home
***
CD-ROM
|
disk
|
FTP
|
other
***
search
/
Aminet 1 (Walnut Creek)
/
Aminet - June 1993 [Walnut Creek].iso
/
aminet
/
biz
/
misc
/
probrd1.lha
/
pb.htex
< prev
next >
Wrap
Text File
|
1992-06-16
|
47KB
|
1,274 lines
Help Information: Place
Manually Place Pads, DIPs, SIPs, 2-Pin devices (resistors,
capacitors, diodes, etc.), and Library Parts on the PCB.
They are Added or Deleted (when their corresponding
placement mode is selected) by Clicking with the LMB or RMB,
respectively, at the Device's Pin#1 location (except Library
Parts which can be Deleted by Clicking with the RMB anywhere
inside the Bound).
Manual Placement supports the requirement that some parts
have to be in certain locations (connectors, switches,
etc.).
DIPs, SIPs, 2-Pins, and Library Parts are the four basic
Device Types cross-referenced in the Part List to support
Guided (manual) Placement. If you have a Net List attached
to this PCB, calling up any of the Device Labels (in the
corresponding Device Type mode) will bring up a ghosted
Device with Guide Lines for all Nets which include Pins of
the Device. Orientation can be adjusted prior to Settling.
Pads have no labels; they are used as mechanical mounting
holes, multi-layer Trace connectors, or unlabelled Test
Points. You can manually Route to them under `1Layer' and
`Wide', but none of the autorouting functions will consider
them except `1Lay' (which uses the Maze algorithm.
Thermos are etch patterns made around Pins which connect to
the Power Planes (<V>oltage and <G>round) to increase the
reliability of solder connections as well as identify the
Pins.
Boxes and Circles under Place are different than under Draw.
Available Work layers are <P>ad Master, Component, and
Solder layers. You cannot draw Boxes or Circles on the
<L>abel, <V>oltage, or <G>round layers or any Signal layer
other than 1 or 2 (the Component and Solder layers).
Device orientation is determined by one of the four
orientation IFKs Selected prior to Placement. If you decide
to alter the orientation after Placement, enter
Improv/Rotate.
You may Move a Device singly or in a group of Parts. Traces
already routed to a Device are Deleted when the Device is
Moved unless both ends of the Trace are also Moved.
Help Information: Auto Place
Automatic Placement mode. Pro-Board V3.0 will analyze the
Net List connections and determine Device Placement for
minimum Trace length based on the Placement Grid and Device
FootPrints.
After the Devices which must be in a certain location are
specified in (manual) Place, Glue the Parts (Devices), Group
them (reduces Placement time), set the PGrid, Orientation,
and F-Areas, and let Pro-Board determine the optimum
Placement for minimum PCB area and trace length.
The usual procedure is to Glue any Parts which were manually
Placed, such as goldfinger edge connectors, jacks,
potentiometers, etc. Also, the autoplacement routine starts
with the Part having the most connected Pins in any Group,
so it is advisable to Place the largest Part in each Group
manually and Glue it before invoking the autoplacement
routine.
Groups are collections of Parts which are known to be
physically close to each other. While not strictly
necessary for the autoplacement routine to function,
separating the Parts into Groups will reduce calculation
time and, often, improve Placement.
Autoplacement has two modes of operation. Pass1 determines
optimum placement within a Group. As each new Part is
considered for placement, other Parts may be ripped up and
repositioned to provide the lowest cost. If you have more
than one Group of Parts which have been autoplaced, Pass2
will look at the Selected Groups and adjust the orientation
to minimize the Cost of interconnecting the Groups.
The recommended autoplacement procedure is to Group the
Parts which are not yet Placed with the Glued Parts they
will be near. Specify the Orientation options and set the
Placement Grid for each Group, then Select that Group for
Auto-P and hit Go. Repeat for each Group.
Help Information: Route
Perform manual routing. There are three main Menus for
manual routing, 1Layer, 2Layer, and Wide.
1Layer is the basic single trace autorouter from Pro-Board
V2.0 and earlier. It allows Guided routing (forcing the
Trace to follow a specific path), easy Pin to Pin routing,
and Repeated routing (see 1Layer Help Screen for use).
2Layer allows for autorouting the Net connected to one Pin
or all the Nets connected to a Part. The same Channel
algorithm is used as in Auto-R with AnyVia mode specified,
but there is not as much control.
Wide allows specifying ten Trace Widths from 12 to 400 mils
and routing either manually or automatically by Net.
NetOpt analyzes PCB layout and reorders the Net List to
provide the shortest Guide Lines.
Via allows you to place Vias at random or with a constant
offset. Vias are small connector points to all Signal layers
(but not to Power or Ground planes).
Tile and Shrink support altering sections of a Trace.
Modify provides several tools for rearranging Traces to add
Parts or meet other needs.
Check analyzes Placement & routing for the entire PCB and
sends the results to one of three destinations, or checks a
specific Pin and sends the results to the Workbench screen.
Help Information: Auto Route
Automatic routing mode. The various IFKs in this mode let
you specify the Routing Rule, which Nets or Pins to
autoroute, the order in which they are routed, and areas to
avoid when routing.
