Boldly Go Collection

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

/ Boldly Go Collection / version40.iso / TS / 05B / PCTRACE5.ZIP / PCTRACE.DOC < prev next >

Wrap

Text File | 1992-06-21 | 135.8 KB | 3,084 lines

PCTRACE Version 5.0 Users Manual June 21, 1992 by Douglas E. Ehlers Ehlers Technical Consultants 4520 S. 58th St. Lincoln, NE 68516 (402) 435-8440 Voice (evenings) (701) 642-3846 BBS 9600,N,8,1 V.32, V.42bis 2 Table of Contents Notice of Copyright............................................3 Introduction...................................................4 Installation...................................................4 System Requirements............................................5 Software Setup.................................................5 Old file Upgrades..............................................6 User support Methods...........................................6 Voice.....................................................6 BBS.......................................................7 Input/Output Menu..............................................8 Board Definition Menu..........................................9 Chip Placement...........................................10 Interactive Router............................................14 Mouse use................................................18 Autorouter....................................................18 Board Statistics..............................................19 Printer Menu..................................................21 Export Menu...................................................21 Exiting the program...........................................22 Tutorial......................................................24 RPRINT Subprogram.............................................26 DEFGEN Subprogram.............................................28 PC-Trace Keyboard control summaries...........................32 Schematic CAD.................................................33 Drawing Symbols..........................................36 Entering Components/Symbols..............................40 Making Connections.......................................43 Additional Drawing Commands..............................44 SCAD active keys.........................................49 Conclusions...................................................50 Appendix A - .NLT file format.................................51 PC-Trace Users Manual 3 Notice of Copyright This program is protected by a copyright held by the author and filed with the United States Government. Copying of this software is forbidden and a criminal offense. Anyone caught distributing this software without the author's consent will be prosecuted to the fullest extent of the law. Note: This program was originally marketed under the name PCROUTE but for copyright reasons has been renamed to PCTRACE. SCAD is short for Schematic CAD and is a schematic capture program that is part of the PCTRACE system. PC-Trace Users Manual 4 Introduction PCTRACE is a computer aided design program for printed circuit boards. It contains programs that can take the designer from a schematic, to a board layout, to computer control of the machines needed to make high quality circuit boards. The program should be quite adequate for most purposes. This program is not meant for IBM's use to design the next PS/2 motherboard. It is intended for the late-night engineer to build home projects. It contains a full featured autorouter that averages a 93% completion rate on low density boards and 70% on higher density boards. It also supports most popular printers for its output. PCTRACE is the general name given to all the programs that make up this system. For example, PCTRACE includes SCAD, RPRINT, and PCTRACE itself. Key features include: 1. Autorouting 2. Graphic interactive routing 3. Board layout functions 4. Flexible pinouts for devices 5. 2X and 1X output for use in making PC boards 6. Disk functions built into the software 7. Sophisticated component and connection entry systems 8. General statistics 9. Up to 300 components and 1800 connections 10. Mouse support in the interactive router 11. Variable pad and trace sizes 12. Single and double sided boards 13. Manual placement of traces 14. CGA, EGA, and VGA graphics support to display the board. CGA:80x25 EGA:80x43 VGA:80x60 15. Gerber, DXF, and Autocad Script file output 16. Actual size silkscreen creation 17. Error handling for critical errors 18. Schematic Capture for a complete cad system. 19. The authors continued support Installation Contents of PC-Trace directory: PCTRACE .EXE - The board layout/main program SCAD .EXE - Schematic CAD RPRINT .EXE - The PC-Trace printer output program SPRINT .EXE - The SCAD printer output program CONVCDT .EXE - Converts 4.0 and older files to 5.0 CONVDEF .EXE - Converts 4.0 and older files to 5.0 PC-Trace Users Manual 5 * .DEF - PC-Trace part layout files * .DIA - SCAD symbols System Requirements: To run this program requires: 1. CGA, EGA, or VGA graphics 2. 640k of memory with 520k free 3. 1 floppy disk drive 4. Hard Disk Drive or Large capacity floppy 5. One of the following printers: a. IBM PC or compatible printer b. EPSON LQ-2500 or compatible printer c. HP Laserjet II or compatible d. Adobe Postscript Compatible printer e. HP Deskjet or Deskjet + f. Epson MX-80 or compatible g. IBM Proprinter 24pin must be in AGM mode h. HP and Roland Plotters 6. Mouse is required for SCAD and usable in PC-Trace A fast processor and math coprocessor are also beneficial. Software Setup: For PCTRACE to run reliably, a line must appear in the config.sys files that says FILES=20. If any other major commercial software applications are in use this command probably exists, but it should be checked. To install the software insert disk 1 in either drive A: or B:. Change to the drive that the floppy disk is in. To do this type A: or B: from the dos prompt. To start the installation process, type INSTALL from the DOS prompt. The installation program will run and prompt for the drive that the install disk is in. Enter the letter and verify that it is correct. The next prompt is for the destination drive. This should be the letter of a hard-disk or alternate floppy disk that has at least 1mb of free space. Verify that the destination of the program is correct. The installation program will notify the user that it is ready to start the installation process and that Disk 1 should be placed in the disk drive. This should already be the case. Press SPACE to begin. After a few moments, a prompt will appear for the user to insert disk 2. If PCTRACE was shipped on a single floppy (3.5 inch) disk 2 is the same as disk 1. If the program came on two floppies (5.25 inch) insert the second disk. Press space to finish the installation. To execute the programs the user must change into the PCTRACE5 directory using the command CD \PCTRACE5. The programs PC-Trace Users Manual 6 will not run properly if run from some other directory than PCTRACE. To run the programs type PCTRACE, SCAD, or RPRINT from the DOS prompt. Install will also create two subdirectories called DEFILES and DIAGRAMS to store the definition files for PCTRACE and symbol files for SCAD. Two programs are included to help with the update process. CONVDEF.EXE is used to modify the old .DEF files that the user might already have created. To use this program, copy it into the subdirectory that holds the old .DEF files. Type CONVDEF, the program will run and update the file format of all the old files. CONVDEF can now be deleted from the hard-disk anywhere that it appears. The second program is used to update the .CDT files. This program requires that the .CDT file be in the same directory as CONVCDT.EXE. To convert the file, type: CONVCDT file1.CDT file2.CDT file3.CDT. The program will update the file from