratsnest connection or a pad within the net. If you click in a location that is not a connection or pad, you will be prompted to supply a net name. Type in the net name, or press [image] to select from the dialog box list..

See also:	Autorouting


Un-Route Connection
Un-Route-Connection

Shortcut keys:

Summary:	Removes all free primitives on a valid netlist connection.

Procedure:	Choose a document window. Choose Auto-Un-Route Connection, then choose a free primitive.

See also:	Autorouting


Un-Route Track
Un-Route-Track

Shortcut keys:

Summary:	Converts a single routed track segment back into an un-routed connection, with ratsnest display. The track must have connection information (e.g. a netlist must be loaded for the project and the track must have been placed by the autorouter or Auto-Manual Route command).

Procedure:	Choose a document window. Choose Auto-Un-Route Track, then click on a routed track segment. You can continue to rip-up segments one-at-a-time, providing that they are contiguous. A connection cannot be broken at two locations (e.g., at either end) at the same time. As you un-route individual segments, obsolete vias are removed.

See also:	Autorouting


Un-Route On Component

Shortcut keys:

Summary:	Removes free primitives on valid netlist connections on a component.

Procedure:	Choose Auto-Un-Route On Component, then choose a component.

See also:	Autorouting


Un-Route Selection
Un-Route-Selection

Shortcut keys:

Summary:	Removes all selected free primitives on valid netlist connections within the document window.

Procedure:	Choose a document window. Use Edit-Select and Edit-De-Select as necessary, then choose Un-Route Selection.

See also:	Selection

Edit-Select

Edit-De-Select

Autorouting


Current Pad Type
Current-Pad Type

Shortcut keys:	  or [image] +

Summary:	Defines the pad attributes that will be in effect during subsequent pad placements.

Procedure:	Choose Current-Pad Type.

This command allows you to pick one of the pad types from the current pad type list. When you place a pad, this pad type will be placed.

The current pad type is also displayed on the status line.

See also:	Library-Pad Types


Current Track
Current-Track

Shortcut keys:

Summary:	Defines the track width that will be in effect during subsequent manual track placements.

Procedure:	Choose Current-Track, choose a track width, or choose Other to enter another value between .001 and 9999.999 mils. This value is the width of tracks placed with the Place-Track Command. The current track width is also displayed on the status line.


Current Via Diameter
Current-Via Diameter

Shortcut keys:

Summary:	Defines the via diameter that will be used during subsequent manual via placements, and manual routing.

Procedure:	Choose Current-Via Diameter, choose a size or choose Other to enter another value.

See also:	Current-Via Hole Diameter

Current-Via Type


Current Via Hole Diameter
Current-Via Hole Diameter

Shortcut keys:

Summary:	Defines the via hole diameter that will be used during subsequent manual via placements, and manual routing.

Procedure:	Choose Current-Via Hole Diameter, choose a size or choose Other to enter another value.

See also:	Current-Via Diameter

Current-Via Type


Via Type

Shortcut keys:

Summary:	Defines current default via as either Through Hole or Blind/Buried. This type of via will be in effect during subsequent manual via placements and manual routing.

Procedure:	Choose Current-Via Type and either Through Hole or Blind/Buried.


Component Text Comments

Shortcut keys:

Summary:	Defines the component comment attributes that will be in effect during subsequent component placements.

Procedure:	Choose Current-Component Text Comments.

This dialogue box controls the settings used for displaying the text of component comments after they have been placed.

All these options are defaults, you can change them later using the move and change commands.

The Options Are:

Layer:	Component designators can be either copper (on the top layer for a top layer component) or overlay (on the top overlay for a lop layer component).

Height:	The height of the designators displayed letters (in mils or millimeters).

Font:	The displayed text of the designator or comment  can be displayed in any one of the system fontsFonts available.

Hide Status:	The show attribute can be set to either Hidden or Show. If hidden, then the text will not be shown on either the screen or on subsequent plots. Note that no information is lost by showing or hiding the designator, and that it can be changed at some later time.

Vertical Align:	Controls the vertical position of the text relative to the component.

Horizontal Align:	Controls the Horizontal position of the text relative to the component.

See also:	Current-Component Text Designators


Component Text Designators

Shortcut keys:

Summary:	Defines the component designator attributes that will be in effect during subsequent component placements.

Procedure:	Choose Current-Component Text Designators.

This dialogue box controls the settings used for displaying the text of component designators after they have been placed.

The options are:

Layer:	Component designators can be either copper (on the top layer for a top layer component) or overlay (on the top overlay for a lop layer component).

Height:	The height of the designators displayed letters (in mils or millimeters).

Font:	The displayed text of the designator or comment  can be displayed in any one of the system fontsFonts available.

Hide Status:	The show attribute can be set to either Hidden or Show. If hidden, then the text will not be shown on either the screen or on subsequent plots. Note that no information is lost by showing or hiding the designator, and that it can be changed at some later time.

Vertical Align:	Controls the vertical position of the text relative to the component.

Horizontal Align:	Controls the Horizontal position of the text relative to the component.

See also:	Current-Component Text Comments


Free Text Height

Shortcut keys:

Summary:	Defines the text height that will be in effect during subsequent placements of free text.

Procedure:	Choose Current-Free Text Height, choose a size or choose Other to enter another value between  36 and 4000 mils.


Free Text Font

Shortcut keys:

Summary:	Defines that the font in effect during subsequent placements of free text will be the internal Advanced PCB font.

Procedure:	Choose Current-Free Text Font Default, Serif or Sans Serif.


Current Snap Grid
Current-Snap Grid

Shortcut keys:

Summary:	Defines the alignment grid for manual movement and placement of objects.

Procedure:	Choose a document window. Choose Current-Snap Grid, then choose a size or choose Other to enter another value.

See also:	Snap Grid


Current Visible Grid 1
Current-Visible Grid 1

Shortcut keys:

Summary:	Defines the first display grid.

Procedure:	Choose Current-Visible Grid 1, then choose a size or choose Other to enter another value.

See also:	Visible Grid


Current Visible Grid 2
Current-Visible Grid 2

Shortcut keys:

Summary:	Defines the second display grid.

Procedure:	Choose Current-Visible Grid 2, then choose a size or choose Other to enter another value.

See also:	Visible Grid


Current Layer
Current-Layer

Shortcut keys:

Summary:	Displays and changes to a layer, even if display is toggled off.

Procedure:	Choose a document window. Choose Current-Layer, then choose a layer.

Any layer can be selected. If you select a layer that is toggled off, then it will be turned on. The current layer is displayed on the Tool Bar, together with a color box to help you identify which items are on the layer. When you use the edit, move, delete or other design commands, the current layer is the layer searched first  during selections. You can change layers at any time during editing (except when menus or dialogs are on the screen) with the [image], [image] or [image] keys.  switches to the next signal layer that is turned on.  and [image] move down and up through the turned on layers respectively.

See also:	Options-Layers

Layer and Display Colors


Layer and Display Colors

The Color that layers are displayed in is controlled by the Layers dialog box from the options menu.

Some of the specialized settings are:

Back Ground:	The physical background Color.

Connections:	The Color of the rats nest. Connections are generated, from the net list, by the netlist optimize command.

DRC Errors:	Primitives that have failed clearance checks made by DRC are drawn outlined in this color.

Selection:	All highlighted items are drawn outlined in this Color.

Grid Color 1, 2:	The colors of the 2 Visible Grids. These are only display if the lines will be 5 or pixels apart.


Options Layers
Options-Layers

Shortcut keys:

Summary:	Toggles layer display and defines colors.

Procedure:	Choose a document window, then choose Options-Layers.

Transparent	You can make selected display layers Transparent (color and gray scale displays only) rather than solid color. This makes identification of overlapping objects easier when several layers are active at the same time. However, transparent colors will make screen redraw significantly slower. So you may wish to leave this option off, until needed during the final clean-up of the board.

Dithered	Dithered colors are created by mixing two solid colors. Leave this option off if you want to display solid colors only. This can be helpful if you are displaying primitives in Draft mode (Options-Display command).

All Layers Off	Provides a shortcut for turning all the layers off in one-step.

Used Layers On	Restores the layer selections to include all the layers in the current PCB file.

All Layers On	Activates every layer with a single command.

Current Layer On	Activates the Current layer. Leaves other layer selections undisturbed.

Preview mode

Preview mode minimizes the amount of vector information which must be re-drawn as you change your view of the screen. To invoke this mode, choose Options-Layers then select the Current Layer Only or All Layers Off button. When active, this option displays one layer at a time.

When toggling layers (*, + or - key) only the current layer is displayed, with the following exceptions:

Signal layers are displayed with the Multi-layer (through-hole pads) visible.

Mechanical Layers are displayed with the current layer if they have been specified in the Output Options dialog box.

See also:	Layer and Display Colors

Setting up the workspace layers


Setting up the workspace layers

Normally you will want to start a new project by selecting the layers needed for the design. In PCB this will include the signal (or Copper Trace) layers, Internal Power Plane layers, Mechanical layers, Silkscreen Overlay layers, and Special layers used to display details of your design.

Before we can access any of these layers, the layer must be turned "On". Once a layer is active, it will be displayed or edited:

To activate and setup layers:

1.	Choose the Options-Layers command  to open the Setup Layers & Colors dialog box;

Note how the layout and display layers are grouped by layer type. Some layers correspond directly to the tooling of the board, like the Copper Trace layers. Other layers are provided for display or output purposes.

For each of the layers on the printed circuit board there is a check box which you can click ( [image]) to turn the layer on or off, just to the left of the layer name. An "X" in the box indicates that a layer is active.

The default active layers will be updated when you Exit PCB. Any layers that you have activated will be active the next time you start the PCB application. When you load a PCB file, all layers used in the design are automatically activated.

2.	Click in the layer check boxes to activate the required layers.

To assign colors to activated layers:

1.	Choose the Options-Layers command to open the Setup Layers & Colors dialog box;

2.	Click in the color box, to the right of the layer name to open the Color Selector box;

The color currently assigned to the layer is displayed in the left pane of the Color/Solid box. The Solid color (right hand pane) is the color assignment used if the Dithered Colors option is not selected (Dithered colors are colors derived by mixing two solid colors). Depending upon your graphics card and display type, you can choose from up to 233 solid or dithered colors plus a user-defined palette of 16 custom colors.

3.	Click in one of the color boxes to re-set the layer assignment;

4.	Click in the Solid (right) pane to make the solid color equivalent the assignment;

5.	Click OK to accept the assignment or Cancel to exit the Color Selector without changing the layer color.

You may wish to use all solid colors if you are displaying primitives in Draft display mode. This is because the primitives will be rendered in lines of one pixel  (screen picture element) width. Dithering will obscure the lines with many color combinations.

Preview mode

Preview mode minimizes the amount of vector information which must be re-drawn as you change your view of the screen. To invoke this mode, choose Options-Layers then select the Current Layer Only or All Layers Off button. When active, this option displays one layer at a time.

When toggling layers (*, + or - key) only the current layer is displayed, with the following exceptions:

Signal layers are displayed with the Multi-layer (through-hole pads) visible.

Mechanical Layers are displayed with the current layer if they have been specified in the Output Options dialog box.

See also:	Customizing Colors


Customizing Colors

In addition to the 233 pre-defined colors from the Color Selector dialog box, users can also define a custom palette of colors using RGB (Red/Green/Blue) balues between 0 and 255 units. This custom palette is stored with the PCB file defaults, between editing sessions:

1.	Double-click on any color in the Setup Layers (Options-Layers command) to open the Color Selector.

To customize a color:

2.	Click on one of the custom color boxes;

3.	Set the individual RGB values between  0 and 255 units;

4.	Click OK to accept the assignment or Cancel to exit the Color Selector.

As you make color assignments, it is important to make sure that your assignments don't conflict in some way that will obscure vital details when you edit your layout. It is recommended that you start with the Background and Selections assignments (Special layers), if you wish to change a number of the defaults.

Remember, some layers may only need to be displayed during printing or plotting (or plot file generation) For example, the Solder or Paste masks can be left "off" unless you are editing or plotting these layers. The more layers displayed, the slower the screen will re-draw.

Although several layers can be "active" and displayed simultaneously, only one layer can be the "current" layer. Single layer items such as tracks, fills, arcs or text are always placed on the current layer. The current layer color (or pattern) is displayed in the Layer box at the left of the title bar and the layer name is displayed (along with the filename, if any) in the title bar.