Forbidden areas (F-Area) are useful when you have to keep
clear areas for mounting brackets or are going to mix
various device types, such as Analog and Digital components,
on the same board but want to keep the signals separate.
Before autorouting a group of Nets, specify which areas are
to be avoided on each Signal layer.
The Routing Rule allows you to specify several options for
the autorouter. See the Routing Rule screen in the manual.
0Via allows only vertical or horizontal Traces with
slight deviations controlled by the Channel Width
selector.
1Via
2Via will Route a Selected Net only if it can be done
with the allowed number of Vias.
AnyVia will allow more Vias to connect a Trace.
AnyPath expands the limits that the autorouter will
search for an available path to Route the Trace.
Trace Width allows selecting the width of the Traces to
Route, but only the 12 mil Traces will
connect at 45 degree angles.
Speed trades off `thoroughness' versus `speed'.
`1' is fastest and `5' gives the best chance of
success for difficult boards.
Also controls the number of retries when the
`RipUp' option is specified.
Channel Width controls the allowable deviation from
horizontal or vertical before a Trace is
forced to change layers to make a connection.
Also controls the `0Via' autorouting mode.
SelNet selects the Nets to autoroute. It is not always
best to Select every Net for routing and just turn the
autorouter on. Sometimes, it is best to autoroute only
sections of a board or only certain Nets. The IFKs under
SelNet support easy selection.
The autorouter can be `guided' by specifying that certain
Nets will be considered before others. Entering a Weight
for a Pin or Net under SetWei aids this process.
RipUp is an option that allows the autorouter to ReRoute the
Nets in a different order to increase the success rate of
the entire board. Note that RipUp doesn't remember the best
routing order. If it fails to completely autoroute, you
will be left with the results of the last attempt, not the
best attempt.
ReRoute differs from Go in that it will use all the Selected
Nets and Pins. Go will only use Selected Nets and Pins
which are not already routed.
Via optimization (ViaOpt) is a powerful command that
analyzes the specified Nets and applies the Maze algorithm
to improve the routing. It will delete and reroute the
Traces several times to eliminate as many Vias as possible.
Help Information: Draw
The IFKs under this heading allow you to place Lines, Text,
Circles, and Boxes on your PCB. All modes work on the
<L>abel, <V>oltage, <G>round, and Signal Pair layers. In
addition, Circles can be drawn on the <P>ad Master layers.
Compare limitations with BoxCir
Help Information: Rule
Bring up the Design Rule screen.
The Design Rule screen is the same as the one brought up
with NEW, but some of the choices made when first defining
the PCB cannot be changed, specifically Fine Line, Trace
Orientation, and Signal Layer Pairs. In addition, the PCB
Width and Length may be increased, but not decreased.
The most used reason for returning to the Design Rule during
PCB creation is to load a new Net List. If you have enough
memory, Pro-Net can run at the same time as Pro-Board.
Modifications can be made to the schematic so a new Net List
can be generated for use very quickly.
To exit the Design Rule screen after any changes, enter OK.
A question on the Entry Bar will ask if you have changed the
Net List. A Yes answer will load the Net List and Part List
and cross-check them. If you specify a new Net List name,
<NETname>.NET, be sure to have a Part List with the same
base name, <NETname>.PAT.
Exit (the Escape key or Clicking the Right Mouse Button
while the cursor is over the IFK region at the bottom of the
screen) will return from the Design Rule screen without any
changes.
Help Information: Set Reference
Specify a local origin. Useful when the default origin does
not lie on an irregularly shaped PCB or for more convenient
coordinates for some operations (specifying a Box or Library
Part Placement with Comm, for instance).
Help Information: Border
The Border is a requirement for proper results. During
automatic or manual Placement and routing, the Border will
prevent Devices or Traces from extending outside the
specified area. It is also useful for microcomputer add-in
boards with cutouts for Goldfinger edge connectors.
The Line segments drawn will be Purple until you Select
Next, at which time the Border will turn Gold, closing the
polygon if necessary. While it is possible to draw an
irregular polygon (edges cross each other), it is not
recommended. Line segments are not restricted to horizontal
or vertical, so pay attention to the coordinate display at
the lower right of the screen.
Help Information: Post
Post Processing. Write information and statistics on
current PCB to the Data Disk.
.BPrt lists the Device Labels for each Part and associated
FootPrints. This information will normally be included in
the <NETname>.PAT file, but <PCBname>.BPrt will reflect the
Parts actually on the PCB (including extra Parts not in the
Net List), not the file generated by Foot-P from reading the
Net List.
.BTGrp lists the Trace Groups actually in use. Presented in
a Net List format, the Net names will be replaced with the
Tra# prefix and the ordering of the Trace Groups will
reflect actual usage by Pro-Board, including separated Nets
(i.e. two or more sections of a Net are routed, but not
interconnected) and extra Traces. Nets in the Net List
which are not routed will not be referenced in this list.
.BStat provides statistical information useful in estimating
cost and labor charges, including board size, number of Pins
& Vias, and the number of Signal layers.
Help Information: Edit Board
The root menu for PCB editing. From here, every available
operation can be performed except File Selection, File
Management, FootPrint generation, and Configuration.
Rule returns you to the Design Rule screen where you
originally specified the parameters for the PCB.