the 3.0 and 4.0 format to the 5.0 format. The old file will be saved in a .BAK file. One major consideration when moving a 4.0 file to the 5.0 system is the advanced silkscreening. The parts are referenced to a most upper left corner for placement, this includes silkscreen parts. If a part exists on an old board and is converted to the 5.0 program, that part should be left unchanged as far as silkscreen. If the silkscreen is drawn around that part, it will offset the location of the pads and the existing traces will not meet the pads in the correct place. This will be immediately visible as the affected parts will appear to have too many pads. If the user desires the silkscreen on the old board with the 5.0 software, they should be prepared to move components around in the interactive router to get the pads in the popper places. Traces that were overwritten by the incorrectly placed pad may have to be repaired as well. User Support Methods Phone Calls: All registered users are free to call anytime to notify the author of bugs, perceived bugs, program usage questions, suggestions of additions, and anything else that the end user feels the need to discuss with the author. The BBS is also a good way to receive support for the registered user. Un-registered users are also welcome to call during the evening when having problems getting the demonstration version of PCTRACE running. The support will be more limited. A better, and preferred method by the author, is for these users to use the BBS. PC-Trace Users Manual 7 BBS Support: Perhaps the best reason to register the demo version is to get the support of the registered user section on the BBS. The complete PCTRACE system is posted in this area for downloading. Upon registration all users receive a password on this system that allows them to download the most current bug fixes any time they like. The user name and password appear on the first page of the manual. Part and symbol libraries will also be posted and hopefully uploaded by users of the system. Other programs deemed useful by the author will be posted for all users as well as the demo version of the software. To access the BBS, call the number listed on the opening screen of the software with a modem control package such as PROCOMM or QMODEM. Support is provided courtesy of the author. Please feel free to log in to the BBS anytime. Voice calls should be at a decent hour and evenings are best. Please exhaust all possibilities before making the call and be sure to try and understand the problem before making the call to better explain it to the author. If it is possible, please try and isolate the problem to the point that it can be repeated by executing a certain sequence of events. By doing this, it becomes much easier to find and fix the errors in programming. PC-Trace Users Manual 8 PC-Trace Manual Input/Output Menu 1. Load Data: This function is used to retrieve from a disk necessary information to design a printed circuit board. Select this function from the menu and when prompted, enter the file name. No extension is used, the program will add the .CDT extension. The path should not be used on the filename itself. There is a function that will be discussed later to set the path name. After entering the filename, press Return. The program will ask if this is the correct name, enter Y or N to answer. If the file is not found the program will reprompt for file name. The ESC key is used to jump back to the main menu instead of entering the file name. 2. Save Data: This function will save a complete description of the design layout, component list, and connection list. When prompted, enter the filename. Again do not specify the file extension or path name. PCTRACE will ask, after entering the file name, if everything is correct. If so, enter a Y or N. If the file exists the program will ask if it is alright to overwrite the file. N will prompt for a new file name. ESC will bypass the prompt back to the I/O menu. 3. Erase Data: This routine clears the memory of the program. It erases the boards, component list, and connection list. The program will ask for confirmation before erasing the data in memory. Answer Y or N. The program will respond with "Erasing..." and after a few seconds drop back to the I/O menu. 4. Import Data: This load routine works the same as the primary load command in this menu. The difference is that it is made to load a netlist generated by SCAD. Creation of this file is covered in the SCAD manual. Once this file has been loaded, assuming that it is a complete design, all that remains is to place the parts, make any minor design changes, and autoroute the board. This is a best case scenario and more work is usually required. 5. Disk Directory: This function displays a listing of the all the circuit data files on the current drive and path. Use the space bar to view twenty file names at a time. When no more files PC-Trace Users Manual 9 exist, the space bar returns to the I/O menu. 6. Change drive/path: This function changes the current path. The ESC key will back out of the function without changing the path. The function will display the current drive and path and then prompt for a new one. Just enter the new one and press Return. Define/Edit Board Menu 1. Component Edit/Entry: This function is used to enter components into the system. Selecting this function will place the user in the entry/editing environment. If no components have been entered only two possible commands will be shown, if there are components in memory the programs shows options to delete, copy and perform other functions. New Component Entry: Typing an "A" will allow entry of new components. The program will display the component number being entered and then prompt for the name. The name may be up to 15 characters long and serves only to remind the designer of what the device is. ESC can be used at this point to return you to the entry/editing environment. The next question is for the designation. This is the unique name that is given to the component and will be used in the future to refer to it. Typical names include IC1, R1, IC2, and A1. There are two reserved designations. The first reserved designation starts with "V" and then a number, so V1 would not be accepted but VI1 would be. The second reserved designation is "GRNDP". If this is specified as a source or destination pad in the autorouter, a connection to the ground plane will be attempted if one is defined. ESC may be used to back up while entering the designation name to reenter the component name. Third, the program will prompt for the definition file name. This is the name of a file that tells the program how the pins on the device being entered are situated. The program first shows a list of possible definition file names at the lower right. At the end of the list the program will prompt for a name. Do not enter a file extension, the program will add it for you. If the name of the file entered exists, it will read the file and display the chip definition to see if it is correct. If the user answers "yes" the program will continue to the next question. If the user answers "no", the program will reprompt for the definition name after displaying the possible files. ESC may be used to back up and reenter the component designation. New definition files can be created with the subprogram DEFGEN. See PC-Trace Users Manual 10 that section of the manual for information on its usage. The fourth prompt asks for the pad size for the device. A small window will pop up and prompt for a pad size between 0.05 inches and 0.15 inches. All pads are circular. Enter the corresponding number to the pad size. The next question the program will ask if everything is correct. Answering "no" will restart this process with re- prompting for the name. Answering "yes" will get the