See also:	Color assignments


Color assignment
Color assignments

On the bottom of the Set-up Colors dialog box is another command for setting the specific color to the full 24 bit resolution of Windows. If your system supports 256 colors then your palette on will be re-set to display as many available solid colors as possible when you close the Setup Layers dialog box.

Windows reserves the first 20 colors in the palette for its own system use. When using applications that take advantage of 256 color palettes, use of more than the standard 20 Windows default colors may cause "stealing" of colors from the system or from other applications. For example, if you have a bit-map as your background for Windows which used 256 colors then the quality of the display of the bit-map will deteriorate as you select more colors for Advanced PCB.

On 16 color VGA systems, all 16 colors are set by Windows for the system palette, which cannot be re-programmed by the user. On EGA systems there are only 16 (from a 64 palette) colors, so the quality of the standard windows display is poor and no reprogramming is possible.


Options Preferences
Options-Preferences

Shortcut keys:

Summary:	Defines various system settings. These options affect all document windows.

Procedure:	Choose a document window, then choose Options-Preferences.

User defined options include:

Auto Pan

Auto Via

Question Delete

Clean Redraw

Select Hidden

Snap to Center

Lock Cursor

Drag Tracks

Dynamic Reconnect

Save Defaults

Dots for Grids

Online DRC

Loop Removal

Rotation Step Size

Auto Backup

Board Cursor

Engineering Change Orders

Automatic Report Editing

Automatic Report Editing


Clean Redraw option

This option gives the user the choice of detailed re-draws (Clean Redraw enabled) or less-detailed redraws (disabled). When this option is disabled, the system response is generally faster, as less detailed redraws are performed, but the display may become untidy when moving or deleting items. When disabled, redraws are performed on the changed item only. Clean redraws redraw all primitives in the modified area, in their proper display order. Zooming or panning as you work will also redraw the effected area. To manually update the display, use the Zoom-Redraw command (or Redraw tool button).

See also:	About Version 2.0


Engineering Change Orders

This option specifies the filename for .ECO (Engineering Change Order) files and allows the user to enable/disable the system. The ECO system records changes to the physical/logical design and can be used to update the design from an externally modified .ECO file using the Netlist-Run ECO File command. The ECO file format is compatible with the PADS ECO system.

See also:	About Version 2.0

Netlist-Run ECO File


Auto Backup option

This option allows the user to pre-define the time interval for generation of Auto Backup files. These files a created using the extension AB0, AB1, etc. When AB9 is reached, the cycle returns to AB0, etc. To disable the Auto Backup feature, type 0 (zero) into the Time Between Backups text box.


Rotation Step Size option

This option allows the user to define the amount of clockwise rotation applied to a primitive, component or selection being moved, when the [image] is pushed. Default setting is 90 degrees.

Warning:	There are limitations to the rotation of components with pad shapes other than round. To rotate components to other than 90, 180, 270 or 0 degrees, first convert the pads to round shapes.

See also:	About Version 2.0


Online DRC option

When this option is enabled (Options-Preferences dialog box), Advanced PCBs Online Design Rule Check feature is activated. This system detects clearance violations as you edit the PCB and signals violations by highlighted the clearance area around the offending primitives. Move either primitive to remove the violation condition and reset the highlight. You can also reset all collision highlights using the Netlist-Reset DRC Error Markers command.

See also:	About Version 2.0


Dots for Grids option

When this option is enabled, the visible grid will be displayed using dots, rather than solid grid lines.


Save Defaults option

When this option is enabled (Options-Preferences dialog box), user defaults and settings will be saved in the .PCB and .INI files. See page 220 of the Advanced PCB Reference for a detailed listing of .INI file contents.


Lock Cursor option

When this option is enabled (Options-Preferences dialog box), the workspace cursor will be linked with the logical (Windows) cursor, which continuously update the status line coordinates.

When this option is disabled, the cursor can be used to access menu commands, without losing the current workspace position. You can press [image] or [image] to update the cursor coordinates.


Snap to Center option

When this option is enabled (Options-Preferences dialog box), the cursor will automatically jump to the center of a pad, track or other primitive when using a Move command or shortcut. When moving a component, the cursor will jump to the reference point designated for the component (often the center of pin 1 or the geometric center of the component outline). When moving text strings, the cursor will jump to the lower left corner of the string.

When this option is disabled, the cursor will maintain its relative position to the item being moved.


Draft/final Mode

Tracks, Arcs, Fills, Pads, Strings or Vias, can be drawn as hollow, solid or hidden. If hidden, they will not be displayed. Hidden items cannot be selected unless the Select Hidden option is enabled in the Options-Preferences dialog box.


Cursor Shape
Board Cursor

Choose Options-Preferences to select the type of cursor to use for editing in the work space. Options are Large Cross, Small Cross (default) and (small) 45 degree Cross. This does not affect the Windows (arrow) cursor which is used choosing menu commands and dialog box options.


Component Track Drag Mode

This option controls what happens to tracks connected to a component when the component is moved, If set, when you select a component to move, all of the tracks connected to it will be dragged, maintaining orthogonal connections. Tracks that run under the component (on different layers) will be dragged as well. This is to minimize unintended track crossing (shorting-out).

Note: This option does not work with the Move-Selection command


Auto Pan

Options-Auto Pan controls what happens when the working cursor reaches the window edge (while selecting or dragging an item). If enabled, the screen will move toward the cursor and redraw with the cursor re-centered in the workspace. Holding the SHIFT key when panning will move the display at 5X the normal rate.

See also:	Zoom menu


Auto Via Insertion

When this option is enabled, Advanced PCB will automatically place a via where the tracks change layers. This option works when using the Place Track command to route without a netlist  or when using the Auto-Manual Route command to route netlisted (ratsnest) connections.


Delete Confirmation

Every time you delete an item, the program will ask for confirmation. To control this option, choose Options-Preferences and Check or Un-Check then Delete Confirmation check box.


Select Hidden Primitives
Select Hidden

When using the Edit-Select or De-Select-Inside Area command, primitives whose display status is Hidden are included by default. Disabling this option will exclude hidden items from selections.


Loop Removal

When enabled, this option removes duplicate track segments (loops) when using the Auto-Manual Route command to re-route existing netlisted connections.


Dynamic Reconnect

When enabled, this option updates the ratsnest display while using the Auto-Manual Route command. As a connection is being routed, the ratsnest connection dynamically re-connects to the nearest pad on the current net, irrespective of the connection order in the netlist and the existing netlist display.


Automatic Report Editing

The user can pre-define the target application for CSV and Protel (text) reports. This application will automatically launch when a report is generated and the report file will be opened.

For example, CSV files are generated when the File-Reports-Bill of Materials (or BOM) command is chosen. A CSV (comma separated value) compatible editor (such as a spreadsheet or database application) can be specified in this field. When a BOM is generated, the specified application will launch, displaying the BOM.


Options Display
Options-Display

Shortcut keys:

Summary:	Defines display attributes for each type of primitive. Three modes allow displaying, not displaying, or displaying primitives as outlines. These attributes affect all document windows.

For pads, the Name and Net Name of the pad can also be displayed.

Procedure:	Choose a document window, then choose Options-Display.


Track Mode Any Angle

Shortcut keys:

Summary:	Changes the manual track placement mode to permit track placement at any angle.

Procedure:	Choose a document window, then choose Options-Track Mode Any Angle.


Track Mode 90/90 Line

Shortcut keys:

Summary:	Changes the manual track placement mode to permit track placement at only 90 degree angles.

Procedure:	Choose a document window, then choose Options-Track Mode 90/90 Line.


Track Mode 45/90 Line

Shortcut keys:

Summary:	Changes the manual track placement mode to permit track placement at either 45 or 90 degree angles.

Procedure:	Choose a document window, then choose Options-Track Mode 45/90 Line.


Track Mode 90 Arc/Line

Shortcut keys:

Summary:	Changes the manual track placement mode to permit track placement at 90 degree angles or arcs.

Procedure:	Choose a document window, then choose Options-Track Mode 90 Arc/Line.


Options Tool Bar
Options-Tool Bar

Shortcut keys:

Summary:	Toggles the Tool Bar display on or off.

Procedure:	Choose Options-Tool Bar.


Options Status
Options-Status

Shortcut keys:

Summary:	Toggles the Status Line display on or off.

Procedure:	Choose Options-Status.


Options Scroll Bars
Options-Scroll Bars

Shortcut keys:

Summary:	Toggles the Scroll Bars display on or off.

Procedure:	Choose a document window, then choose Options-Scroll Bars.


Options Toggle_Units
Options-Toggle Units

Shortcut keys:	  or press

Summary:	Toggles the current measurement system units between imperial (mils) and metric (mm).

Procedure:	Choose Options-Toggle Units.


Options Memory Monitor
Options-Memory Monitor

Shortcut keys:	  or press

Summary:	Allows user to define thresholds for memory use; monitors memory use from inside Advanced PCB; alerts user when available memory decreases below pre-set limits.

Procedure:	Choose Options-Memory Monitor.


Zoom Window
Zoom-Window

Shortcut keys:

Summary:	The region chosen within two opposite corners is displayed to fill the document window.

Procedure:	Choose a document window. Choose Zoom-Window and follow the prompts.

See also:	Zoom-Point


Zoom Point
Zoom-Point

Shortcut keys:

Summary:	The region chosen by a center point and a corner is displayed to fill the document window.

Procedure:	Choose a document window. Choose Zoom-Point and follow the prompts.

See also:	Zoom-Window


Zoom Select
Zoom-Select

Shortcut keys:

Summary:	The display magnification of the chosen document window is changed to reflect a chosen value. The range of values is 1 to 400. 1 is the most zoomed in.

Procedure:	Choose a document window. Choose Zoom-Select and Choose a magnification level or choose other to enter another value.


Zoom All
Zoom-All

Shortcut keys:	  or [image] +

Summary:	The region defined by objects at the highest and lowest coordinate points is displayed to fill the current document window. In order to utilize this feature with a new document, you must first use the Info-Board command.

Procedure:	Choose a document window, then choose Zoom-All.


Zoom In
Zoom-In

Shortcut keys:	  or

Summary:	Increases display magnification in the current document window to the next higher default value.

Procedure:	Choose a document window, then choose Zoom-In.


Zoom Out
Zoom-Out

Shortcut keys:	  or

Summary:	Decreases display magnification in the current document window to the next lower default value.

Procedure:	Choose a document window, then choose Zoom-Out.


Zoom Pan
Zoom-Pan

Shortcut keys:	  or

Summary:	Redraws the current document window with the previous cursor location at the center of the window.

Procedure:	Choose a document window, then choose Zoom-Pan.


Zoom Redraw
Zoom-Redraw

Shortcut keys:	  or

Summary:	Redraws the current document window.

Procedure:	Choose a document window, then choose Zoom-Redraw.


Info System Status
Info-System Status

Shortcut keys:

Summary:	Displays disk and memory status.

Procedure:	Choose a document window, then choose Info-System Status.


Info Board Status
Info-Board Status

Shortcut keys:

Summary:	Displays the quantity of components and primitives within the current document window.

Procedure:	Choose a document window, then choose Info-Board Status.


Info Components on PCB
Info-Components on PCB

Shortcut keys:

Summary:	Displays a list of placed components within the current document window.

Procedure:	Choose a document window, then choose Info-Components on PCB. To save the list, double click on any component in the list. Enter a valid filename to save the list as an ASCII file or enter the DOS reserved name PRN and the list will be dumped directly to the printer port.

The format is:	U1 (74LS123) Designator (Type/Value/Comment)


Info Selected Pins
Info-Selected Pins

Shortcut keys:

Summary:	Displays the component and pin designators of selected pins within the current document window.

Procedure:	Choose a document window, then choose Info-Selected Pins. To save the list, double click on any pin name in the list. Enter a valid filename to save the list as an ASCII file or enter the DOS reserved name PRN and the list will be dumped directly to the printer port.

The entries are sorted by component designator first and pad designator second.

The format is:	U1-16 Component designator - Pad designator


Info Nets
Info-Nets

Shortcut keys:

Summary:	Displays the names of nets within the current document window.