SetRef allows you to specify a Local Origin which is used by
the coordinate display at the lower right of the screen.
Border is required for limiting the area in which a Device
can be placed or a Trace routed. You can also draw the
outlines of irregular PCBs (such as microcomputer add-in
cards with Goldfinger edge connectors).
Place allows manual placement of all Devices (i.e. those
with Pin numbers).
Auto-P is the Automatic Placement menu. Here you can set
Forbidden Areas to prevent Parts from occupying the space
set aside for brackets and connectors; specify the
allowable Orientation for Parts when they are placed; Glue
those Parts which are already Placed so that they won't be
moved when the autoplacement function kicks in; specify a
Placement Grid to limit the points where a Part can be
Placed; Group Parts which you know will be close so the
autoplacement function doesn't have to slow down by
considering every Part at the same time; Place the Parts
within a Group (Pass1) and optimize the interconnections
between Groups (Pass2); Delete Parts (-Part) and Improve the
placement of Parts on the PCB.
Help Information: Draw Line
Draw Lines on any layer except the <P>ad Master layer.
End a Line or sequence of Lines with the Next command.
You can draw closed, hollow polygons by Clicking the last
point over the first point before pressing Next.
Selecting Fill allows drawing Filled polygons. R0, R1, R2,
& R3 specify radii for corners. After at least three points
have been specified, enter Next to close the polygon. The
radii of Filled polygons are listed below:
Setting Radius
------- -------------------
R0 none (sharp corner)
R1 55 mils
R2 60 mils
R3 65 mils
Note that the <V>oltage and <G>round layers are displayed in
reverse, so any lines drawn on them will be bare board
surrounded by Copper.
If you wish to separate the <V>oltage or <G>round layers (to
isolate Analog and Digital Power Planes, for instance), it
would be better to use the Box command. It is easier and
faster to lay out the 1/4" separation that is recommended
for separating Power Planes on one layer than using the Line
command to outline the same area.
Help Information: Draw Text
Write text on any Work layer except the <P>ad Master layer.
Position cursor at desired text position. Select Vertical
or Horizontal orientation and Text Size (Small or Medium),
then enter a Text String in the prompt on the Entry Bar.
Text will appear at the cursor, but is not yet Settled
(fixed in position). Click to Settle the text. To move the
text before Settling, Drag (press and hold the Left Mouse
Button while moving the cursor) the text to the desired
location.
The cursor should be over the main screen (i.e. not over the
IFKs or the Entry Bar) when text is entered in the prompt
(with the Enter key). At that time the entire Entry Bar
blanks, including the DISPLAY and WORK gadgets.
If you forgot to position the cursor over the main screen
before entering the Text String, you can Drag the text to
the desired position and Settle it (starting a Drag
operation moves the Text String to the cursor no matter
where the Text String was).
Help Information: Draw Circle
Draw a Circle on the layer specified by the WORK gadget (not
allowed on every layer in every mode).
Click at the location for the Center of the Circle, then
Click at a point on its Radius.
If the Fill option is available and activated, the Circle
will be solid. Otherwise, it is hollow.
The wedges control which quadrants of the Circle will be
drawn.
Comm allows entering the coordinates of the Circle and its
radius via the keyboard for more precise positioning. The
mouse is limited to multiples of 25 mils (Standard mode) or
20 mils (Fine Line mode), but Comm allows an accuracy of 1
mil (0.001").
Help Information: Draw Box
Click the Mouse Cursor at the diagonals of the rectangular
area to be marked. A Box will be drawn in a somewhat
identifiable manner in the color of the Work layer.
Mode Appearance Layers
------------- ---------------- ---------
Auto-P/F-Area Dashed P, C, S
Auto-R/F-Area Horizontal Lines Signal
Draw Filled or Hollow Any but P
Place/BoxCir Dashed P, C, S
Route/F-Area Horizontal lines Signal
Remember to check the Work Layer before starting this
function.
Help Information: Set Routing Weight
Specify a Weight for an autorouting priority. Allowable
values are 0 to 255.
If Weights are not set on Pins or Nets, the Traces will be
autorouted in order of occurrence in the Net List. If some
Traces do not route because other, previous, Traces block
Pins, specifying the order in which these Nets are presented
for routing will improve your success rate.
The RipUp option in Auto-R will increase the Weight of any
Traces which fail to Route to increase the routing success
rate.
AllNet will display a prompt to set the Weights for all the
Nets. ByPin and ByNet control the range over which weights
are applied when a single Pin is Clicked.
Weights set for Signals assigned in Pro-Net are not
considered as their only purpose is to set the order of the
Nets in the Net List.
Help Information: Set Routing Pin Pair
Select and Display connections to be autorouted. A Pin or
Net must be Selected for the autorouter to consider it. If
a Guide is Displayed, but not Selected, it will be Displayed
in White. If Selected, it will be Displayed in Cyan.
Outside of this area, only Selected Guides will be displayed
(in White) until you invoke one of the functions which
control Guide Line display.
For the purposes of description, a Net is the sequence of
Pins to be connected with Traces. It is displayed as a
sequence of white Guide Lines. A Net Segment is two Pins
which end a Trace, shown by a single Guide Line segment.