next prompt. The next prompt is to keep this device. Answering "no" will skip the next prompt and ask if you wish to enter another device. Answering "yes" displays the next prompt. This prompt asks if the user wishes to place the device now. Entering "no" will allow the delay of this until later. All devices must be placed somewhere on the board before they can be connected. Placing a chip goes as follows: Placing Chips: When the graphic screen comes up a representation of the current circuit board with all other placed components and ground planes are shown. The chip being entered will be shown in the upper left corner of the board. The arrow keys will move this chip around on the board. By using a shift- arrow combination the chip can be moved faster. Move the chip to its final place and press return. Chips cannot be overlapped. The chip is now placed in this location. ESC will exit without placing the chip. Confirmation of abandoning the placement is asked. Yes will go to the next prompt, no will return to the place before hitting ESC. The last prompt is to enter another chip or not. Answering "yes" will put the user back at the name prompt to enter another chip. No will put the user back in the entry/editing environment. Editing Component Definitions: Selecting E from the entry/editing environment allows editing of any part of each definition. Simply select the letter of the item to change. For example, to change the name, press A after pressing E and enter the new name. Either enter the new name, or press ESC to leave it unchanged. When done editing, press the key that corresponds to exiting the edit. If editing the placement of chips, the chip definition file must be present in the DEFILES subdirectory for the placechip function to work. The only time this is a problem is if the board being edited is not your own, such that the chip definition files have different names from your own. PC-Trace Users Manual 11 Deleting Component Definitions: This function allows removal of a component. The component that will be deleted is the one currently displayed on the screen. Press D and confirmation will be asked for before deleting the component. Answer accordingly. All connections that contained the deleted function will also be deleted. Copying Components: This function will allow copies of a chip definition to speed the entry of chips. It will copy everything from the displayed definition to a new definition except for the designation from which it will take the alpha part and then increment the numerical part to the next available part. It also does not put the chip in the same location. The program will ask if the user wishes to place the chip now or later. Searching for a Component: Sometimes finding the component that needs to be edited or deleted can take some time on a large board. This function allows a search for components by designation. When prompted, enter the designation. PCTRACE will change the case to upper. If it exists, the program will display that device's number. If it doesn't exist, nothing happens. Incrementing and Decrementing the displayed Component: Using + and - will change the displayed component. + increments and - decrements. The display is circular in nature, therefore hitting + at the last component will move it to the first and hitting - at the first will move it to the last. Exiting the Entry/Editing Environment: Use the N key to end these functions and return to the board definition menu. 2. Connection Edit/ Entry: This system allows for entry and editing of all the connections that need to be made between the components in the system. The functions are very similar to the component functions. New Connection Entry: Typing an "A" will allow entry of new connections. The program will display the connection number being entered and then prompt for the name of the source designation. The name must exist in memory as a component. ESC can be used at this point to return to the entry/editing environment. If a ground plane has been defined, the reserved designation "GRNDP" can be used to connect to it. The associated pin is ignored and defaults to 1. The next question is for the source chip pin number. Enter PC-Trace Users Manual 12 the number of the pin that the trace is to connect to. ESC will back up to the previous prompt. The program will now prompt for the name of the destination designation. The name must exist in memory as a component. "GRNDP" can be used as a destination as well. ESC can be used at this point to return to the previous prompt. The next question if for the destination chip pin number. Enter the number of the pin that the other end of the trace is to connect to. ESC will back up to the previous prompt. The program will now ask if this is a priority route or not. By answering "yes", this trace will be routed before all other non-priority routes no matter how long it may be and what other routes it may block. This might be used for making sure a memory access bus is all done in copper instead of using jumpers for a vital connection. Next, the program will want to know the desired trace width. Traces from 0.01 to 0.07 are supported. Select the number corresponding to the size required. The following table will show what size trace will go between two pads of some size that are spaced on 0.1 inch centers. Pad Size (inches) Trace width 0.05 0.06 0.07 0.01 Yes Yes No 0.02 Yes No No 0.03 Yes No No 0.04 No No No 0.05 No No No 0.06 No No No 0.07 No No No These tolerances can be overridden using the interactive router which will be discussed later. The next question the program will ask is if everything is correct. Answering "no" will restart this process by reprompting for the source designation. Answering yes will bring up the next prompt. The next prompt is if the user wishes to keep this connection. Answering "no" will skip the next prompt and ask if you wish to enter another connection. Answering "yes" brings up the next prompt. The last prompt asks if another connection needs to be entered. Answering "yes", will put start back up at the source designation prompt to enter another connection. "No" returns the program back to the entry/editing environment. Editing Connection Definitions: Selecting E from the entry/editing environment will gives the user the ability to change any part of each connection. Simply select the letter of the item to change. For example, to PC-Trace Users Manual 13 change the source designation, press A after pressing E and enter the new designation. Either enter the new designation, or press ESC to leave it unchanged. Press N to exit the edit mode. Deleting Connection Definitions: This function allows removal of a connection. The connection that will be deleted is the one currently displayed on the screen. Pressing D will confirm before actually deleting the connection. Answer accordingly. Searching for a Connection: Finding the connection to edit or delete can take some time on a large board. This function allows a search for connections by designation. When prompted, enter the designation sought. PCTRACE will change the case to upper for you. PCTRACE then will search from the current connection to the end. It looks at both the source and destination designations for a match. If it finds the search string the program will display that connection's information. If it doesn't exist, nothing changes. Incrementing and Decrementing the displayed Connection: Using + and - will change the displayed connection. + increments and - decrements. The display is circular in nature, therefore typing + at the last connection moves it to the first connection and pressing - at the first will move it to the last connection. Exiting the Entry/Editing Environment: Use the N key to end these functions and return to the board definition menu. 3. Ground Plane: This function is used to set up a ground plane. The program will display a picture of the board. It will prompt for the width of the ground plane on all four sides on both the component side and solder side of the board. Each digit entered corresponds to .05 actual inches. The ground plane may be changed at any time. ESC will also back out of the first prompt only (top-solder side). *** Please note that this function erases any work done in the interactive router (discussed later). 