Procedure:	Choose a document window, then choose Info-Nets. To save the list, double click on any net name in the list. Enter a valid filename to save the list as an ASCII file or enter the DOS reserved name PRN and the list will be dumped directly to the printer port.


Info Measure Distance
Info-Measure Distance

Shortcut keys:

Summary:	Displays the distance between two chosen points.

Procedure:	Choose a document window. Choose Info-Measure Distance and follow the prompts.

X-Distance and Y-Distance measurement to the dialog box. Three measurements are displayed: (For example)

Distance Measured = 82.462Mil (the point-to-point distance)

X Distance = 80Mil

Y Distance = 20Mil


Info Length of Selection
Info-Length of Selection

Shortcut keys:

Summary:	Displays the total physical connection length of selected primitives within the current document window.

Procedure:	Choose a document window. Use Edit-Select and Edit-De-Select as necessary, then choose Info-Length of Selection.

See also:	Edit-Select

Edit-De-Select

Selection


Power Planes Plane 1
Power Planes-Plane 1-4

Shortcut keys:

Summary:	Displays the designators of all pins with direct or thermal relief connections on Plane 1 within the current document window.

Procedure:	Choose a document window, then choose Info-Power Planes-Plane 1. To save the list, double click on any pin name in the list. Enter a valid filename to save the list as an ASCII file or enter the DOS reserved name PRN and the list will be dumped directly to the printer port.

Split planes can be created by placing polygons on internal plane layers, with full preservation of net integrity and DRC functions.


Power Planes Plane 2
Power Planes-Plane 1-4

Shortcut keys:

Summary:	Displays the designators of all pins with direct or thermal relief connections on Plane 2 within the current document window.

Procedure:	Choose a document window, then choose Info-Power Planes-Plane 2. To save the list, double click on any pin name in the list. Enter a valid filename to save the list as an ASCII file or enter the DOS reserved name PRN and the list will be dumped directly to the printer port.

Split planes can be created by placing polygons on internal plane layers, with full preservation of net integrity and DRC functions.


Power Planes Plane 3
Power Planes-Plane 1-4

Shortcut keys:

Summary:	Displays the designators of all pins with direct or thermal relief connections on Plane 3 within the current document window.

Procedure:	Choose a document window, then choose Info-Power Planes-Plane 3. To save the list, double click on any pin name in the list. Enter a valid filename to save the list as an ASCII file or enter the DOS reserved name PRN and the list will be dumped directly to the printer port.

Split planes can be created by placing polygons on internal plane layers, with full preservation of net integrity and DRC functions.


Power Planes Plane 4
Power Planes-Plane 1-4

Shortcut keys:

Summary:	Displays the designators of all pins with direct or thermal relief connections on Plane 4 within the current document window.

Procedure:	Choose a document window, then choose Info-Power Planes-Plane 4. To save the list, double click on any pin name in the list. Enter a valid filename to save the list as an ASCII file or enter the DOS reserved name PRN and the list will be dumped directly to the printer port.

Split planes can be created by placing polygons on internal plane layers, with full preservation of net integrity and DRC functions.


Window Tile
Window-Tile

Shortcut keys:

Summary:	Displays all non-minimized document windows without overlapping.

Procedure:	Choose Window-Tile.


Window Cascade
Window-Cascade

Shortcut keys:

Summary:	Arranges all document windows and overlaps all except the title bars.

Procedure:	Choose Window-Cascade.


Window Arrange Icons
Window-Arrange Icons

Shortcut keys:

Summary:	Arranges all document icons across the lower portion of the application window.

Procedure:	Choose Window-Arrange Icons.


Window Close All
Window-Close All

Shortcut keys:

Summary:	Closes all Document windows and icons, prompting to save any modified documents.

Procedure:	Choose Window-Close All.

See also:	File-Save, File-Save As


Help Index
Help-Index

Shortcut keys:	  or

Summary:	Displays a list of help topics, these offer access to all areas of the help system.

Procedure:	Choose Help-Index.


Help Using Help
Help-Using Help

Shortcut keys:

Summary:	Displays information about using the help system.

Procedure:	Choose Help-Using Help.


Help Basic Concepts
Help-Basic Concepts

Shortcut keys:

Summary:	Displays an index of basic operation topics, these offer access to detailed information about Advanced PCB techniques.

Procedure:	Choose Help-Basic Concepts.


Help Commands
Help-Commands

Shortcut keys:

Summary:	Displays the Advanced PCB Commands index, these offer access to detailed information about each command.

Procedure:	Choose Help-Commands.


Help Printing
Help-Printing

Shortcut keys:

Summary:	Displays an index of printing topics, these offer access to detailed information about printing and plotting.

Procedure:	Choose Help-Printing.


Help Managing Files
Help-Managing Files

Shortcut keys:

Summary:	Displays an index of file management topics, these offer access to detailed information about using file in Advanced PCB.

Procedure:	Choose Help-Managing Files


Help Screen Regions
Help-Screen Regions

Shortcut keys:

Summary:	Displays an index of screen area topics, these offer access to detailed information about using the Advanced PCB interface.

Procedure:	Choose Help-Screen Regions


Help Reference
Help-Reference

Shortcut keys:

Summary:	Displays an index of reference topics, these offer access to detailed information about these topics.

Procedure:	Choose Help-Reference.


Help About
Help-About

Shortcut keys:

Summary:	Displays the application name and version number.

Procedure:	Choose Help-About.


Tool Bar

The tool bar, when displayed, appears below the menu bar. It contains buttons and tools to speed up many of the most frequently performed Advanced PCB operations.

Toggle the tool bar off and on by choosing Options-Toolbar. Click on each button for a description:

bmc bttn020.bmp}


File-Open command

Opens a PCB file in its own window.


File-Save command

Saves the contents of the current PCB file window.


File-Print command

Prints the contents of the current PCB file window.


Zoom-All command

Redraws the display to include all the current PCB window contents.


Zoom-Window command

Prompts the user to define a new display window area, then redraws the display.


Zoom-Redraw command

Updates the screen display without changing the zoom level or center location.


Edit-Cut command

Removes all selected items from the document window; places selection into clipboard.


Edit-Paste command

Adds the current clipboard contents to the current PCB window.


Edit-Select-Inside Area command

Prompts user-defined selection rectangle; items that fall entirely inside rectangle are added to selection.


Edit-De-Select-All command

Removes everything from the current selection.


Edit-Move-Selection command

Allows the user to move the current selection to a new location in the workspace.


Current-Snap Grid  command

Pops-up menu for assigning the current snap grid value.


Edit-Place-Arc command

Initiates arc placement (by center) sequence; current track width value is used as the default arc width.


Edit-Place-Component

Initiates sequence to place a component footprint in the current PCB window.


Edit-Place-Fill command

Initiates sequence to place a rectangular area fill on the current layer.


Edit-Place-Pad command

Initiates free pad placement on current layer; uses the current pad type as the default pad.


Edit-Place-String command

Initiates text string placement on the current layer using current font and string size as default.


Place-Track command

Initiates sequence to place a track segment on the current layer. Current track width is the default track.


Place-Via command

Initiates sequence to place a free via on the current layer. Current via type is the default via.


Place-Array command

Opens the Place-Array dialog box.


Auto-Manual Route command

Interactively routes/re-routes a connection.


Netlist-Add/Modify Connections command

Adds or deletes connections associated with a net.


Auto-Align Components command

Aligns two or more components.


Library-Components command

Opens the Library-Components dialog box


File-Run Schematic command

Launches Protel Advanced Schematic, if included in the current DOS PATH statement.


Edit-Undo command

Removes the effect of the last edit.


Edit-Redo command

Restores the effect of the last Undo.


Help-Contents command

Launches the Advanced PCB On-line Help system.


Window Sizing Border

The border around a window that mouse users can drag to change the window's shape and size.

Drag the top, bottom, or side border to size in one direction only.

Drag a corner of the border to size in two directions at once.

You can also size a window by using the Control Size command.


Application Window Control menu

Restore	Restores the active window to its former size and location.

Move	Displays a four-headed arrow you can use to reposition the active window or an open dialog box that has a Control menu.

Size	Displays a four-headed arrow you can use to change the size of the active window.

Maximizev	Enlarges the active window to fill the available space.

Close	Closes the active window or an open dialog box that has a Control menu.

Switch To	Lists all currently open applications and activates the one you select. This command appears only on the application Control menu.

Minimize	Reduces the application window to a small icon at the bottom of the screen.


PCB Window Control menu

Restore	Restores the active PCB window to its former size and location.

Move	Displays a four-headed arrow you can use to reposition the active window or an open dialog box that has a Control menu.

Size	Displays a four-headed arrow you can use to change the size of the active window.

Maximize	Enlarges the active PCB window to fill the available Application work space.

Close	Closes the active PCB window or an open dialog box that has a Control menu.

Next Window	Activates the next open PCB window.

Minimize	Reduces the PCB window to a small icon at the bottom of the screen.


Application Control menu Close

Closes the active application window or PCB Window. If a dialog box is open and has a Control menu, choosing this command closes the dialog box. For mouse users, double-clicking the Control menu icon is the same as choosing Control Close.

Closing the application window is the same as choosing File-Exit.

If you close a PCB Window, any other open windows for that PCB Window remain open

To close all open PCB Windows, use the Window-Close All command.

Shortcuts	+ [image] (closes PCB Window)

+ [image] (closes application window)


Application Control menu Maximize
Application Control menu Control Maximize

Enlarges the active window to fill the available space.

For mouse users, clicking the Maximize icon is the same as choosing Control Maximize.

Expands the Advanced PCB window to fill the entire screen.

Expands a PCB Window to fill the entire Advanced PCB workspace.

You can restore a maximized window to its former size by using the Control Restore command.

Shortcut	  (maximizes the PCB Window)


Application Control menu Minimize
Application Control menu Control Minimize

Reduces the Advanced PCB window to an icon at the bottom of the screen.

For mouse users, clicking the Minimize icon is the same as choosing Control Minimize.

Minimizing is useful when you are running another application at the same time as Advanced PCB.

You can restore a minimized window to its former size by using the Control Restore command.


Application Control menu Move
Application Control menu Control Move

Displays a four-headed arrow you can use to move the active window.

If a dialog box is open and has a Control menu, you can also use this command to move the dialog box.

If the window is maximized, this command is unavailable.

Shortcut	+ [image] to move the PCB Window


Application Control menu Size
Application Control menu Control Size

Displays a four-headed arrow you can use to change the size of the active window.

If the window is maximized, this command is unavailable.

Shortcut	+


Application Control menu Restore
Application Control menu Control Restore

Restores the active window to the size and location it had before you chose the Control Maximize or the Control Minimize command.

With the mouse, click the Restore icon of the window you want to restore.

Does not affect changes made to a window with the Control Move or Control Size command.

Shortcut	  (restores PCB Window)


Application Control menu Switch To

Lists all the open applications.

Switch To	Activates the selected application.

End Task	Closes the selected application.

Cancel	Closes the Task List window.

Cascade	Sizes all open applications so they overlap and each title bar is visible.

Tile	Arranges all  open applications and sizes them so that they are all visible and do not overlap.

Arrange Icons	Arranges the icons of all minimized applications across the bottom of the screen.


Window Control menu Close
PCB Window Control Close

Closes the active application window or PCB Window. If a dialog box is open and has a Control menu, choosing this command closes the dialog box.

For mouse users, double-clicking the Control menu icon is the same as choosing Control Close.

Closing the application window is the same as choosing File-Exit.

If you close a PCB Window, any other open windows for that PCB Window remain open

To close all open PCB Windows, use the Window-Close All command.

Shortcuts	  (closes PCB Window)

  (closes application window)


PCB Control menu Maximize
PCB Window Control Maximize

Enlarges the active window to fill the available space.

For mouse users, clicking the Maximize icon is the same as choosing Control Maximize.

Expands the Advanced PCB window to fill the entire screen.

Expands a PCB Window to fill the entire Advanced PCB workspace.

You can restore a maximized window to its former size by using the Control Restore command.

Shortcut	   (maximizes the PCB Window)


PCB Control menu Minimize
PCB Window Control Minimize

Reduces the Advanced PCB window to a small icon at the bottom of the screen.

For mouse users, clicking the Minimize icon is the same as choosing Control Minimize.

Minimizing is useful when you are running another application at the same time as Advanced PCB.