AllNet: If Nest is specified, Select all Nets for
autorouting. If Remain is specified, those Nets which are
not completely Routed will be Selected. Note that any Nets
which were already Selected will remain Selected. See also
[Auto-R/]Go and ReRout.
NoNet: If Nest is specified, DeSelect all of the Nets. If
Remain is specified, DeSelect only those Nets which are
Routed.
Nest sets the widest scope for the AllNet and NoNet
functions. It is mutually exclusive with Remain.
Remain limits the scope of the AllNet and NoNet functions.
ByPin: Click on a Pin to Select the one or two Net Segments
that connect to the specified Pin.
ByNet: Click on a Pin to Select the entire Net which
includes the Pin.
ByBox: Specify the diagonals of a Box that surrounds the
Pins to be Selected. You can Select some or all of the Pins
of a Device. Only the Net Segments which include the
Specified Pins will be Selected.
ByPat: Click on any Pin of a Part (Device) to Select all the
Net Segments which include its Pins.
Help Information: Forbidden Area
Forbidden Areas are used to keep clear areas of the PCB that
have mounting brackets, large screw heads, height
limitations, etc. that will not allow Devices.
While Forbidden Areas could also be used to speed the
autoplacement process, using different PGrids for different
Groups is better suited for this task as they can be saved
and reused.
Automatic Placement mode
------------------------
Use Circles or Boxes to mark areas that are not to be
considered for Placement of Devices. Can specify <P>ad
Master, Even, or Odd layers. The areas will be marked with
dashed lines or arcs.
Automatic or manual Routing
---------------------------
Use Circles or Boxes to mark areas that are not to be
considered for routing of Traces. Traces can be inhibited
on either the Odd or Even layers. To inhibit on both
layers, specify the same area on each layer. The <P>ad
Master and Power layers may not be specified as Traces
cannot route on those layers.
Set limits on or Guide the routing process. Very useful
when you want to keep Analog and Digital signals separate or
want to avoid routing to a Device on one layer (when
planning a pseudo-Ground Plane, for instance), or altogether
(by surrounding a Device with Forbidden Areas on both the
Even and Odd layers).
Help Information: Place Orientation
Specify the Orientation options for Automatic Device
Placement (Right, Left, Down, and Up). Any combination is
allowable.
While increasing the number of allowable Orientations will
increase the computing time, it will also improve the
chances that Devices can be Placed in some circuits. On the
other hand, limiting Orientation choices will improve the
layout in other circuits, as well as reducing assembly error
for Devices which are physically, but not electrically,
symmetrical.
Help Information: Glue Parts
Lock a Device's location on the PCB before autoplacing the
rest of the Devices.
Certain Devices must be in a specific location (connectors,
goldfingers, etc.). These Devices are specified in Place.
If autoplacement is desired for the remaining Devices, use
Glue to fix the position of the necessary parts or they will
be Deleted and repositioned during the automatic placement
process.
When invoked, all Devices which have not been Glued will be
ghosted. Select the proper Work Layer (usually <P>ad Master
unless the Device exists on only the Component or Solder
layer) and Click with the Left Mouse Button within the Bound
of the ghosted Device. It will now display normally to show
that it has been Glued.
To UnGlue a Device, Click inside the Device's Bound with the
Right Mouse Button.
The autoplacement routine finds the Device with the most
pins in each Group it is Placing and Places the other
Devices in the Group around it according to the PGrid,
F-Area, Orientation, and available space. If the largest
Device is not Glued, it will be Placed at the upper left of
the PGrid. It is therefore advised that you Glue the
largest Devices in each Group. Remember that you may adjust
Grouping for different levels of Placement.
Help Information: Set Placement Grid
The Placement Grid tells the autoplacement routine which
locations to consider for Device Placement. Parts are
Placed with Pin#1 on the selected Grid coordinate.
Orientation options are set in Orient.
PGrid is not required before autoplacement, but the results
may look less than professional as the autoplacement routine
won't be concerned if the Devices don't line up. The
default placement grid will dynamically adjust according to
the available area, the number and size of Devices, and the
perceived difficulty in routing the Devices (according to
the Net List of interconnections).
Obviously, the PGrid you specify must have enough grid
intersections for all of the Devices. You must also
remember that a Device may obscure one or more grid
intersections, reducing the number available for subsequent
Devices.
The PGrid may be constructed via the Mouse or Comm. In
addition, PGrids may be Saved and Loaded for use on multiple
boards, or repeated use on the same board after
modifications have been made to the Net List.
Regular spacing is supported by both the mouse and Comm
functions. Clicking the mouse at any two locations sets an
offset (Delta) for more PGrid lines via the Repeat key. The
Delta can also be set directly in the Comm function prompt
on the Entry Bar.
Help Information: Set Placement Group
Separate Devices into Groups for more efficient Placement.
While Grouping is not necessary, it greatly speeds the
autoplacement process. It also aids proper Placement of
Devices which interconnect with larger Devices.
It should be noted that Groups are only used to isolate
Devices for later Placement. While all 8 Groups can be
Selected at the same time, you can save time by Placing
Devices in one Group at a time with a PGrid restricted to
the desired area for just those Devices.