4. Define Board Size: This function is the first function used. It defines the dimensions of the board. The maximum board size supported by PCTRACE is 8" X 10". When prompted for numbers, the PC-Trace Users Manual 14 numbers are entered as multiples of 5. Each number represents 0.05" of actual size. So an entry of 100 would correspond to 5". Board sizes can be changed at any time during the design process by calling the routine again. If the board is made smaller, the chips that were outside the new border will have to be replaced. ESC will back up to the previous prompt, or jump out of the routine leaving the board size unchanged. 5. Spider Web: This function is useful for checking to see if a chip would be more logically placed somewhere else. By using the + and - keys, various chips and their connections can be displayed. As each chip is selected, it, as well as all traces connected to it are highlighted in red. Once a chip is highlighted, selecting M will allow movement of the chip. After pressing M, the arrow keys become active and the chip, as well as all its connections will be rubber banded around the board. Pressing RETURN will place the chip at the current location, or press ESC to not place the chip and put it back at its original location. The ESC or E key will exit from this function. *** Please note, if chips are moved, the work done by the interactive router is erased. Interactive Router This board editing system allows the designer to interactively design a board. It can be very useful for finding possible routes that the autorouter was unable to find. Upon entry to this section, the program generates the borders and places the pads of all the chips. If a large number of components has been placed on the board, it could take a few moments. It will also ask the user to place all the chips that have not been placed yet. If you intend to route the entire board this way, place your chips and then leave them. Moving them around after placing the chip will distort the board. PCTRACE has no way of connecting traces up to a chips new location. The screen will show all the chips with their designations centered amid each component pin unless DEFGEN is used to lock the location of the designation. This system has many keys that are active while in this environment. An explanation of each follows. S - switch sides: This function changes the side of the board displayed. When S is pressed, the other side of the board becomes visible. The program supports only 2 sides, solder and component. PC-Trace Users Manual 15 K - Silkscreen toggle: Pressing this key toggles the silkscreen display on and off while in the interactive router. It defaults to ON upon entry to the interactive router. C - move a component: Pressing this key will give the user the option of moving a component within the interactive router. After pressing C, the bottom of the screen will show a brief listing of a component. The name and designation are listed. + will move to the next component, and - to the previous one. ESC will exit the component movement function. Pressing M will erase the displayed component and redraw the screen. At this point, move the cursor to the upper left corner of the area where the component will be placed and press G to place it. It is important to understand that the cursor represents the absolute upper left corner of the part including any silkscreen extensions. G - grab location: The key is only active at certain times. The F1, F2, F4, F5, F6, F7, and F10 function all use this key. The key is normally used to mark a location on the board or a piece of a trace. B - Turn on background: This key is used to turn on and off the background layer. If editing the solder side, a lightened view of the component side can be turned on. On a color monitor, it will appear dotted and red. Black and white monitors will show dotted graphics only. Pressing B again turns this mode off. E or ESC - end: Pressing E or ESC will exit from the interactive router. Cursor Keys: The cursor keys move the solid block around on the board. Each time an arrow key is pressed, the cursor will move 1 space. Relative coordinates are displayed at the bottom of the screen. Using Shift-Arrow moves the cursor 10 spaces. If the edge of the screen is encountered, but not the edge of the board, the screen will shift the board over. Function Keys: The function keys numbered F1-F10 do the majority of the work in PCTRACE. They allow placement of vias, running traces, deleting traces, resizing traces, and deleting vias. PC-Trace Users Manual 16 F1 - Set Source: By pressing F1, the bottom of the screen will say to position the cursor on the pad that will be designated as the source and then press G to grab it. The bottom status line will display exactly what chip and pin number have been selected. F2 - Set Destination: This function works exactly as the F1 function but selects the destination pin. F3 - Run Trace: Once a source and destination have been defined, pressing F3 will attempt to connect the two pins with a trace 0.01 inches wide. If it is successful, the screen will be redrawn and the trace will appear. If it cannot complete the route, a message will be displayed at the bottom of the screen. At this point try placing a via and routing from the source to it on one side and from the via to the destination on the other. F4 - Delete Trace: This function will delete any part of any trace on the board. Pressing F4 enters the delete selection mode. After pressing F4 the screen will say to use G to grab the parts to be deleted. As the user presses G on valid traces, the pieces will be highlighted. Changing screens by moving the cursor off the screen will not lose the already selected traces. Once all the pieces to delete have been selected, press F4 again and the program will prompt to confirm deleting of the selected traces. Answer Y to finish the delete operation. F5 - Add Via: This function key will add a via at the location of the cursor when G is pressed. It will be V and then the next available number. Use these for multilevel routes or just extra pads needed. A via cannot be placed adjacent to an existing pad. One can be placed diagonally from a pad . A via also may not be placed in the middle of a trace. All vias are deleted by the autorouter when it is invoked. F6 - Del Via: This function deletes the via at the cursor location when G is pressed if a via exists there. PC-Trace Users Manual 17 F7 - Resize trace: This function will resize a trace to any valid trace size. Select F7 and use G to select the traces to resize. Once the traces to resize have been selected press F7 and the program will ask for confirmation of the resize. Answer Y to resize. The program will prompt for the trace resize value. 