You can restore a minimized window to its former size by using the Control Restore command.


PCB Control menu Move
Window Control Move

Displays a four-headed arrow you can use to move the active window.

If a dialog box is open and has a Control menu, you can also use this command to move the dialog box.

If the window is maximized, this command is unavailable.

Shortcut


PCB Control menu Size
PCB Window Control Size

Displays a four-headed arrow you can use to change the size of the active window.

If the window is maximized, this command is unavailable.

Shortcut


PCB Control menu Next Window
PCB Window Control Next Window

Activates the next PCB Window .

Shortcut	+


PCB Control menu Restore
PCB Window Control Restore

Restores the active window to the size and location it had before you chose the Control Maximize or the Control Minimize command.

With the mouse, click the Restore icon of the window you want to restore.

Does not affect changes made to a window with the Control Move or Control Size command.

Shortcut	  (restores PCB Window)


Managing Files

Change the drive or directory

Change to a subdirectory of the current directory

To change to the parent directory of the current directory

Close the active PCB Window

View a list of files in a directory

View PCB files in a directory

View all files in a directory


To change the drive or directory

1.	Choose File-Open.

2.	In the File Name box, type the name of the drive or directory or both followed by *.*

3.	Choose OK.

4.	To close the dialog box, choose Cancel.


Change to a subdirectory of the current directory
To change to a subdirectory of the current directory:

1.	Choose File-Open.

2.	In the Directories box, select a subdirectory.

3.	Choose OK.

4.	To close the dialog box, choose Cancel.


Change the parent directory
To change to the parent directory of the current directory:

1.	Choose File-Open.

2.	In the Directories box, select "[..]".

3.	Choose OK.

4.	To close the dialog box, choose Cancel.


To close the active PCB Window
To close the active PCB Window:

1.	Choose File-Close. If there are no changes, the PCB Window is closed immediately. If there are unsaved changes, Advanced PCB asks if you want to save changes.

2.	Choose Yes to save changes, No to discard changes, or Cancel to cancel the command.

If the file hasn't been saved  before, the File-Save As dialog box is displayed.

3.	In the Save As box, type a name for the file or use the proposed name.

4.	Choose OK.

If the specified file already exists then you will be asked to confirm overwrite

5.	Choose Yes to continue, choose No to enter another name, or choose Cancel to cancel the command and return to the PCB Window.


To view a list of files in a directory
To view a list of files in a directory:

1.	Choose File-Open.

2.	In the File Name box, type a file specification.

It can include drive, directory, and the wildcard characters "?" (to match a single character) and "*" (to match any number of characters).

3.	Choose OK. The Files box displays the names of all files matching the file specification you type.

4.	When you have finished viewing the list, choose Cancel.


View PCB files in a directory
To View all PCB files in a directory

1.	Choose File-Open.

2.	In the File Name box, type *.PCB (asterisk, period, PCB).

3.	Choose OK.

4.	When you have finished viewing the list, choose Cancel.


View all files in a directory
To View all files in a directory:

1.	Choose File-Open.

2.	In the File Name box, type the name of the drive or directory or both followed by *.*

3.	Choose OK.

4.	To close the dialog box, choose Cancel.


Screen Regions

Control menu Icon

Maximize Icon

Minimize Icon

Restore Icon

Scroll Bar

Status Bar

Title Bar

Tool Bar

Window Sizing Border


Control menu icon

Mouse users can click the Application Control menu or PCB Window Control menu icons to display commands that control the size and position of the windows.

The Control menu icons are located at the left end of the title bar in the application and PCB windows.

See also:	PCB Window Control menu

Application Control menu


Restore icon

Mouse users can click the Restore icon to return a window to the size and location it had before it was sized.

Restoring an application window also restores any PCB Windows that are open within the application.

Clicking the Restore icon has the same effect as choosing the Control Restore command.

It does not affect changes made to a window with the Control Move or Control Size command.


Scroll bar

The shaded bars along the right and bottom sides of a window.

Mouse users can use the scroll bars to move through a PCB Window or Help topic.

The position of the scroll box in the scroll bar indicates the part of the PCB Window ,list or topic currently displayed in the window.

To scroll quickly to another part of the PCB Window or topic, drag the box.

To scroll one quarter of a window size in a given direction, click the arrow at that end of the bar.

To scroll one full window size in a given direction, click in the bar on that side of the scroll box.

To scroll past the area of the PCB Window you are currently using and view the entire

PCB Window, hold down [image] while you drag the scroll box.


Maximize icon

Mouse users can click the Maximize icon to enlarge a window to its maximum size.

A maximized PCB Window fills as much of the Advanced PCB window as possible and has no borders.

You can maximize the Advanced PCB window only if it is not full screen, or if it has been minimized to an icon.

Clicking the Maximize icon has the same effect as choosing the Control Maximize command.

To restore a maximized window to its former size, choose Control Restore.

With the mouse, click the Restore icon.


Minimize icon

Mouse users can click the Minimize icon to shrink the Microsoft Advanced PCB window to a small icon.

As an icon, the application remains in memory but does not take up room on your desktop.

When you minimize the Advanced PCB window, any open PCB Windows are minimized with it.

Clicking the Minimize icon has the same effect as choosing the Control Minimize command.

To restore the Advanced PCB window, and any PCB Windows that were open when you minimized it, choose Control Restore.

With the mouse, click the Restore icon.


Status bar

The status bar at the bottom of the screen displays information about the current activity or mode.

When a command is selected, the left side of the status bar briefly describes the chosen command.

The left side of the status bar also indicates the current cursor position.


Title bar

The bar across the top of a window that contains the window's name.

You can move a window by choosing the Control Move command from the PCB Window.

Mouse users can move the active window by dragging the title bar.

If a dialog box has a title bar, it can also be moved.


To increase memory

Use as many of the following procedures as practical. After each step below, you can try again to complete the task that requires more memory.

Quit any other applications you are running.

Choose File-Save All.

Close all windows except the active window.

In the Options-menu, turn off  Scroll Bars, Tool Bar, and status bar.

Quit, and then restart Windows and Advanced PCB.

As a last resort, quit Advanced PCB and Windows, then restart your computer. If possible, leave off networks, TSRs, and any other utilities you usually run.


Pad types

In Advanced PCB, each pad has all of its own details, size shape etc., stored with it. To avoid having to enter this information each time we place a pad, we use pad types and the current pad type list. This is a list of pad types, each with a name (Round50 for example), which is kept in memory. We can save this list to a pad type file and reload it later on. This allows us to build a library of pad types. For example we may keep a list of SMT pads, for use in designing SMT boards, and a list of standard multilayer pads for standard boards.

In the Library-Pads menu there are a series of commands to be used to Set-up, edit, load, save and generally control the use of pad types. When placing a pad we are using the current pad type (one of the pad types in the current list).

The pad type list, referred to in this section, is the list of pad types that are currently active. When the program starts up it attempts to load a pad type file called Advanced PCB.PAD. This contains a list of default pad types. To change the default list (the one loaded at the start) simply save your list to this file name.

New	To create a new pad type and add it to the current pad type list, choose Library-Pads New. The program will ask you for a new name. When you have entered a name, the program will move you to Edit-Pad type with a set of default pad type parameters.

Delete	If you wish to remove an unused pad type from the pad type list Choose Library-Pads Delete and select the pad type to be deleted from the displayed list of all current pad types.

Rename	Used to change the pad type identifier (ROUND50, etc.).

Edit	Allows the user to edit the Pad description. See Pad Type Edit.

Load	Choose Library-Pads Load to load a pad type file to the current list.

Pad type files always have the extension .PAD. If you have made any changes to your current pad type list then save it before loading another list or your changes will be lost.

Save	After you have changed the current pad type list (which is stored in memory) you will need to save it to disk to make the changes permanent. Choose Library-Pads Save to do this. The file name you specify will be forced to extension PAD. If the file already exists you will be given the option to over write it.

Merge	If you wish, you can copy a single pad type, from another pad type file, into the current list. To do this, choose Library-Pads Merge. Enter the name of the pad type file (as in Loading a list of pad types), then, when prompted, enter the name of the pad type to merge form the other file. When you have entered a name, the pad type is copied from the pad type file on disk to the list of pad types in memory.

Clear	Choose Library-Pads Clear to remove any details of pad types currently stored in memory. If you have made any changes to these, then save your pad type list first. No changes or deletions are made to any pad type files on you disk.

See also:	Editing a Pad type (above).


Pad Type Edit
Pads-Edit

To modify an existing pad type Choose Library-Pads Edit and select the pad type to be edited from the displayed list of all pad types in the current list. The pad type parameters which can be changed are

Name	A 10 character identifier, ROUND100, for example.

Hole Size	This is the size of the hole in the center of the pad type. For no hole (SMT or Edge connector) set this to zero.

Shape	The options for shape are, rectangular, octagonal and rounded.

X Size	This is the horizontal size of the pad type in mils (or millimeters). Any value up to 1000 can be used for this.

Y Size	This is the vertical size of the pad type in mils (or millimeters). Any value up to 1000 can be used for this.

Layer	This specifies whether the pad type is single layer (SMT or edge connector) or multilayer. Double sided edge connectors require two separate pads. For single layer pads, the actual layer (top or bottom) is not decided until the actual placement, where it takes on the current layer. Single layer pads can only be placed on the top or bottom layers.


Print

Introduction to Printing

Printer Setup

Generating Prints & Plots


Printing introduction

About pen plotting

A new Plot command (for pen plotting) has been added to the File menu for version 2.0, which by-passes the Windows plot drivers (and their associated limitations). We recommend that you use this option if you are plotting to a HPGL/DMPL-compatible (vector) pen plotter. See page 188 of the User Guide for details.

The updated pen plotter routines support HPGL (Hewlett Packard) and DMPL (Houston Instruments) plot languages, which are compatible with many plotter types. The generic use of these plot languages will be compatible with most plotter models that support these languages, although some specific features may not be available for a particular model. Setting up your plotter to support one of the available languages may be necessary. Consult your plotter documentation for details.

It is also possible to plot via the File-Print command, if your device is properly supported by the available Windows plotter drivers.

Microsoft Windows provides a set of raster and postscript printer drivers. These range from Epson 9 pin dot matrix printers to Linotronic high resolution raster image processors (photo-typesetters).


Printing

Note: Please see Introduction to Printing for information regarding improved Pen Plotting routines, added to version 2.0.

While the print is being generated, the status line will report the current completion. As each area on the board is printed, the screen display of that area will changed Color.

You can interrupt or pause the print at any time. Choose any key and a dialog box will open, allowing you to confirm the cancellation of the print job.

Pen Plotting

The File-Pen Plot command by-passes the Windows plot drivers (and their associated problems). We recommend that you use this option if you are plotting to an HP-GL or DMPL-compatible vector pen plotter.

To use this new plot routine, choose the File-Plot command.

When this command is chosen, a dialog box opens, presenting the plot options.

These routines support the HPGL (Hewlett Packard) and DMPL (Houston Instruments) plot languages which are compatible with many plotter types. The generic use of these plot languages will be compatible with most plotter models that support these languages, although some specific features may not be available for a particular model. Setting up your plotter to support one of the available languages may be necessary. Consult your plotter documentation for details.

It is also possible to plot via the File-Print command, if your device is properly supported by the available Windows plotter drivers. Many newer plotters are specifically supported by Windows drivers. Check with your plotter manufacturer for details.


File Printer Setup dialog box
Printer Setup dialog box

Select Printer	Select the printer you want to use. Only those printers installed in Windows appear. Use the Control Panel to add printers.

Batch Mode 	Choose Separate Page For Each Layer or Panels.

Options	Specify Border Between Sheets (clearance) for panelized prints and to set the minimum margin for the sheet. Enable the Show Holes option, if you wish to print pad and via holes as visual targets for manual drilling.

Scale 	Options include: Fit Layer on Page; Scale (range depends upon device specified) and Corrections (see below).

Corrections	These two values are multipliers for all co-ordinates sent to the printer. The X-correction is multiplied with all horizontal values and the y-correction is multiplied with all vertical values. Use these values to correct any linear errors in either axis of the printer. If you are only using the printer for check prints (not final artwork), then you can leave these set at 1x.


