Aminet 1 (Walnut Creek)

home *** CD-ROM | disk | FTP | other *** search

/ Aminet 1 (Walnut Creek) / Aminet - June 1993 [Walnut Creek].iso / aminet / biz / demo / pbdemo303.lha / PRODEMO.LHA / pb.htex < prev next >

Wrap

Text File | 1992-06-18 | 51KB | 1,372 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 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 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 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 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 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 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 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 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 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 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 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 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 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 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 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 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. Help Information: File Management Pro-Board and other Prolific E-CAD products manage files by means of indices. For Pro-Board, the file BOARD maintains an index of the PCB files in the Data directory or disk. This practice is a carry-over from the first release of Pro-Board back in 1987 when almost all users had only floppy disk storage. Reading one small file was much faster than performing a wild card listing. Even today, with Pro-Board installed on hard drives, many users still store their PCB data files on floppy. The main drawback of this system is that Pro-Board File Management MUST be used to Copy, Rename, or Delete PCB data files. To Copy, Rename, or Delete a file, it must be highlighted. The Page Display IFKs move through screens of files and the Up and Down Arrows move the Highlight Bar to the desired file. Once set, Select the desired operation. Copying files Highlight the desired file. To copy a file to a new name in the same data disk, enter the new PCB name in the prompt. To copy a file to another data disk with the same PCB name, enter the volume name of the data disk. To copy a file to another data disk with a new PCB name, enter the volume name of the data disk and the desired name. Renaming files Highlight the file to rename and invoke Rename. Enter the new name in the prompt. Deleting files Highlight the desired file and invoke Delete. You will be presented with a prompt; answer `Y'. Help Information: Footprint A Footprint describes to Pro-Board the physical layout of the Device it is placing. A Part List file must cross-reference each Device Label found in the Net List with its footprint. Foot-P will prompt for a Net List name (not the PCB name, although they can be the same). Do not enter the .NET suffix. The Net List will be read and the Device Labels will be displayed in order of occurrence. For each Device Label, you must specify whether it is a DIP, SIP, 2-Pin, or Library Part by Selecting the appropriate IFK. Once the type of Device has been specified, enter the required information in the prompts. As new data is entered in each prompt for a Device type, it becomes the new default. If each DIP in your design has 16 Pins and a 300 mil Row Separation, you will only have to specify DIP and hit the <Carriage Return> key when the Devices are Highlighted. It would be helpful to generate the Bill Of Materials (BOM) when Post Processing is performed in Pro-Net and print it out for reference. Once finished, the Part List will be saved with the same base name as the Net List, but with a .PAT suffix. Help Information: Configuration screen At this screen, use the mouse to Click on the Plotter, Photo Plotter, and Drill File formats that meet your needs. Enter the Data and Lib disk paths in the prompts. Paths must end with either a `:' or `/'. A `:' indicates a Disk or Volume assignment. A `/' at the end of a string would point to a sub-directory. If you prefer, you can ASSIGN (see your AmigaDOS manual) a a name to a sub-directory path and use it. Adding this Assignment to your StartUp-Sequence or User-StartUp files will make it available each time you boot your system. The `Save' and `Use' IFKs allow setting default and temporary configurations. The file `pcb.conf' contains all the default settings.