1 corresponds to 0.01 up to 7 which corresponds to 0.07 inches. Be careful not to overlap other traces or pads with this function. F8 - Check Route: This function will check to see if a selected pair of pads can be connected. It will report back whether the route can be completed, the route exists already, or if no route can be found. This is useful for doing multi-layer routes using vias. Checking for an available route before laying the actual trace will save a number of deletes if later the path is blocked. F9 - Manual Route: This function allows the user to manually route traces. Place the cursor on the starting pad or trace and press F9. A prompt will appear at the bottom of the screen asking for the trace width. Enter the number that corresponds to the desired size and press return. Now use the cursor control keys to route the trace. Every time the cursor moves, the trace is lengthened. When done, either stop in an open space and press F9 or stop on a trace or pad and press F9, the correct connecting piece will be added to make the connection. Please note that moving over an existing trace will cause PCTRACE to cut that trace in favor of the new path. This works well for putting short jumpers on the board. This is very useful for routing traces that would normally block other routes if they were not placed this way. With the interactive router any size trace can be placed anywhere. It is possible to over-ride the autorouter and run a 0.01 inch trace between two 0.07 pads. If the board-making process used is accurate to 0.01 many low power traces can be completed this way. The manual router is also used in many advanced "tricks" for making specialized boards. F10 - Write Text: Pressing F10 allows additional text to be added to the silkscreen layer. After pressing F10, the program will ask the user to move the cursor to the starting position for the text and press G. After pressing G, the software will prompt for the text string. It will accept up to 20 characters. When done entering text, press return. The PC-Trace Users Manual 18 next prompt is for double sized text. Answer "yes" and the text will appear double sized. The board will then be redrawn with the text added in. The only thing to be aware of is that normal silkscreen text takes precedence over user added text. Using a mouse in the interactive router: The mouse allows a faster method to do all the functions mentioned previously except for the manual router. The mouse must be installed before running the PCTRACE program. When entering the interactive program four arrows will appear in the lower right corner of the screen. By using the mouse, putting the cursor on one of these arrows, and pressing the left button, the screen will be moved by half in that direction. The same thing was accomplished by moving the cursor off the board using the arrow keys. Pressing the right button will pop up a menu along the bottom of the screen. The menu corresponds to function keys F1- F8, and F10. The exit command at the far right, exits the menu. By placing the cursor anywhere on the command desired, execution of that command is done by pressing the left button. If the command selected is F1, F2, F4, F5, F6, F7, or F10, the program will be using the "Grab" method. The left button works the same as the G key in these cases. Use it to highlight sections and locations on the board to work with. When using the delete and resizing functions (F4 and F7) the user must press and release the left button for each piece of trace. Autorouting Selecting this from the menu will enable the user to connect all or most of the connections desired. The program will first draw borders, place pads, and set up the ground planes. If a component has not been placed, the program will ask the user to place it. The program requires all chips to be placed before it can route. There are four routing strategies that can be employed. Select each strategy by pressing Y or N as the cursor moves to each option. If Y is selected for single or double via routing a prompt will also appear for the maximum number of tries for each. Just enter a number. Bigger numbers are better for bigger boards, smaller numbers for small boards. The PCTRACE system is totally re-entrant. The first question asked is if the user wishes to clear all traces. Answering "yes" clears anything currently on the board. "No" would keep the screen as it was. ESC can be pressed during any routing strategy to exit that routine and the autorouter. The program will then show the list of all unconnected routes still existing. If the router has not completed one run-through the connection list, traces may have been completed by the earlier route and still be reported as unconnected. A design check can PC-Trace Users Manual 19 be done to see which routes in the connection list have not been connected, either by hand or by the autorouter, by running the autorouter and not erasing the current traces. This is because the autorouter will not reroute a connection that has already been completed. Just select the double or single sided route system. It will report any routes that are incomplete. Any route that was completed before will be marked as complete and not reported. The program will report whatever routes weren't done and the ones it couldn't complete. Single Sided Route: This function will attempt to place all the routes on the solder side of the board. It is the least efficient strategy but is great for small projects where ease of making the board itself is a priority. This function cannot be used in conjunction with the next three strategies. Double Sided Route: This function will do its routing on two sides of the board. It has a higher completion percentage than the single sided strategy. Single Via Route: This function requires that the double sided strategy be selected first. This function is used after the double sided strategy to try to complete any uncompleted routes. It places a via and tries to do the single route with a trace on each side of the board. A number such as 50 is good for the maximum number of tries prompt. Double Via Route: This function also requires that double sided routing be selected to work. It uses two vias to attempt to complete the route. A good maximum number of tries is 30 or so. This function can take a great deal of time so be patient. Board Statistics This function displays 5 statistics. Equivalent Integrated Circuit Count: This function is the total number of pins divided by 16. Board Density: This is the amount of space total that each chip has to occupy. It is calculated by taking the area of the board and dividing by the Equivalent IC count. PC-Trace Users Manual 20 Total Trace Length: The function gives the total length of all the traces on the board. The smaller the number, the better the design. Board size: The board dimensions in inches. File name: This is the file name currently in memory. PC-Trace Users Manual 21 Printer Menu 1. Print Components: This function will generate a list of all the components. It can be sorted by name or designation. 2. Print Connections: This function will generate a list of all the connections in memory. It can be sorted by the source or destination designation. Export Menu The export menu allows for files to be created that various other cad software and board producers use. After selecting the Export menu from the main menu, four export choices will be seen. 1. Write Autocad Script file: This function will write a file that can in turn be read into and edited with Autocad. The process is one way, no way is provided to read autocad files back into PCTRACE. Call this function from the Export menu and give a name when prompted. Specify no path or file extension. The extension .SCR will be added to the file. Once the program is done writing the file, Autocad may be started. Use the command "SCRIPT" from the "Command:" prompt. Autocad will ask for the script file name. Specify the same name (with path if needed) as the one created in PCTRACE and Autocad will read in the file. Autocad will display three layers: solder, component, and silkscreen. Each may be edited and saved as Autocad drawing files. Doing this greatly increases the number of printers that can be used for output as Autocad supports a large number of printers. 