Devices with a Group Number of `*' cannot be Grouped. They
connect only to the Power and Ground Planes, not to any
Signal Nets.
The cursor controls (Up Arrow, Down Arrow, Page Up Arrow, &
Page Down Arrow) or the mouse can move the Highlight over
any Device. To manually change the Group of a highlighted
Device, enter a number from 0-7.
Device also supports manual Grouping of Parts. The Group
Number and Label prompts appear in the Entry Bar. This is
the fastest way to Group Parts because the order that Parts
are displayed on screen is unimportant. Once specified, the
Group Number becomes the default for any more Parts. Use
the <Backspace> key to clear the prompt and enter a new
Group number.
Batch Grouping of Parts is supported in the Reset and AutoGp
commands. Reset issues a prompt for the Group number to
apply to all the Parts. You can also manually assign Group
numbers to several `seed' Parts and let AutoGp assign the
rest according to the Net List connections. AutoGp will
work even without the `seed' values, but its results will
depend on the Net List.
Help Information: Delete Part
Click to specify the diagonals of a box surrounding the
Part(s) to be Deleted. They will ghost and Guide Lines will
list connections to Parts which are not tagged for Deletion.
Help Information: Improve Placement
Manually improve the Placement of Devices.
Select among Move, Rotate, and Swap.
Be sure to specify the proper WORK layer (usually the <P>ad
Master layer, except for single layer SMT Devices)
Move allows Selecting one or more Devices by Clicking to
define a box around the desired area. Devices which are
selected will ghost and Guide Lines will connect their Pins
to any other Pins not Selected for Moving.
Rotate a Device in 90 degree increments by Clicking on it
and specifying a rotational direction.
Swap two Devices by Clicking on each and verifying the
prompt. While Through-hole and SMT Devices can be Swapped,
you will have to Select the proper WORK layer for each
Device. Traces to any Pin will be deleted when its Device
is Swapped.
NetOpt analyzes Placement and reorders the Net List so the
Guide Lines between the Pins to be connected are as short
and direct as possible. Display the results with Nest or
the PinGui and PatGui functions.
Delete allows easier Deletion of Devices. Normally, you
have to enter each mode (DIP, SIP, 2-Pin, Lib, or Pad) to
Delete that type of Device. Select the proper WORK layer
(usually <P>ad Master) and Click to define the diagonals
of the box that surrounds the Devices to be Deleted. All
Selected Devices will ghost and Guide Lines will connect to
their Pins. A prompt will ask for verification.
Help Information: Block Move
You may Move a Device singly or in a group of Parts. Traces
already routed to a Device are Deleted when the Device is
Moved unless both ends of the Trace are also Moved.
Specify the Device(s) to Move by Selecting the proper WORK
layer (usually <P>ad Master unless the Part is a single
layer Surface Mount Device) and Clicking to specify the
diagonals of a box which surrounds the Device(s) to Move.
You will not be able to Move a Device and Settle it so that
a Pad is over a Trace or another Device, although any
drawing on Label layer may overlap Traces or Pins. You also
cannot Move a Device so that its Bound overlaps another
Bound, although the Bounds may touch. Prior to Settling the
Device with the LMB, you can cancel the operation with the
RMB.
Help Information: Rotate Part
Click to Select a Device for Rotation. Once Selected, it
will ghost and Guide Lines will display the Guide Line
segments which connect to its Pins.
The Device can be Rotated with the Rot+ and Rot- IFKs. You
can also Drag the Device to a new location by placing the
cursor over the Device, pressing and holding the Left Mouse
Button, and moving the cursor until the Device is
positioned.
Settle the Device by Clicking the LMB within its bound.
The Device cannot be Resettled if it overlaps another Device
or one of its Pins overlaps a Trace. Prior to Settling the
Device with the LMB, you can cancel the operation with the
RMB.
Help Information: Swap Part
Swap two Devices by Clicking on each and verifying the
prompt. While Through-hole and SMT Devices can be Swapped,
you will have to Select the proper WORK layer for each
Device. Traces to any Pin will be deleted when its Device
is Swapped.
You cannot Swap Devices if the Device Bound of one of the
two Devices would overlap another Device Bound (touching it
is OK). You cannot Swap Devices if a Pin would contact a
Trace. Prior to Settling the Device with the LMB, you can
cancel the operation with the RMB.
Help Information: Block Delete
Delete allows easier Deletion of Devices. Normally, you
have to enter each mode (DIP, SIP, 2-Pin, Lib, or Pad) to
Delete that type of Device. Select the proper WORK layer
(usually <P>ad Master) and Click to define the diagonals
of the box that surrounds the Devices to be Deleted. All
Selected Devices will ghost and Guide Lines will connect to
their Pins. A prompt will ask for verification.
Help Information: Label Hidden
The device label can be hidden from view by Clicking within
its Bound with the Right Mouse Button.
If you decide later to display the label, Click within the
Bound with the Left Mouse Button.
Note that, if you had Moved the Device Label prior to Hiding
it, making the Label visible again will restore it to its
default position.