Photoplotting

Photoplotting Background

Gerber Photoplotter Language

Apertures

Photoplotter Setup

Photoplotting


Photoplotting background

All photoplotters print images directly onto photographic film. In this way they are closer to the desired result since no photo-reduction or further photography is required.

photoplotters fall into two classes :

Vector Plotters	These make images in much the same way as pen plotters. They select a drawing instrument (or aperture) and describe a vector in the drawing space. The result can be seen as flashes (filled arcs) and strokes (a line the width of which is defined by the aperture).

Raster Plotters	These work in much the same way as your screen, or a Laser printer. They construct a bit map image of the object to be printed. This bit map is then translated to the film by some form of optical scanner.


Gerber photoplotter language

It is a fact of evolution that nearly all photoplotters receive their commands in a vector based language developed by The Gerber Scientific Instrument Company. It is this fact which creates the few difficulties and limitations to be experienced by the photoplotting designer.


Apertures

Any given photoplotter supports a number of drawing tools or apertures. In the case of a vector plotter these apertures are real optical identities which are projected onto the film emulsion by the plotter's optical system. In the case of a raster plotter, the apertures are synthesized and represented by a bit map.

See also:	Using Apertures

Aperture Library


Aperture use

To make photoplotting as reliable and easy as possible, only use track and pad sizes and shapes for which there is a corresponding aperture. Configure your pad type list to match your aperture list.

It follows that if the designer familiarizes himself with the aperture set supported by the target photoplotter, and tailors the choice of objects placed on a PCB design  (what pad and track size he uses) accordingly, then the photoplotter will be able to faithfully reproduce precisely what the designer had in mind.

However, it is not always desirable to limit the range of choices to the family of apertures supported by an arbitrary photoplotter. Some system must be provided to allow the successful interpretation of any pad shape or track size  that the designer feels he must use.

The program will select apertures ( if they fit within set tolerances) and modify the design data base to match the final photoplot.


Photoplotter setup

G54 on change	Some early model photoplotters require a specific G54 command to be inserted in the control code before every aperture change command. Consult with your photoplot bureau first, and then turn this on or off as they suggest.

Software Arc	Some photoplotters do not support a specific arc drawing command. Advanced PCB can generate a series of line segments to simulate an arc. Consult with your photoplot bureau first, and then turn this on or off as they suggest. The hardware arc is only used for arcs that are in multiples of 90 degrees. For small arc angle, the series of line segments is always used.

Tolerances	If Advanced PCB uses an aperture that does not match exactly, then the design data base will be changed. In this example, the 52 mil track will be replaced in the data base by a 50 mil track. If you do not want the changes, then save you file before plotting.

While the program is generating the photoplot, it will look for an aperture to match each item. For example, if it finds a 52 mil track on the board, but only has a 50 mil aperture, how is this shape plotted?

The two match tolerances control this. In the above example, the closest aperture is 2 mil smaller than track. If the Plus Tolerance is set to 2 mil or larger, then the 50 mil aperture can be used. Otherwise an aperture which can paint the unmatched shape will be assigned and used by the plotter.


Generating photoplots

The Advanced PCB photoplot routines will photoplot all the physical layers  that you have currently got turned on. Tracks, pads, vias, arcs, fills, and text strings will always be photoplotted in final mode.

When the photoplotter is configured and you have the appropriate layers switched on or off, then Choose File-Gerber-Gerber Out to generate the plots.


NC drilling

Introduction to NC-Drilling

Generating NC Drill files


NC-drill use

The use of numerically controlled (NC) drilling machines has provided advantages for both board manufacturers and board developers. By supplying the board maker with a control file which he can send directly to the drilling machine, to drill all the holes in the board, you can save the cost of manually programming the drill, and remove the danger of holes being missed on a complex board. There are however a number of dangers to be considered.

The golden rule is, if you are generating and using NC drill files, then your plots of the board must be very accurate, preferably photoplotted.

Firstly, NC drills are accurate. If your plot is not accurate, then the holes will not be drilled in the center of the pads. Consider a 300mm long printed circuit board. If the plotter has a scale (linear) error of 0.3%, then the total error on the board could be up to 0.9 mm. If the drill is manually programmed from the plot master then the error would not matter, since it would be very small over the length of any single component. If the drill is programmed from a CAD generated file, then the NC Drill will put the hole in exactly the correct position, up to 0.9mm from where it appears on the plot master.


NC Drill files

When creating NC files, Advanced PCB will generate three files types with the same name and different extensions.

You should not modify the report file. If the hole sizes are incorrect, then use the global editing facilities in Advanced PCB to change the hole sizes in the PCB design. This will insure that the PCB design file matches the actual board.

The control file (Extension DRL)

This is in the EIA character format (this is machine readable, not human readable) and is in the EXCELLON language. The data is specified in mils with trailing zero suppression. The drill tools are simply numbered from 1 up to 255. This is the file which is actually sent to the drilling machine.

The ASCII file (Extension TXT)

This file contains the same information as the  EIA file described above but is stored in ASCII character format and hence is readable.

The report file (Extension DRR)

This file contains the list of drill numbers and tools sizes, hole counts, and travel lengths. All in inches and millimeters. Print this file out, and give it the board maker, together with the NC drill control files.


Special files

Advanced PCB.EXE	The main program file.

Advanced PCB.INI	This is used to store all your current settings from one session to another. This file doesn't come with the program but is created the first time you run the program. If you want to have several default set-ups, for different kinds of PCB job, then copy this file to another file name and copy it back before running the program.

Advanced PCB.PAD	This is the default set of pad type definitions. Advanced PCB will search for this at start up. If not found then no components will be able to be placed. To change the default set, simply save your set of pad type definition to the file Advanced PCB.PAD

Advanced PCB.LIB	The default library of patterns for components on the PCB. Advanced PCB will search for this at start up. If not found then no components will be able to be placed until another library is specified.


File types

file.PCB	Used to store a PCB layout.

file.NET	Net list file.

file.DRC	Design rule check result file.

file.BOM	Bill of material file.

file.AB0 to AB9	This is the auto back-up file used to store the layout you are working on.


Photoplotter output files

The following extensions are automatically used when generating Gerber files.

The format is <filename>.G**.

Top (component side)  layer	.GTL

Mid  (signal) layers 1-14	.G1 (-14)

Bottom (solder side) layer	.GBL

Top Overlay (silkscreen)	.GTO

Bottom Overlay (silkscreen)	.GBO

Top Paste mask layer	.GTP

Bottom Paste mask layer	.GBP

Top Solder mask layer	.GTS

Bottom Solder mask layer	.GBS

Internal Power Planes 1-4	.GP1 (2,3,4)

  	Drill Guide Top/Bottom pair	.GG1

  	Drill Guide Top/Mid1 pair	.GG2

  	Drill Guide Mid2/Mid3 pair	.GG3

  	Drill Guide Mid4/Mid5 pair	.GG4

  	Drill Guide Mid6/Mid7 pair	.GG5

  	Drill Guide Mid8/Mid9 pair	.GG6

  	Drill Guide Mid10/Mid11 pair	.GG7

  	Drill Guide Mid12/Mid13 pair	.GG8

  	Drill Guide Mid14/Bottom pair	.GG9

  	Keep Out layer	.GKO

  	Mechanical  (fab & assy) layers 1-4	.GM1 (2,3,4)

Drill Drawing Top/Bottom pair	.GD1

Drill Drawing Top/Mid1 pair	.GD2

Drill Drawing Mid2/Mid3 pair	.GD3

Drill Drawing Mid4/Mid5 pair	.GD4

Drill Drawing Mid6/Mid7 pair	.GD5

Drill Drawing Mid8/Mid9 pair	.GD6

Drill Drawing Mid10/Mid11 pair	.GD7

Drill Drawing Mid12/Mid13 pair	.GD8

Drill Drawing Mid14/Bottom pair	.GD9

Pad Master	.GPM


Selection

The Advanced PCB system allows you to change the elements of your design in two ways:

Choose a command such as Move, then select an item to be moved, or;

Select one or more items then choose a command which acts on the selection such as Move, Clear, etc.

Selection is simply the process of choosing one or more items, upon which some action is to be performed. Under Advanced PCB, selection is a highly flexible process. You can select multiple items, either as a group, or one-at-a-time.

Similarly, you can remove items from the current selection individually or in groups.

See also:	Selection for Autotrax Users

Selection and highlighting

Making selections

The selection hierarchy

Select and De-select commands

Selection rule changes (V2.0)


Selection for Autotrax users

In Advanced PCB the functions of the Block and Highlight commands (such as Block Define or Highlight Net) have been merged into a single concept: Selection. If you wish to perform an operation on a group of primitives on the printed circuit board, you first select the items, then use one of the Edit menu commands. Operations performed on single primitives can be performed using the action-target model similar to Autotrax. For example, choosing the Edit-Move-Pad command (the "action"), prompts you to Select a Pad (the "target").


Selection and highlighting

When you select an item, the color changes from its normal layer color to the Selections color assigned from the Options-Layers dialog box. The item remains selected until you remove it from the selection using either the De-select command or [image] + [image].

Highlighting is related to selection but works within an operation, such as re-routing a track or when generating a netlist. You can see tracks highlight during both of these processes. As primitives highlight, you will notice that highlighted item is not displayed in the Selections color but in the reverse of the layer color. Both selection and highlighting are based the on the geometry of primitives in the workspace - not on the current netlist. In other words, items that are physically connected are included in the selection. This allows you to use selection to trace the connectivity of your design - like a "continuity" check as you manually route connections and to perform other selection-based operations, such as Cut, Copy or Paste. When you select connections or nets, other previously  selected items stay selected until de-selected.


Making selections

Selections are made in three ways:

1.	By direct selection, using [image] + [image] to add (or remove) individual items to the current selection;

2.	By using the Edit-Select and De-select commands to define a selection group;

3.	By choosing an  action, like the Move command, then selecting a single target item for that action.


Direct selection using the mouse and keyboard

Direct selection is the most flexible way to designate one or more items to be moved, copied, cut and pasted into a new location or deleted. To make a select one item:

1.	Use [image] + [image] with the cursor position over an item;

The item will be re-drawn in the Selection color (Options-Layers command). You can do this repeatedly, each time adding another item to the current selection.

If you hear a "beep" or nothing appears to be selected, try zooming in closer (press [image]  and make sure that the cursor is directly over the item you wish to select. Components, especially complex components can take a moment to select.

The Snap to Center option  command) will cause the cursor to "snap" to the nearest primitive, when making the selection. This can make it easier to select items from a dense layout, or when zoomed out from the board.

To add another item to the current selection:

2.	Use [image] + [image] over another item;

To release individual items from the selection,:

3.	Hold down [image] and click on any selected item.

When released, the item will be re-drawn in its original (layer) color. Other selected items remain selected until they are either individually released using [image] + [image] or until the Edit-DeSelect-All command is executed.

You can use the Zoom commands and hot key shortcuts [image] and [image], at any time when making or releasing selection.


The selection hierarchy

When making a direct selection using [image] + [image], the selection routine looks first  for vias, then tracks, then pads, then area fills, then strings and then components. If you wish to select a component using this method you simply position the cursor inside the component, being careful to avoid any free primitives that are placed inside the component.

When using selection commands (Edit-Select-All, Edit-Select-Inside Area), free primitives will not be included in the selection if they are hidden (Options-Display command). Also, free primitives will be selected only if their layer is active (Options-Layers command). This allows the user to control which free primitives are included in a selection by hiding specific primitives or by turning off specific layers. This applies only to free primitives, not components.

The same selection hierarchy operates when you de-select items individually, using [image] +


Select and De-select commands

The Edit-Select commands allows you to select all items inside or outside of an area, all items on one layer, or all free primitives (items other than components, dimensions or coordinate markers). You can also select by physical net or physical connection. These options allow you to extend the selection (or de-selection) beyond a few items.

Edit-De-Select provides the same set of options. Using these two sets of commands you can define complex grouping which can then be moved, copied or deleted. The Edit-Toggle Selection command allows you to turn the selection state of individual primitives "off" or "on" duplicating "direct" selection performed using [image] + [image], described above.

When using selection commands (Edit-Select-All, Edit-Select-Inside Area), free primitives will not be included in the selection if they are hidden (Options-Display command). Also, free primitives will be selected only if their layer is active (Options-Layers command). This allows the user to control which free primitives are included in a selection by hiding specific primitives or by turning off specific layers. This applies only to free primitives, not components.