2. Write a DXF file: The DXF file is used by many cad packages to incorporate data into their systems. Autocad is one prime example. The DXF file includes all three layers in its output (Solder, Component, and Silkscreen). The command will prompt for a file name. Enter the filename with no extension. The extension .DXF will be added. After the filename has been entered, the DXF file output will be created. Autocad will load this file using the command "DXFIN" from the Autocad "Command:" prompt. Wordperfect will also read a DXF file and convert it to its own graphics format (WPG files). PC-Trace Users Manual 22 3. Write a Gerber file: A Gerber file is the standard file type that is used by professional board manufacturers. The PC-Trace software will generate this file format and is accurate to 3 decimal places. Upon selection of this option, the user is prompted to enter aperture names to be used. The aperture is used to describe an entity on the board. If the photo plotter that the board maker is using requires that a pad 0.05 inches in diameter be specified as D23, then the 0.05 inch pad aperture name must be changed to reflect this. The software will ask if the aperture list is OK. If it is, press Y for yes and the program will continue. If N for no is pressed, each aperture must be re-entered as the cursor goes down the column. ESC will bypass a selection without erasing. Retyping will change the selection and return will erase the selection which would make it necessary to re-edit the aperture list. Once the list is determined to be correct, the program prompts for the board side to be plotted to the file. Press the number that corresponds to the desired selection. Last of all the program will ask for an output filename. Enter the filename with no extension. Upon pressing the return key, the program will generate the Gerber file. Two files will be created. The first file will be the filename plus the extension .GER for the actual Gerber file. The second file is the filename plus the extension .AP for the aperture list. Both of these files should be sent to the manufacturer. A file must be generated for each board side that is desired to be manufactured. Only one aperture file need be sent. 4. Write a CNC Drill file: A CNC drill file contains the information for a Computer Numerically Controlled drill press to drill the holes for the pins of the components to be placed though. The software will prompt for the drill bit (tool number) size that should be used for each different sized pad. The entry system works the same as that of the Gerber aperture definition screen. The user will next be prompted for the output file name. It should be entered without an extension. After pressing return at the end of the filename the computer will create the filename with the extension .NC. The file contains the X,Y coordinates of all the pads. Exiting the Program Selecting 8 from the main menu will exit from PCTRACE back to DOS. If there is data in memory the program will ask if you wish to save it. Answering "Yes" will prompt for a file name. PC-Trace Users Manual 23 Enter the file name as was done in the save data function in the Input/Output menu. ESC will abort the save, but it will not return the user to the program. Answering "No" to the save query will cause the program to go immediately to DOS. PC-Trace Users Manual 24 Brief Tutorial The following is intended as a method of getting up and running with the program. It will give a general idea of how the program works. 1. Begin by running PCTRACE. This information can be found back in the section on setting up PCTRACE for your machine. 2. Once at the main menu, press 3 for define/edit board, and then select 4 for define board dimensions. For our purposes we will use a board size of 80 x 80, which translates into a 4 inch square board. 3. Select function 1 to enter new components. You will see that no data has been entered yet. Press A to enter data. We will put three chips on the board and two resistors. Answer each prompt below with the following data. When asked to place each chip answer Y and place the chip with the cursor keys. After you have entered the last item, answer N to the "Enter another component?" prompt. Name: 8051 uP Designation: IC1 Definition file: DIP40V6 Placement: Left side Pad Size: 0.05 Name: 74ls373 Designation: IC2 Definition file: DIP20V3 Placement: Upper right Pad Size: 0.05 Name: 2716 Designation: IC3 Definition file: DIP24V6 Placement: Lower right Pad Size: 0.05 Name: 100k resistor Designation: R1 Definition file: 2PAD50V Placement: Upper middle Pad Size: 0.06 Name: 10k resistor Designation: R2 Definition file: 2PAD50V Placement: Lower middle Pad Size: 0.07 N exits to the board definition menu. 4. Next, enter the list of connection between chips. Select 2 from the menu to enter the connection entry section. Enter the following connections. All traces should be 0.02 inches wide. Answer N to each prompt of "Is this a priority connection?". When the last connection has been entered answer N to the "Enter another connection prompt?". Source Device Pin Destination Device Pin PC-Trace Users Manual 25 IC1 2 IC3 2 IC1 3 IC2 16 IC3 22 IC2 6 R1 1 IC2 4 R2 1 IC1 8 R2 2 IC3 6 R1 2 IC1 31 IC2 8 IC3 17 IC1 21 IC1 15 IC2 8 IC3 8 IC2 9 IC3 9 IC2 10 IC3 10 IC1 14 IC2 9 N returns to the menu. 5. Ok, let's autoroute the board. Go back to the main menu and select 4 to autoroute the board. When prompted to use single sided routing or not, answer Y. Now hit the ESC key and watch the machine route. When it is done is will display the list of uncompleted connections to the printer or screen. Select whichever you wish. We will now be dropped back to the main menu. We can take a look at what we have done by selecting number 5 from the menu. Cursor around and see a representation of the board on the screen. Hit ESC when done. Now let's re-route the board using double sided techniques. This time say N to single sided and Y to double sided and then hit ESC. The machine will route double sided and again give a list of incomplete connections if any exist. Select printer or screen for this list. Let's take a look at the board again. This time we may also want to use the S key to change sides of the board that we are viewing. When you are done hit ESC. 6. From the main menu, hit 6 for statistics. Displayed are five statistics that tell you how good your design is. Hit space when you are done with this. 7. Last of all we'll print out our design. Follow instructions in the section on the RPRINT Subprogram to do this. PC-Trace Users Manual 26 RPRINT.EXE Subprogram Execute this program by typing RPRINT from the dos prompt. Upon entry into this program the user will be prompted for a printer type. Enter the corresponding number. The second prompt is for the board name. Type the name with no extension. The main control panel will now explode onto the screen. A math coprocessor is particularly useful in this program. 1. File name: Selecting 1 will allow changing of the file to be printed. Enter the filename with no extension. 2. Board side: This selects the board side to print. Selecting this number will toggle between three possible sides to print (Solder, Component, and Silkscreen). Single sided boards are done on the solder side. 3. Mirroring: This selection toggles between mirroring and not mirroring the board. 4. Negative: This function will allow the user to select between printing a negative or a positive of the actual board. 5. Actual size: Laser printers and 24 pin dot matrix printers can output the images at actual size. If the selected printer lacks the resolution to achieve acceptable results, this menu choice will not exist. Selection of this choice allows toggling between actual size and double sized printing. 6. Pin1 square: Toggling this to the on position will print the number one pin of all components as a square. This is useful for identifying the number one pin when placing the components on the finished circuit board. 