Help Information: Place DIP
Specify DIPs for Addition to or Deletion from the PCB. A
DIP is a Dual In-line Package device, such as a typical
Integrated Circuit `N' package. DIPs have a Pin separation
of 100 mils with a variable Row separation. They are fully
specified by entering the Device label and the values for
number of Pins and separation between rows of Pins. If you
need a different separation between the Pins in one row, you
can create a Device in Pro-Lib. DIPs are automatically
entered on the <P>ad Master layer.
Enter a Device Label.
If the Device Label is referenced in the Net List and
cross-referenced in the Part List, the number of Pins and
row separation is already known. The Device will be loaded
and ghosted for Placement. Guide Lines will connect any
Pins in the ghosted Device which share a Net with any of the
Pins in Devices already Placed.
If the Part List cross-references the Device Label to a
Device Type other than a DIP, you will get an error. Switch
to the proper Device Type entry mode or alter the Part List
to call out a DIP and reload the Net List under Rule.
If the Device Label is not referenced in the Net List, you
will be prompted to continue with Placement. If the Device
Label is also not referenced in the Part List, you will have
to specify the DIP. If the Device Label has been referenced
in the Part List, the DIP will be loaded and ghosted for
Placement.
If there is no Net List, you will have to fully specify the
DIP.
If the Device Label is in the Net List but is not
cross-referenced in the Part List, you would have received a
Net List error before leaving the Design Rule screen and
will have no Net List or assistance in Placement or routing
for any Device.
Once the DIP has been called out, but before it has been
Settled, verify that the Orientation is as desired, Drag it
if necessary, then Click to Settle.
Help Information: Place SIP
Specify SIPs for Addition to or Deletion from the PCB. A
SIP is a Single In-line Package device, such as a resistor
network, with a Pin separation of 100 mils. SIPs are fully
specified by entering the Device Label and the number of
Pins. If you need a Pin separation other than 0.1", you
will have to create a Library Part in Pro-Lib. SIPs are
automatically entered on the <P>ad Master layer.
Enter a Device Label.
If the Device Label is referenced in the Net List and
cross-referenced in the Part List, the number of Pins is
already known. The Device will be loaded and ghosted for
Placement. Guide Lines will connect any Pins in the ghosted
Device which share a Net with any of the Pins in Devices
already Placed.
If the Part List cross-references the Device Label to a
Device Type other than a SIP, you will get an error. Switch
to the proper Device Type entry mode or alter the Part List
to call out a SIP and reload the Net List under Rule.
If the Device Label is not referenced in the Net List, you
will be prompted to continue with Placement. If the Device
Label is also not referenced in the Part List, you will have
to specify the SIP. If it has been referenced in the Part
List, the SIP will be loaded and ghosted for Placement.
If there is no Net List, you will have to fully specify the
SIP.
If the Device Label is in the Net List but is not
cross-referenced in the Part List, you will have received a
Net List error before leaving the Design Rule screen and
will have no Net List or assistance in Placement or routing
for any Device.
Once the SIP has been called out, but before it has been
Settled, verify that the Orientation is as desired, Drag it
if necessary, then Click to Settle.
Help Information: Place 2-Pin
Specify 2-Pin to Add or Delete 2-Pin devices on the PCB. A
2-Pin is a device such as a typical resistor, capacitor, or
diode. 2-Pins are fully specified by entering the Device
Label and the separation between the two Pins. They are
automatically entered on the <P>ad Master layer.
Enter a Device Label.
If the Device Label is referenced in the Net List and
cross-referenced in the Part List, the Pin separation value
is already known. The Device will be loaded and ghosted for
Placement. Guide Lines will connect any Pins in the ghosted
Device which share a Net with any of the Pins in Devices
already Placed.
If the Part List cross-references the Device Label to a
Device Type other than a 2-Pin, you will get an error.
Switch to the proper Device Type entry mode or alter the
Part List to call out a 2-Pin and reload the Net List under
the Rule.
If the Device Label is not referenced in the Net List, you
will be prompted to continue with Placement. If the Device
Label is also not referenced in the Part List, you will have
to specify the separation. If the Device Label you enter
has already been referenced in the Part List, the 2-Pin will
be loaded and ghosted for Placement.
If there is no Net List, you will have to fully specify the
2-Pin.
If the Device Label is in the Net List but is not
cross-referenced in the Part List, you will have received a
Net List error during the check performed before leaving the
Design Rule screen and will have no Net List or assistance
in Placement or routing for any Device.
Once the 2-Pin has been called out, but before it has been
Settled, verify that the Orientation is as desired, Drag it
if necessary, then Click to Settle.
Help Information: Place Lib Parts
Specify Library Parts for Addition to or Deletion from the
PCB. A Library Part is a custom device with an atypical
footprint, such as a connector mount, a PGA or PLCC IC, a
goldfinger edge connector, etc. Library Parts are fully
specified by entering the Device Label and Library Part
name.
Enter a Device Label.
If the Device Label is referenced in the Net List and
cross-referenced in the Part List, the Library Part name is
already known. The Part will be loaded and ghosted for
Placement. Guide Lines will connect any Pins in the ghosted
Part which share a Net with any of the Pins in Devices
already Placed.
If the Part List cross-references the Device Label to a
Device Type other than a Library Part, you will get an
error. Switch to the proper Device Type entry mode or alter
the Part List to call out the Library Part and reload the
Net List under the Rule.