Shortcut:	Press [image] to choose from the De-Select command options.

Select  and De-select commands include:

Select/Deselect Inside Area

Select/Deselect Outside Area

Select/Deselect Free Primitives

Select/Deselect All

Toggling the selection


Select Deselect Inside Area
Select/Deselect-Inside Area

This command allows you to define a rectangular area. Only those tracks, components, strings or fills that lie completely inside the area will be included. Free pads or vias will be included in the selection if their center is inside the rectangle.

To choose the items inside a selection rectangle.

1.	Choose the Edit-Select-Inside Area command;

You will be prompted "Select First Corner."

2.	Move the cursor then press [image] or [image] to define the first corner of the selection rectangle;

The prompt changes to "Select Second Corner."

3.	Move the cursor to enclose the selection area in the highlighted rectangle;

4.	Press [image] or [image] to complete the selection.

The newly selected primitives will be highlighted using the selection color. Any previously selected items will remain selected until de-selected.

When using selection commands (Edit-Select-All, Edit-Select-Inside Area), free primitives will not be included in the selection if they are hidden (Options-Display command). Also, free primitives will be selected only if their layer is active (Options-Layers command). This allows the user to control which free primitives are included in a selection by hiding specific primitives or by turning off specific layers. This applies only to free primitives, not components.


Select Deselect Outside Area
Select/Deselect-Outside Area

This option selects everything outside the selection rectangle. The rules for inclusion in the selection are the same as for the Inside Area command. The procedure for defining the selection rectangle is the same as for Inside Area.

See also: Select/DeSelect Inside Area


Select Deselect All
Select/Deselect-All

This command selects everything placed in the Protel document window;

See also: Select/DeSelect Inside Area


Select Deselect Free Primitives
Select/Deselect-Free Primitives

This option selects all tracks, vias, free pads in the document window. Components are not selected. This feature is useful for stripping a routed, or partially routed board back to its "placed" condition.

See also: Select/DeSelect Inside Area


Select Deselect All on Layer
Select/Deselect All on Layer

With this command the selection will include all primitives on the current layer. Multi-layer items (typically multi-layer pads and vias)  are excluded from the selection.

See also: Select/DeSelect Inside Area


Toggling selections
Toggling the selection status

The Toggle Selection command allows you to select or de-select specific primitives, by type. Using this option, rather than the [image] + [image] shortcut, can be helpful when you are working in a densely populated area of your design where components and other primitives are overlapped or when you wish to quickly add and remove a number of items from the selection. To use this feature:

1.	Choose the Toggle Selection command;

2.	Choose one of the available options: Arcs [image], Components [image], Fills [image], Pads [image], Strings [image], Tracks [image] or Vias [image];

You will be prompted "Select (primitive)."

3.	Click on the selected primitive type to add or remove the item from the current selection;

The prompt "Select (item)" will be continuously displayed.

4.	Press [image] to leave the Toggle Selection command.


Making changes

The Change command is used to modify specific attributes of placed items. Each item or primitive has its own range of editable attributes.

You can change one item or extend changes across your entire design using powerful global editing options.

To change any placed item, move the cursor over the item and double-click the [image] button. This shortcut will open the Change (item) dialog box for the selected item.

You can also use the Change command from the Edit menu:

1.	Choose Edit-Change;

2.	Choose the type of item to be changed: Arc [image], Component [image], Fill [image], Pad [image], Track [image] or Via [image];

The prompt "Select (item)" will appear on the status line.

2.	Position the cursor over the target item and press [image] or [image];

A dialog box opens, displaying the editable attributes for the item. It is now possible to change any or all attributes of the selected item, such as a track width or layer. These options are described in the next section, Global Changes.

4.	Press [image] or click OK to accept your changes. To cancel the change and close the dialog box press [image];

The status line will prompt "Select (item).

5.	Select another item to be changed or press [image] or [image] to leave the Change command.

PCB will not prevent changes that violate specified design rules. A Design Rule Check(DRC) should always be performed before final artwork is generated.


Global changes

Changes can be made to a single selected item or they can be applied globally across the entire board using flexible, powerful global editing options.

Virtually every editable attribute can be globally applied. A simple example would be changing the hole size assigned to a single pad. Typically, the designer would want this new hole size applied to other pads as well. However, it might be important that the new hole size be applied only to pads with the same (original) hole size as the selected pad, or perhaps pads of a specific shape or size only, etc.

All of these options (and more) are supported by the Change commands in Advanced PCB.

The possible applications for global changes are limited only by the imagination of the designer.

The large number of global change options may make this feature appear somewhat complex at first. However, the principles of applying global changes are reasonably simple, once understood.

When mastered, this feature can be an important productivity tool.

Matching attributes for global changes can be assigned by clicking the Options button in any of the Change (item) dialog boxes. When you click Options, the dialog box expands to display the parameters for global matches.

Each Change (item) dialog box may contain different options since every type of item has a unique set of attributes. For example, tracks have two changeable attributes - Width and Layer, while a Pads have seven. For a detailed description of all items and the valid range for each attribute please see the section on PCB files in Appendix A.

There are four groups of options in the expanded dialog box:

Attributes

Attributes to Copy

Attributes to Match By

Edit Change Scope


Attributes

These are the changeable parameters of the item. For a Track, the changeable attributes are Width, and Layer. Any or all of the changeable attributes may be changed at each opening of the dialog box.


Attributes to Copy

Any number of the editable attributes can be copied to other items. Click in the box corresponding with the desired attribute to assign the changes to the target items.


Attributes to Match By

These attributes define matching criteria for other items. There are three settings possible for each copyable attribute:

Same	Change all items which match the value of the item being changed;

Different	Change all items which do not match the value of the item being changed;

Any	Change whether or not the attribute matches the item being edited.

Matching can be performed using mixed attributes. For example, track matching attributes include width, layer, and selection status. It is possible to make a global changes to  currently selected tracks of any width, on the same layer, etc.

This provides feature provides comprehensive control over global changes.


Edit Change Scope

This option applies changes locally or globally.

This Item Only	Local editing applies the changed attributes to the selected item (default setting);

Change All Matched	Applies changes globally, using the Attributes To Match By and Attributes to Copy settings.


Changing arcs

Arc attributes which can be edited include:

Line Width	Arc line width can be any value between 1 - 255 mils (0.25 - 25.0 mm). The current default track width setting is used as the default arc line width.

Layer	Arcs can be assigned to any layer of the PCB. To change the layer assignment, click in the Layer box and choose a new layer.

Global Options	Click Options to view the global edit options for arcs.

Attributes to Copy 	Attributes which can be copied to other arcs are Line Width and Layer.

Attributes to Match By 	Attributes which determine the arcs to be globally edited include Line Width, Layer, and Selection.


Changing components

Component attributes which can be edited include:

Designator	Component designators and comments have a number of editable attributes:

Pattern	The current physical pattern (or footprint) of the component can be changed to any other available pattern in an open component library.

Click the Pattern button to scroll the selection bar through the current components.

Component patterns can be changed freely; however, if there are netlist connections to the pads, the new footprint must have the same pin numbers available as the previous one or a warning message will be displayed.

For example, changing a DIP16 to an SMD16A would update the internal connection list. Changing a DIP16 to a  TO-3 would generate a warning and the replacement would be canceled.

The ratsnest display would also be updated to reflect these un-routed nodes. A DIP16 can also be changed to a DIP14, providing there are no connections to pins 15 and 16 on the DIP16.

These rules also apply to global pattern changes.

Layer	Components can be assigned to either the top or bottom layer of the PCB. To change the layer assignment, click in the Layer box and choose Top layer or Bottom layer.

Changing the layer status swaps the component to the opposite layer. For example, when moving a Top layer component to the Bottom layer, primitives on the Top Overlay layer will be automatically re-assigned to the Bottom Overlay layer. The orientation of the component will be flipped along the X axis and the component overlay text will read from the "bottom". Single layer pads are also swapped between the Top layer and Bottom layer.

Place Status	Component placement status has two possible states. Free To Move indicates that the component position can be changed by the Auto Place options. Locked In Place  indicates that the component will not be moved by Auto Place. When a component is first placed by Auto Place its status remains Free To Move until its position is changed by the user. Once you move a component, its status is changed to Fixed In Place. This allows you to lock seed components into place and then re-run Auto Place.

Global Options	Click Options to view the global edit options for components.

Remember, component designators and comments have their own global options, described above. Component global options include:

Attributes to Copy	Attributes which can be copied to other components are Pattern, Layer, and Place Status.

Attributes to Match By	Attributes which determine the components to be globally edited include Pattern, Comment, Layer, Place Status, selection, and Wildcard Name.

Wildcards	The Wildcard Name field is used to apply changes to components that share designator prefixes (or some other common element). For example, to change all components whose designators start with "U" type U* in the Wildcard Name option. If you use this feature, components with designators U1, U2, etc. will be changed.


Changing designators and comments

Component designator attributes which can be edited include:

Text	The component label, U1 etc. This attribute is not globally editable as each component must have a unique designator. Designators can be a maximum of 8 characters in length (spaces are not allowed). It is standard practice to use a single letter prefix and numeric suffix.

PCB stores the designators used each time you place a component and will automatically supply and incremental designator when you place any previously placed pattern. For example, if you designate a DB9F connector "J1" a second DB9F will be automatically assigned a default designator of "J2", and so on.

Height	The size of the text in mils (.001 inch) or mm;

Layer	Designators can be assigned to any layer. Click the Layer button to scroll the selection bar through the layer options. The selected layer will be displayed in the Layer box;

Font	Three special vector fonts are available. Click the Font button to choose the Default font, Sans Serif font or Serif font;

Show/Hide	Component text can be displayed or hidden. Hidden text will not be printed. Click the Show/Hide button to toggle the display status.

Component comments share the same editable attributes as component designators. However, unlike designator text, comment text changes can be globally applied to other components.

See also:	Component text comments

Component text cesignators


Changing fills

Fills can be assigned to any layer of the PCB. To change the layer assignment, click in the Layer box and choose a new layer.

Global Options	Click Options to view the global edit options for fills.

Options Include:

Attributes to Copy	Fill layer assignment can be copied to other fills .

Attributes to Match By	Attributes which determine the fills to be globally edited include Layer and Selection.


Changing pads

Free pads or component pads can be individually and globally edited. Attributes which can be edited include:

Designator	Pad designators are used to label pads with pin numbers when creating a new component.

Free pads can also include a designator. The default value for free pad designators is empty.

X Size	This field describes the size of the pad on the horizontal (x) axis. Range is 1-1000 mils (.25-25.0 mm).

Y Size	This field describes the size of the pad on the vertical (y) axis. Range is 1-1000 mils (.25-25.0 mm).

The X size and Y size can be changed independently of each other to modify pad shapes.

Hole Size	This attribute assigns the size of the hole diameter to be drilled in the pad during fabrication, in mils (.001 inch) or mm. For SMD pads or edge connectors this must be set to zero.

Layer	Pads can be assigned to any artwork layer. Multi-layer pads are used for through-hole components. SMD pads are typically assigned to either the Top layer or Bottom layer. Click the Layer button to scroll the selection bar through the available layers to choose a new layer.

Shape	Pad shapes include Rounded, Rectangular, and Octagonal. Shapes can be manipulated by changing the X and Y size settings. A Component can have any number of differently shaped Pads. Typically, Pad 1 is assigned a unique shape for orientation during insertion onto a board during assembly.

Pwr/Gnd	This attribute is used to manually assign a through-hole (Multi-layer) pad's connection status to any of four internal power planes, if used. Pad's can be connected to a power plane by either a Direct or Relief connection. SMD pads can be Tagged To Plane for automatic connection during automatic or interactive routing. Split planes can be created by placing polygons on internal plane layers, with full preservation of net integrity and DRC functions.

Global Options

Click Options to view the global edit options for pads. Options Include:

Attributes to Copy	Attributes which an be copied to other pads are Designator, X size, Y size, Hole Size, Layer, Shape and Pwr/Gnd assignment.

Attributes to Match By	Global match attributes include Designator, X size, Y size, Hole Size, Component Pattern, Layer, Shape, Pwr/Gnd layer assignment, selection status and Group.