7. Output file: After selecting this menu choice, the user is prompted for an output file name. Enter the filename without an extension. The printout of the file will now be sent to the file that was designated. The file will be given the extension .PRT. Be careful if printing multiple files not to overwrite a previous printing. 8. Print Board: This selection starts the printing of the board. 9. Exit program: This selection exits the RPRINT program back to DOS. Plotter Notes: In using RPRINT with plotters, no provision is made to print to a serial port. With DOS 3.3 and later, the MODE command can be used to redirect printer output to the serial port. Two PC-Trace Users Manual 27 commands are needed. MODE ComX:9600,N,8,1,p (press return) X is the com number MODE LPT1:=ComX: (press return) MODE LPT1: (press return) will return to normal operation PC-Trace Users Manual 28 DEFGEN Subprogram The program needs to know the exact pin layout of any component placed on the board. This function allows creation of these definitions. The largest difference between this version and previous versions of PCTRACE is that surface mount support can be acheived more easily. When a device is defined, all pins of the surface mount part must be terminated at a through-holed pad. That is the same as before. With version 5.0, pads and traces can be defined within the definition file allowing the user to draw small traces with flat pads to serve as locations to mount a surface mount part. A silkscreen outline can also be drawn with the manual router in "SILKSCREEN" mode. The program is started by typing "DEFGEN" from the dos prompt in the PCTRACE subdirectory. ***Note: Most chip dimensions are available in data books such as RCA cross reference manuals. Radio Shack also puts device dimensions on the back of their packages. When running DEFGEN to create new chip layout patterns many keys are active. A summary of each key follows: S - switch sides: This function changes the side of the board displayed. When S is entered from the keyboard, the other side of the board will be displayed. The program supports only 2 sides, solder and component. K - Silkscreen toggle: Pressing this key toggles the drawing on the silkscreen layer as opposed to the solder or component layers. When K is pressed a green "SILKSCREEN" appears at the bottom of the screen. The only commands that are available at this point are the F9, manual router, which is used to draw the part outline, F10 which allows placing text in addition to the component designation, F1 which is Load, F2 which is Save, and F3 which is erase. G - grab location: The key is only active at certain times. The F4, F5, F7 and F10 functions all use this key. B - Turn on background: This key is used to turn on and off the background layer. If the user is editing the solder side, this key will show a PC-Trace Users Manual 29 lightened view of the component side. On a color monitor, it will appear dotted and red. Black and white monitors will show dotted graphics only. Pressing B again turns this mode off. E or ESC - end: Pressing E or ESC will exit from the DEFGEN program. The exit is immediate and should be used carefully. Cursor Keys: The cursor keys move the solid block around on the board. Each time the arrow key is pressed, the cursor will move 1 space. Relative coordinates are displayed at the bottom of the screen. Using Shift-Arrow moves the cursor 10 spaces. If the cursor comes to the edge of the screen, but not the edge of the board, the screen will shift the board over. Function Keys: The function keys numbered F1-F10 do the majority of the work in DEFGEN. They allow the user to place vias, run traces, delete traces, resize traces, add pads, and draw component outlines. F1 - Load Definition: By pressing F1, the bottom of the screen will prompt for an input definition file name. Enter the filename with no extension. If the file is found it will be displayed on the screen for editing. Please feel free to use the provided definition files in creating others. F2 - Save Definition: This function will prompt for a save filename for the definition. Enter the save filename with no extension. The program will notify the user if the file already exists and check to make sure that it is alright to rewrite the file. Once the file has been written with this command, DEFGEN can be exited and the definition used in PCTRACE. F3 - Erase: This command has four options. Option 1 will erase the component layer of everything except the pads. The second option deletes everything but the pads off the solder layer. The third layer will remove everything off the silkscreen layer except for the placement of the designation text. Option 4 deletes everything, including the pads. Option 5 exits without deleting anything. PC-Trace Users Manual 30 F4 - Delete Trace: This function will delete any part of any trace that exists in the definition. Pressing F4 enters the delete selection mode. After pressing F4 the screen will say to use G to grab the parts to be deleted. As G is pressed on valid traces, the pieces will be highlighted. The user can change screens by moving the cursor off the screen without losing the already selected traces. Once all the traces to delete have been selected, press F4 again and the program will prompt to make sure you wish to delete the selected traces. Answer Y to finish the delete operation. F5 - Add New Pad: This function key will add a pad at the location of the cursor when G is pressed. All components must have pad definitions. The router is unable to route to a trace that cannot be specified by an attached pad. The pads are placed in sequence so be sure to place them in the package numbering order. F6 - Delete Last Pad: This function deletes the last placed pad from the screen. It requires that the definition be regenerated so the screen will be redrawn. F7 - Resize trace: This function will resize a trace to any valid trace size. Select F7 and then use G to select the traces to resize. Once you have selected the traces to resize, press F7 and you will be asked if you really wish to resize the traces, answer Y if you do. Next the program will prompt for the trace size. 1 corresponds to 0.01 up to 7 which corresponds to 0.07 inches. Be careful not to overlap other traces or pads with this function. F8 - Coordinates for Designation: This function will anchor the location of the part designation. Normally the designation moves to the centroid of the area defined by the pads. For most applications, like DIPs, this is acceptable. Some parts, such as transistors, benefit from having the designation text placed above or below the pads. Selecting this option will prompt for a location for the center of the designation text. Move to that location and press G. The next prompt asks if the user desires double sized text. If "yes" is entered, the designation will be drawn 0.1 inches high on the silkscreen layer. "No" will draw text 0.05 inches high. PC-Trace Users Manual 31 F9 - Manual Route: This function allows the user to manually route traces. Place the cursor on the starting pad, trace, or open area and press F9. Now use the cursor control keys to route the trace. Every time the cursor moves, the trace is lengthened. When done, press F9. If the end is on another trace, pressing F9 will add the proper connecting point. If the green SILKSCREEN indicator is on, the trace will be routed in green. This should be used to draw the outline of the part. This outline will be displayed in the interactive router and when printing the silkscreen. F10 - Write Text: Pressing F10 allows the addition of text to the silkscreen layer. After pressing F10, you will be asked to move the cursor to the starting position for the text and press G. After pressing G, the software will prompt for the text string. It will