If the Device Label is not referenced in the Net List, you
will be prompted to continue with Placement. If the Device
Label has been referenced in the Part List, the Library Part
will be loaded and ghosted for Placement. If the Device
Label is also not referenced in the Part List, you will have
to specify the Library Part.
If there is no Net List, you will have to fully specify the
Library Part (enter both the Device Label and the Library
Part name).
If the Device Label is in the Net List but is not
cross-referenced in the Part List, you will have received a
Net List error before leaving the Design Rule screen and
will have no Net List or assistance in Placement or routing
for any Device.
Once the Library Part has been called out, but before it has
been Settled, verify that the Orientation is as desired,
Drag it if necessary, then Click to Settle.
Help Information: Place Pad
Pads have no labels; they are used as mechanical mounting
holes, multi-layer Trace connectors, or unlabelled Test
Points. They are not called out in the Net List, nor are
they cross-referenced in the Part List. If you need to have
a one (1) pin Device, use a one (1) pin SIP so that a label
can be assigned.
Help Information: Place Thermo
Thermos are etch patterns made around Pins which connect to
the Power Planes (<V>oltage and <G>round) to increase the
reliability of solder connections as well as identify the
Pins. They work by restricting heat flow away from the Pin
during the soldering process. This helps prevent the Device
from overheating during the soldering process.
Help Information: Forbidden Box & Circle
Boxes and Circles used to specify Forbidden Areas have two
distinct appearances, depending on whether they are blocking
Device Placement or Trace Routing.
Boxes and Circles which prevent Device Placement are
displayed with dashed lines or arcs. They may be drawn only
on the <P>ad Master, <C>omponent (Layer 1), or <S>older
layers (Layer 2) because those are the layers which can hold
a Device.
Boxes and Circles which block Traces from Routing through a
given area can only be drawn on the Signal Layers (marked
with numerals) as Traces cannot be Routed on the <V>oltage,
<G>round, or <P>ad Master layers.
Help Information: Coordinate Labelling
Standard Device Labels can be replaced with those
corresponding to coordinates applied to the PCB under the
XYMark function.
Coordinates are arranged in a non-linear manner according to
Device Placement so that densely packed Parts in one area of
the PCB do not have the same label.
Help Information: One Layer Router
1Layer is the basic single trace autorouter from Pro-Board
V2.0 and earlier. It allows Guided routing (forcing the
Trace to follow a certain path) and easy Pin to Pin routing.
Repeated routing draws identical Traces, where possible.
The Guide+ and Guide- functions search for incorrect
(incomplete or extra Traces) Nets.
Remain displays all incorrectly routed Nets.
PinGui displays Guide Lines for individual Nets, specified
in the prompts or by Clicking on the Pin.
PrtGui displays the Guide Lines for an entire Device,
specified in a prompt.
NoGuid erases Guide Lines from the display.
ViaEnd inserts a Via and switches Signal layers to continue
Routing. It is an aid for quickly routing on two layers
under manual control.
TilEnd ends a Trace with a Tile.
Help Information: Two Layer Router
2Layer allows for autorouting the Net connected to one Pin
or all the Nets connected to a Part. The same Channel
algorithm is used as in Auto-R with AnyVia mode specified,
but there is not as much control. It is faster than
entering Auto-R and Selecting all the options.
The two routing commands are PinRou (Route the Net which
includes this Pin) and PrtRou (Route all Nets which include
any Pin in this Device). All Traces on the Net will be
autorouted, including sections which aren't directly
connected to the Pin or Part.
The Guide+, Guide-, and Remain functions aid in finding
incorrect Nets.
Help Information: Wide Trace Router
Wide allows specifying ten Trace Widths from 12 to 400 mils
and routing either manually or automatically by Net.
Guide+ and Guide- find incorrect (incomplete or extra Pins)
Nets.
PinGui selects an entire Net by entering the Device Label
and Pin number at the prompt or by Clicking on the Pin.
RouNet autoroutes the displayed Net.
NoVia specifies that Traces can switch Signal layers only at
Pins (used during RouNet). No Vias will be added to
facilitate routing.
ViaEnd adds a Via and switches Signal layers during manual
routing.
TilEnd adds a Tile and ends the Trace. If a Tile is Shrunk
without having been connected to another Trace section, the
Trace will be Deleted.
Next allows ending a Trace at any time without having to
connect to a Pin or Add a Via or Tile.
Help Information: Place Via
Vias are similar to Pads, though usually smaller, in that
they are present on all layers, but are usually used as
transition points as Traces change layers, not as end
points.
Help Information: Place Tile
Tiles are used for modifying Traces. Applied to a Trace,
one section can be Deleted without affecting the other.
Used two at a time, the central section can be Deleted and
rerouted without affecting either end.
Like Traces, Tiles can only exist on the Signal layers (the
Even and Odd Pairs). Be sure to Select the proper WORK
layer.
While Open and Push have their uses, Tile allows for more
flexibility and control in modifying a Trace. The entire
Trace segment between a Tile and a Pin, Pad, Via, or another
Tile can be Pushed, Opened, or even Deleted and rerouted
without affecting the other sections of the Trace. This is
useful when modifying an area of the PCB to Add a Device, or
simply to adjust the Trace to suit your needs for signal
distribution or isolation.