Group refers to pads that are part of a component. This option allows you to restrict changes to component pads, free pads or to allow changes to be made to any pad.


Changing strings

Free text strings can be changed both individually and globally. Editable text string attributes include:

Text	The text content of the string. Strings can be up to 32 characters long and any alphanumeric character, including spaces.

Height	Text size can be set in mils (.001 in) or mm. Range is 36-4000 mils. The stroke width and character width used to display/print the text is automatically proportioned to the height assigned.

Layer	Text strings can be assigned to any layer.

Font	Three special vector fonts are available: Default, Sans Serif and Serif. These fonts are designed to support vector plotting.

Global Options	Click Options to view the global edit options for strings.

Options Include:

Attributes to Copy	Copyable attributes include Text (contents of the string), Height, Layer or Font.

Attributes to Match By	Global matching attributes for strings include Text (contents of the string), Height, Layer, Font and Selection status.


Changing tracks

Free text tracks and component text (designators and comments) can be changed both individually and globally.

Editable text track attributes include:

Width	Track width can be set in mils (.001 in) or mm. Range is 1-1000 mils. The default width assignment is 12 mils.

Layer	Tracks can be assigned to any layer. Generally, tracks are placed on the Top, Bottom and Mid layers to carry signals or currents. Tracks are also placed on other layers for non-electrical purposes.

For example, tracks are used on the Overlay layers to indicate the component outlines on the silkscreen artwork. Tracks are also used to indicate voids in layers which are plotted/printed in reverse, such as power planes, solder masks and paste masks.

Global Options	Click Options to view the global edit options for tracks.

Options Include:

Attributes to Copy	Copyable attributes include track Width and Layer .

Attributes to Match By	Global matching attributes for tracks include track Width, Layer assignment and Selection status.


Changing vias

Vias are special purpose pads used to connect tracks between different layers. Vias can be placed through all layers or on any layer pair. Vias are always circular in shape, this is not an attribute which can be changed.

If a shape other than circular is required a free Pad should be used. Vias can be changed both individually and globally.

Editable via attributes include:

Diameter	Vias can be assigned any size in the range of 1-255 mils.

Hole Size	This option assigns the hole diameter to be drilled through each via. Via hole size can be assigned independently of the via size. The range is 1-255 mils.

Via hole assignments should be determined in consultation with your board fabrication source. The diameter required

Layer Pair	Via layer assignments are made automatically when the vias are placed, either by the autorouter or when manually routing tracks (with the Auto Via option enabled under the Options-Preferences command).

It is possible to change layer pair assignments manually, but the designer should be aware that via layer re-assignment must be approached with great care, if unforeseen effects in the finished board artwork are to be avoided.

Global Options	Click Options to view the global edit options for vias.

Options Include:

Attributes to Copy	Copyable attributes include Diameter, Hole Size and Layer Pair.

Attributes to Match By	Global matching attributes for vias include Diameter, Hole Size, Layer Pair assignment and Selection status.


File Formats
File format support

Advanced PCB will load Advanced PCB binary and text files, Protel Autotrax files, Tango PCB and Tango Series II files, Protel PCB 3.12 files, PADS-PCB and PADS2000 files (in .ASC format) and PCAD (PDIF 5 and 6) files.


ASCII format update

Corrections to PCB 2 ASCII file format

The following are corrections to the Advanced PCB text file format. (see p. 197 of Advanced PCB Reference)

The file header

PCB FILE 6 VERSION 2.60 (Current version has been updated to 2.60)

Component (missing Pad stack description has been added to this section, as below)

50000 50000	Pad TOP x, y size (range: 2-500000).

1	Pad TOP shape (0=rounded, 1=rectangular, 2=octagonal, 6=terminator).

50000 50000	Pad MID/OTHER x, y size (range: 2-500000).

1	Pad MID/OTHER shape (0=rounded, 1=rectangular, 2=octagonal, 6=terminator).

50000 50000	Pad BOTTOM x, y size (range: 2-500000).

1	Pad BOTTOM shape (0=rounded, 1 =rectangular, 2=octagonal, 6=terminator).

Polygon (updated polygon header information, reference to pour over primitives in same net have been added)

PG	Marks special polygon object which can include arcs, fills and tracks.

1	Polygon layer number (range: 1-34).

0	Net number assigned to Polygon, see Definitions.

0 1 1 0 1	This line includes these attributes:

0	Remove dead copper (0 = false, 1 = true).

1	Horizontal tracks (0 = false, 1 = true).

1	Vertical tracks (0 = false, 1 = true).

0	Arcs/octagons at pads (0 = arcs, 1 = ocatagons).

0	Fills for tracks (0 = false, 1 = true)

1	Pour over primitives on the same net (0 = false, 1 = true)


absolute cursor

Display mode where the displayed cursor coordinates are measured from the absolute workspace origin (0,0 coordinates) or lower-left corner.


active layer

Any Board window layer which has been activated using the Options-Layers & Colors dialog box.


aperture file

An ASCII text file which includes a description of each of the apertures used to generate a Gerber photoplot file. These descriptions are stored in aperture files, also called aperture tables.


arc

Circular or semi-circular design elements. Advanced PCB displays arcs as a series of chords, or straight line segments.


Auto Place

Advanced PCB options for automatically loading netlisted components from the current library into a pre-defined board outline.


autoroute

Advanced PCB options for automatically (or interactively) routing the connections in a PCB.


Batch mode

Batch mode is an option under Advanced PCB which allows you to select a number of plot types (or plot layers) to be generated in a single operation.


Bill of Materials

Or, BOM. A list of the components (including quantities) used in a PCB.


block

A group of components, tracks, etc., which once saved as a selection, can be imported into the current workfile.


Board layer

A special edit layer which holds alignment targets, trim marks, annotation or other mechanical details of your PCB, which you may wish to plot with selected layers.


Board window

The window where you display and edit your Advanced PCB PCB file.


Bottom layer

Edit layer for the bottom (or 'solder side') of the PCB.


break

Conversion of a single track segment into two connected segments.


Check plot

A composite plot of multiple artwork layers, used to verify design rules and alignment of the PCB.


clipboard

Reserved memory used to hold Cut or Copy command selections.


Comment

Optional component text field created when a component is placed. Normally used to hold a component value, description or part number.


component

A collection of primitives stored as a single entity in an Advanced PCB library. Components consist of one or more multi-layer pads and tracks and/or arcs on the top overlay, which define the component shape.


component text

Text that is part of a component display. Component text is created at the time the component is placed. It can be moved (including rotate and flip) but cannot be deleted (only hidden). This text remains associated with the component until the component is deleted.


copper

Any non-etched (conductive) portion of any layer of a printed circuit board. Also refers to Top layer of PCB.


current layer

Board window layer displayed on the Title bar. Tracks, text, arcs, or fills will be placed on the current layer only.


cursor

The graphic 'pointer' or selection tool used to select or position objects in the workspace.


default

Program settings or options which remain selected until changed by the user. Most defaults are stored in a file called Advanced PCB Prefs (ie. preferences).


de-select

Removing the highlighted (selected) condition, from an item in the Board window or a Tool. De-selection involves clicking elsewhere in the board window or selecting another tool.


Designator

Also called component label. The unique identifier assigned to each component in a circuit.


Design Rule Check

Advanced PCB routines for checking a routed PCB file using a netlist to verify connections and user-defined clearance settings to check for clearance violations.


double-sided

Refers to a PCB with tracks on both sides of a single laminate layer.


draft code

A code used to identify each aperture in an aperture file or in a Gerber format photoplotter file. Aperture draft codes are typically in the format of a 'D' followed by two or three digits.


draft mode

The display, plotting or printing of primitives (tracks, pads, arcs, fills, etc.) in outline, rather than filled, form.


Drill drawing

A special plot that uses coded targets to indicate the position and tool assignment for numerically controlled (N/C) drill files.


Drill guide

A special plot, similar to a pad master, which indicates the position of all holes on a PCB.


fill

An area fill, or solid rectangular copper on a PCB layer, used for shielding and/or supply of current.


free pad

Any pad that does not belong to a library component. Free pads are identified by the default identifier '0'.


free text

Text placed in the Board window using the Text tool (not component text).


Gerber format

The RS-274 format is the standard file format adopted for coding photoplot files. A Gerber format file describes a photoplot in terms of draft codes and coordinates. The draft codes control the aperture to be used and the opening and closing of the shutter. Coordinates give the position of flashes and strokes on the plot.


Gerber plot

A photoplot stored in a Gerber format file, also used generically to refer to any photoplot.


grid

A system of visible and invisible points on the Advanced PCB workspace used to locate a precise coordinate position.


Ground plane

Special PCB mid-layer supplying all ground pins.


hardware arc

When plotting, arcs which are created by the plotter, from coordinate, line width and radius information. Some plotters support this option, others depend upon software arc descriptions generated by Advanced PCB.


highlight

A unique display color assigned to selected items on-screen to aid in identification or editing. Advanced PCB uses the 'reverse' of the current color or grayscale shade to indicate selection.


imperial measure

Inch-based measurement system  Advanced PCB uses the mil (.001inch) as its default unit. Measurements are stored in imperial format regardless of the display mode.


Keep Out Layer

Special layer used to define a perimeter and 'no go' areas for auto component placement and autorouting.


layer

Printed circuit boards are constructed from one or more layers. Photo-tools, (or master artwork) used to fabricate these layers, are generated as individual plot or print files.


layer bias

Practice of alternating the principal direction of track routing on PCB layer pairs.


Match file

A text file (.MAT extension) that records the aperture assignments generated when creating a Gerber plot file.


metric measure

Metric-based measurement system using mm (millimeter) as the base unit of measure for PCB design and fabrication. Advanced PCB stores all dimensions in imperial format, regardless of the display mode.


Mid layer

Any of four layers (other than the Top and Bottom layers) which can be used for routing the connections on a multi-layer PCB.


mil

Unit of imperial measure equal to .001 inch.


mm

Millimeter - unit of metric measure in Advanced PCB.


minimum X, Y

The minimum X or Y coordinate of items in the Advanced PCB workspace. This describes the left-most and bottom-most coordinates used in the file or plot.


multi-layer

A multi-layer board is one which is made up of two or more sheets of board laminate, which allows electrical connections to be made on a choice of several layers. See also layer.


netlist

A text file which lists all the connections of an electronic circuit. Netlists are used to verify the contents of a design, or to transfer design information between CAD (computer aided design) systems.


offsets

Special corrections applied to the origin (0,0 coordinate) of a plot (or print), used to position the artwork within the plot area. Also, the additional X or Y axis spacing used in the Edit-Repeat placement option.


origin

Location of the 0,0 coordinate in either a PCB file or a plot. Advanced PCB uses the extreme lower left corner of the workspace as the default origin.


orthogonal

Drafting standard where lines are constrained to either vertical, horizontal or 45 degree placement Ð a common practice in PCB design.


Overlay

A special layer of PCB artwork, also called the silkscreen layer. Overlays are used to identify components on the top or bottom of a PCB, and are provided as an aid to manufacturing and maintenance of the PCB.


package

The physical description of a component, e.g. DIP16, defined by the number and location of pins, dimensions, etc.


Pad master

A special plot type that includes all the pads and vias in the PCB, typically used for drilling all pad and via holes in prototype boards .


pad

A design element used to locate and connect tracks to component pins on a PCB, also called a land.


pan

The ability to move the viewing area of the screen as you work on a magnified area of the Board window. Advanced PCB provides automatic panning when placing or moving selected items. The Zoom tool also pans the Board window.


Paste Mask

Special plot of SMD pads, used to define a mask for applying solder paste for 'hot re-flow' fabrication.


pre-route

Connection completed by the designer prior to using netlist-based autorouting options. Advanced PCB processes these connections independently from autorouted connections.


ratsnest

Special straight line display of netlisted connections on the 'placed' PCB layout.


schematic capture

CAD package for circuit design capable of generating a netlist or report output allowing the design information to be transferred to another CAD environment.


select

To position the cursor over an item and 'click' with the mouse button. Selected items are displayed in a highlighted color or pattern.


serial

Refers to RS-232C and RS-422 standard for data terminal equipment (DTE) communication. Defies comprehension.


signal layers

Layers available for routing PCB connections in Advanced PCB, specifically the Top, Mid 1Ð4 and Bottom layers.


silkscreen

See Overlay.


SMD

Surface Mount Device. Also SMT (Surface Mount Technology). Components and special PCB assembly techniques for components which attach to either the top or bottom of the PCB without using holes, carriers or mounts.


snap grid

An invisible array of regularly spaced points on the screen which defines the current cursor position and the available location for any object in the Advanced PCB workspace.


snap to

Special property of track placement in Advanced PCB where tracks will 'attach' to pads without blocking the plotted pad holes, if the track is led to within 10 mils (.010) of the pad center when manually routed.


software arc

When plotting, arcs which are generated by Advanced PCB using straight line chord segments. See Hardware arcs.


Solder mask

Special plot used to create a mask for the top or bottom layers of a PCB. The mask is a 'resist' layer which leaves pads and vias exposed to the solder, while protecting any tracks, etc.


solder side

Refers to the Bottom side layer of a PCB.


Status line

The window at the bottom-left of the screen which displays the current X and Y coordinates of the cursor as well as user prompts.


string

Individual element of free text.


through hole

See Via. Also describes PCB technology where all component pins pass through the PCB.


Title block

Optional line of text which identifies the filename and plot layer.


track

Also called traces, used to carry current or signals on a PCB.


vector font

In Advanced PCB, special font that support pen plotting and photoplotting.


vector plotter

A vector photoplotter creates a plot by 'drawing' each stroke and flash individually. To create a stroke, the film is moved relative the light source. Flashes are made with the film and light source stationary. See also raster plotter.


via

Or through hole, a special purpose pad, with a drilled (normally plated) hole, used to connect tracks on different layers. Advanced PCB vias are multi-layer (occupy all board layers).


visible grid

An array of dots on the screen which provides a visual reference for positioning items accurately on-screen.


workspace

The complete Advanced PCB editing environment including the Board window, Tool palette and Menu bar.


X, Y size

The difference between the minimum and maximum coordinates used on each axis of a PCB or plot, ie. the height and width of the board.


Messages

Auto Place cannot run. No un-locked components

Bad format in Aperture file

Bad format in Pad Type File

Clearance Error

Component Comment Different

Component Designator is already used

Component Designator Not Found

Component Missing From PCB

Component Not Found In Library

Component Pattern Different

Disk Is Write Protected

Draft Code Number Already Used

Drive Not Ready

Drive Write Error

Extra component in net file

Extra net in net file

Extra net on board

Extra Pin On Net

File Corruption Error

File Not Found

File Not Open

Film is too small for plot

I/O Error Number

Invalid Drive

Invalid File Access

Library File Already Exists

Library Name is Already Used

Net Broken Into Multiple Sub-nets

Net Name Not Found

New component cannot be matched with old

No Aperture Space (1000 Limit)

No Apertures Loaded

No Components In Library

No Components Placed

No Holes In PCB

No Horizontal Route Layer Specified

No Libraries Have Been Opened

No Nets Loaded

No Outline On Keepout Layer

No Pad Type Space (200 Limit)

No Pad Types Loaded

No Pins Have Been Selected

No Pins On Power Plane

No Printer Selected

No Selected Primitives For Library Component

No Vertical Route Layer Specified

Nothing Has Been Selected

Nothing to plot

Out Of Memory

Pad Not Found

Pad Type Name Already Used

Pad Type Not Found

Page is too small for plot

Path Not Found

Pin Missing From PCB

Rectangle With No Area Specified

Sector Not Found

Selected Items Will Be Placed Outside PCB Area

String Not Found

This Library is Full

Too Many Files Open

UnRecognized Library File Format

UnRecognized PCB File Format


Auto Place cannot run. No un-locked components

Autoplace can only move components which have been set to " Free to move" using the edit change component command. If there are non free, then the placer will do nothing.


Bad format in Aperture file

The aperture file which you have tried to load or merge from (extension APT) contains text which does not conform to the Protel aperture file format. See the manual for more details.


Bad format in Pad Type File

The pad type file which you have tried to load or merge from (extension PAD) contains text which does not conform to the protel PAD file format. See the manual for more details. These files can also be edited with a standard text editor.


Clearance Error

Only occurs in DRC files.

The two listed items are closer together than is allowed using the current clearance setting. Either move the items or change the clearance setting using Netlist Clearance.


Component Comment Different

Only occurs in DRC files.

The comment of the component with the listed designator, does not match that was found in the DRC netlist.


Component Designator is already used

Components must always have unique names (designators). If you specify a name which is already used then you will get this message. For example, if you are placing a capacitor and type  C21  and that designator is used. For this example try typing  C?  and the program will find you the lowest number with prefix C that you can use.


Component Designator Not Found

You will get this message if you enter a component designator that is not used in the current design. Type  ?  to get a list to select from, or use the Information Components command to display a list.


Component Missing From PCB

Only occurs in DRC files.

The comment of the component with the listed designator, does not match that was found in the DRC netlist.


Component Not Found In Library

While placing a component or editing a component pattern, you have typed in a component name in the library (DIP21 for example) that does not exist. Use the Library Components command to browse through the library.


Component Pattern Different

Only occurs in DRC files.

A component which is listed in the netlist file was not found on the board.


Disk Is Write Protected

Remove the write protection tab or get a new disk.


Draft Code Number Already Used

While editing an aperture file, you have tried to create a new photoplotter aperture with the same draft code as one already created. Either delete the original or use a different draft code.


Drive Not Ready

If this is a floppy, the door is probably open. If it occurs with a hard drive, you may have a system harware/software fault.


Drive Write Error

Most likely cause is running out of disk space.


Extra component in net file

Only occurs in DRC files.

DRC has found a component in the netlist which does not appera on the board.


Extra net in net file

Only occurs in DRC files.

DRC has found a net in the netlist file which does not appear on the board.


Extra net on board

Only occurs in DRC files.

DRC has found a net on the board which does not appear in the netlist file.


Extra Pin On Net

Only occurs in DRC files.

DRC has found a Pin on a net on the board which does not appear on the same net in the netlist file.


File Corruption Error

The PCB design file which you have tried to load from (extension PCB) contains text which does not conform to the Protel PCB file format.

This error indicates that the program Recognized the file as a valid PCB file, but then while actually loading it, some part of it was invalid. If you have been editing the file manually (with a text editor) then see the manual for more information or contact Protel Technical support. Or , if the file is a foriegn format, Tango for example, it may contain elements that are not Recognized by the Protel loader.

Protel AUTOTRAX and EASYTRAX, Tango PCB, Tango Series II and Protel PCB 3.12 files are loaded automatically.


File Not Found

The file name selected could not be found.


File Not Open

The file chosen could not be opened. Check the name and try again.


Film is too small for plot

With the film and border size you have selected, the current board will not fit on the film.


I/O Error Number

Contact Protel Tech support with details of your actions and the I/O error number.

Exit the program, exit windows and try again.


Invalid Drive

You have specified a drive which doesnt exist.


Invalid File Access

Either a network sharing error or some sort of file corruption.

Exit the program, exit windows and try again.


Library File Already Exists

When creating a new library, you must use a name that is not already used.


Library Name is Already Used

Component patterns in the same library must always have unique names. If you specify a name which is already used then you will get this message.


Net Broken Into Multiple Sub-nets

Only occurs in DRC files.

DRC has found a net on the PCB which is not fully routed.

The partial routed section of the net are listed.


Net Name Not Found

You will get this message if you enter a net name that is not used in the current design. Type  ?  to get a list to select from, or use the Information Nets command to display a list.


New component cannot be matched with old

When editing a component pattern, pins with connection going to the them could not be matched with pins on the new pattern. For example, if you change a DIP16 to DIP14 and there is a connection to pin 16, then the program cannot resolve the connection. If you really want to make the change, you must either delete and replace the component, or clear the netlist and reload it after editing the pattern.


No Aperture Space (1000 Limit)

You can only have 1000 apertures loaded at one time.


No Apertures Loaded

You have tried to photoplot or edit an aperture without having loaded an aperture file. See the manual for more details.


No Components In Library

There are no component patterns stored in the current library. The library was probably just created. Select another library.


No Components Placed

You have selected Information Components, with no components placed on the current design.


No Holes In PCB

If you try to generate an NC drill file when there are no through hole items in the current design, you will get this message.


No Horizontal Route Layer Specified

To run the autorouter, you must select a horizontal layer and a vertical layer, or alternatively, select a single layer for both. See the chapter on automatic routing for more details.


No Libraries Have Been Opened

You have tried to list a library or place a component, when there is no library selected. Select a library file and try again.


No Nets Loaded

You have tried to list a net list or autoroute, when  no nets have been loaded. Use the Netlist Nets Get Nets command to load a netlist. See the chapter on netlists for more details.


No Outline On Keepout Layer

Before autoplacing components, you must specify some board outline and keep outs for the program to work within.


No Pad Type Space (200 Limit)

You can only have 200 different pad types loaded at one time.


No Pad Types Loaded

You have tried to edit, list or delete a pad type (or place a pad), when there are none loaded. The default PFW.PAD file should be loaded automatically when the program is started. If not, then make sure this file is the same directory as PFW.EXE, or in directory that appears on the DOS path.


No Pins Have Been Selected

You have selected Information Selected Pins with no pins currently selected.


No Pins On Power Plane

You have selected Information Power Plane 1,2,3,4  with no pins currently connected to the chosen plane. Set the power plabe net names with the Netlist Power Plane command, and reload your netlist to make these connections, or alternatively, manually edit the power plane attribute of these pads with Edit Change Pad.


No Printer Selected

You must selected a windows printer in File Plot/Print before choosing Generate Prints.

Use Window Control Panel to install printers.


No Selected Primitives For Library Component

You have used the Library Components Add command with nothing slected on the PCB. Place some items, selected them, and run the command again.


No Vertical Route Layer Specified

To run the autorouter, you must select a horizontal layer and a vertical layer, or alternatively, select a single layer for both. See the manual chapter on automatic routing for more details.


Nothing Has Been Selected

Use the select/deselect commands or SHIFT+Left Mouse to select some items.


Nothing to plot

Not items were found on the board.


Out Of Memory

While placing items, loading a file or general editing, the program has run out of memory. If you have done some deletions then save, close  and reload you file to clear the Undo stack. If none of these options work, then you need to add some more memory.


Pad Not Found

In the Jump Pad command, the pad designator that you specified was not found any where on the component that you have selected. See the chapter on finding and jumping to items for more details.


Pad Type Name Already Used

While editing an aperture file (See the chapter on aperture files), you have tried to create a new photoplotter aperture with the same draft code as one already created. Either delete the original or use a different draft code.


Pad Type Not Found

You have tried to merge a pad type from a pad type file. The pad type name specified was not found in that file.


Page is too small for plot

With the current printer, scale and border size you have selected, the current board will not fit on the page.


Path Not Found

You have specified a path which doesnt exist.


Pin Missing From PCB

Only occurs in DRC files.

DRC has found a Pin on a net in the netlist file, which does not appear on the board.


Rectangle With No Area Specified

While selecting an area for Zoom Point, Zoom Window or Select Inside, you have specified either the horizontal or vertical dimension of the rectangle to be zero.


Sector Not Found

Hardware read/write error, usually on hard drives.


Selected Items Will Be Placed Outside PCB Area

You cannot move or paste a selection outside the 0,0 32000,32000 workspace.


String Not Found

In the Jump String command, the text string that you specified was not found any where on the board. See the chapter on finding and jumping to items for more details.


This Library is Full

Each library can hold 500 component patterns. If you try to store more than this is a library, you will get this message. Create a new library. There is no limit on the number of libraries that you can have open at one time.


Too Many Files Open

Check you files statement in C:\Config.sys

Set to at least 30.


UnRecognized Library File Format

The library file which you have tried to load or merge from (extension LIB) is not saved in a valid Protel format. It may not be the right file (a Protel Schematic file for example) or it may have been damaged. If it is damaged, then you will have to resort to your floppy back-up (which, of course, you always keep safe).


UnRecognized PCB File Format

Advanced PCB will load Advanced PCB binary, Advanced PCB text, PADS-PCB (.ASC), PADS2000 (.ASC), PCAD (PDIF 5 & 6), Protel Autotrax and Easytrax, Tango PCB, Tango Series II and Protel PCB 3.12 files automatically.

Any other PCB file formats will give this error. This error may also be caused by corruption of the file header.