Tiles can be Placed independently of a Trace. You can also
route to a Tile in 1Layer (manual) mode. But the
autorouting algorithms in 2Layer and Auto-R will not route
to a Tile.
After you have finished your modifications and the Tile has
two Trace segments connected, Shrink the Tile to get rid of
it.
If there is only one Trace segment connecting to a Tile when
it is Shrunk, the Trace segment back to the next Pin, Pad,
Via, or Tile will be Deleted.
If you Delete a Tile, it will Delete the Trace attached to
it back to the next Pin, Pad, Via, or Tile, even if there
are two Trace segments at the Tile.
Help Information: Shrink Tile
Remove a Tile. This is done after all modifications to the
Trace have been performed. The Trace must connect to a Pin,
Pad, Via, Tile, or another Trace at both ends.
Shrinking a Tile that has only one Trace segment attached
will Delete the Trace back to the next Pin, Pad, Via, or
Tile.
Help Information: Trace Modification
Provides a selection of tools for modifying Traces.
Open and OpenAl are used to move a Trace or group of Traces
by specifying an outer box to limit the scope and an inner
box to set the area to avoid.
Push will move a vertical or horizontal section of a Trace.
ReRout and Tauten are used to clean up Traces.
Trace and Via are duplicated from the 1Layer menu to allow
Adding new Traces the same as in 1Layer mode.
Tile and Shrink allow modifying sections of a Trace.
Help Information: Connectivity Checking
Select the destination and Go to receive a report of all
missing or extra connections according to the Net List.
ToTube sends the output to the window on the Workbench
screen.
ToPrin sends the output to PRT: device. Refer to your
AmigaDOS manual for configuraing your system.
ToFile brings up a prompt to specify a file to receive the
output.
Use Query to find any Pin on any Device and display the
Guide Lines for the connections to it.
Help Information: Show Guide Line by Pin
Display the Guide Lines for a Net at any Pin by entering the
Device Label and Pin Number at the prompts on the Entry Bar
or by Clicking on the Pin.
Help Information: Show Guide Line by Part
Display Guide Lines which include the Pins of the specified
Part (Device). Specify the Device by entering the Device
Label in the Entry Bar prompt.
Help Information: Pin Pair Router
Display the Guide Lines for a Net at any Pin by entering the
Device Label and Pin Number at the prompts on the Entry Bar
or by Clicking on the Pin.
Help Information: Part Router
Route every Net which includes Pins of the specified Part.
Specify the Part by entering the Device Label at the prompt
on the Entry Bar. Note that the entire Net will be routed
for the Selected Pin, not just the connections to the
closest Pins. If you wish to Route a partial Net around a
Part, use ByPat or ByPin under Auto-R/SelNet.
Help Information: Net Router
The index lists this function as RouNum. I don't even know
where it is. If you actually read this from the <Alt><Help>
function in Pro-Board, would you mind letting us know where
you found it?
Help Information: Trace Width Selector
Specify the Trace Width to be used when Routing. Note that
any Trace Width other than 12 mils will only connect at 90
degree increments.
Help Information: Open Space
Open an area on one signal layer by moving the Traces to
avoid a given rectangular block. This is used to provide
room for a Pad, Part, or another Trace.
Select the Odd or Even Work layer as needed and Click twice
to specify the diagonals of an Outer box which will limit
the range a Trace can be Opened. Then Click twice to
specify the Inner Box covering the area the Traces are to
avoid. If possible, Open will reroute the existing Traces
outside the Inner Box. If not possible, you will be
notified on the Entry Bar.
OpenAl performs the same function on every Signal layer in
one operation.
Help Information: Push Trace
After Selecting the proper Work Layer (Even or Odd), Click
on a non-diagonal (i.e. only Horizontal or Vertical) section
of a Trace, then Click to one side. The Trace will attempt
to move in that direction. The limit is a Pin, Pad, another
Trace, or a 125 mil deviation.
The entire section of the Trace must be able to move or no
operation will take place. It may be necessary to Tile a
Trace to Push a section of it.
Help Information: Reroute Trace
ReRoute a Trace by clicking on it.
After Traces have been Pushed or Opened and the necessary
additions made to the PCB, ReRout will `pretty them up'.
Select the proper Work layer and Click on the Trace.
If you Click on the Pin instead of the Trace and there are
two Traces connected to the Pin, only the most recent Trace
will be ReRouted. For preferred results, Click on the Trace
instead of the Pin.
Help Information: Route Trace
This is the single trace autorouter used in 1Layer. It has
been duplicated under the Modify Menu for convenience when
modifying Traces. You may route by Clicking on the end
points of the Trace, or you may Guide the Trace by Clicking
at points on the PCB through which the Trace must travel.
Help Information: Tauten Trace
Stretch a Trace between two points.
After Pushing or Opening a Trace, Tauten allows clean-up of
the Trace a section at a time. Click on one section of the
Trace to be stretched. A crosshair marker like that when
specifying a Box will appear. Click on a section of the
Trace on the other side of the region to be corrected. This
differs from ReRout, which will redraw the entire Trace from
Pin to Pin as shown by the Guide Line.