accept up to 20 characters. When done entering text, press return. The next prompt is for double sized text. Answer "yes" and the text will appear double sized. The board will then be redrawn with the text added in. Using a mouse in the DEFGEN program: The mouse allows usage of all the functions mentioned previously except for the manual router. The mouse driver must be installed before running the DEFGEN program. When entering the interactive program, four arrows will appear in the lower right corner of the screen. By using the mouse, putting the cursor on one of these arrows, and pressing the left button the screen will be moved by half in that direction. The same thing was accomplished by moving the cursor off the board using the arrow keys. Pressing the right mouse button will pop up a menu along the bottom of the screen. The menu corresponds to function keys F1- F8, and F10. The exit command at the far right, exits the menu. By placing the cursor anywhere on the command desired, that command can be executed by pressing the left button. If the command selected is F4, F5, F7, F8, or F10, the "Grab" method will be in use. The left button works the same as the G key in these cases. Use it to highlight sections and locations on the board to work with. When using the delete and resizing functions (F4 and F7) the user must press and release the left button for each piece of trace. PC-Trace Users Manual 32 Keyboard Summaries for PCTRACE Chip Placement Screen: ESC - Option to Abandon Placement RET - Place chip at current location Cursor Keys - Moves chip one space for each depression Shift Cursor Key - Moves chip 10 spaces for each depression Spider Web System: M* - Set system to move highlighted chip Cursor keys - Move chip one space on board RET - Place chip at current location ESC - Abandon placement +,-* - Increment and Decrement through chips E* - Exit Web System * - Denotes that this selection is displayed on screen at all times. Interactive Router: S - Display other side of board G - Grab a piece of trace at cursor E,ESC - Exit interactive router B - Turns on and off background C - Allows movement of devices K - Turns silkscreen layer on and off F1 - Select source pad F2 - Select destination pad F3 - Attempt to connect source and destination F4 - Delete traces F5 - Place via at cursor location F6 - Delete via at cursor location F7 - Resize selected trace F8 - See if route is possible between source and destination pads F9 - Enters and exits the manual router F10 - Puts user text on the silkscreen layer PC-Trace Users Manual 33 SCAD Schematic Capture Version 1.0 Users Manual June 21, 1992 by Douglas E. Ehlers Copyright (C) 1991,1992 Introduction Schematic CAD is a program for drawing electrical schematics. While this drawing is being made, the software keeps track of all components and connections between them. It is then possible to create an export file (.NLT) that PC-Trace can load and create a board from. This allows the designer a complete cycle for production of a circuit board. From conceptual design to computer controlled manufacture of the board, this system has it all. Menu Usage: The menu system in SCAD requires the use of a mouse for complete use of the system. Some functions can be accomplished with the use of the keyboard only. Using a mouse, move the cursor to the area of the desired menu selection. By pressing the left mouse button, a pull down menu will appear. Move the mouse down the menu until the desired choice is highlighted and release the button. The menu choice will be executed. Another way to make menu choices is to open the menu by pressing the ALT key and the highlighted menu area key. For example ALT-F will open the Files Menu. The cursor keys can be used to move the highlight bar up and down the menu. Pressing return will select the menu choice. Once the menu appears, pressing the first letter of the desired choice will move the highlight bar to that choice. Some menus have small arrows that point to the right. By moving the mouse across that arrow a submenu will appear. That menu responds the same way as the rest of the menus. Many functions use this concept including Print, Draw, Delete, and Move. File Menu: New Diagram: The New Diagram function from the FILES menu will clear the drawing space that SCAD uses to store files. A dialogue box is used to confirm this selection. Load Diagram: The Load Diagram file will load a schematic that was saved previously. The program will prompt for the file name. Enter the name without the extension (.SCH). The program will add the extension. If the program cannot find the file it will report it and give the user another chance to enter the filename or to exit back to the drawing area. Save Diagram: The Save Diagram function saves whatever is in the memory of the system at a given point. When prompted for a save name, enter the name with no extension. SCAD will add the extension (.SCH). If the program can't find the entered file name, it will save the information from the given mode. If the program finds that the save filename exists, it will prompt to see if the old file should be overwritten, or a new file name should be specified. PC-Trace Users Manual 35 Export DXF: The Export DXF function is used for creating a file format that can be read by many popular CAD programs and word-processing packages. The DXF format used is compatible back to Autocad Version 2.6. The program will prompt for a save name. Give the file name with no extension. The program will add it (.DXF) automatically. If the filename already exists on the disk, the program will prompt as to whether or not to overwrite the file. Answering yes will overwrite the old filename, and answering no will cause SCAD to prompt for a new file name. Export PC-Trace: The function is used to create a netlist that PCTRACE can load. It contains a list of all components and connections that have been entered while using the SCAD software. All that will be required on the PCTRACE side is to place the components and start the autorouter. The program prompts for the export filename. Enter the filename with no extension, the program will add it automatically. If the program finds that the entered filename exists, the program will allow the option of overwriting the file or re- entering a new filename. Print Total/Window: Print has two options, one, the option called Total, that will find the extents of the drawing and scale it to fit on a page. The second, or Window, essentially prints what is currently being viewed on the screen. Once the program is told to print, it will create a print file, save the current drawing and chain to the sprint.exe program. The first prompt in this program is for the printer type. The user should select their printer or one that their printer emulates. The sprint menu can print to a file and that is toggled with option 1. When prompted for a print filename, enter the filename with no extension. The second option will allow printing in portrait or landscape mode. Option 3 actually prints the drawing, and option 4 exits sprint.exe and returns to SCAD. Show Drawing Info: This function will show basic drawing information including the current SNAP value, the current window size, the amount of free memory, and the currently loaded filename. Exit: The exit function exits whichever mode the program is currently running in. This function can also be activated by pressing ALT-X. If the user is currently operating in PC-Trace Users Manual 36 the Component Drawing area, it will exit the drawing pad. If the user is editing the main drawing, it will allow exit of the program. No option is given to the user to save the file once exiting the program is answered with an OKAY. Drawing Symbols: When Draw Component is selected from the Components menu, a box appears in the center of the screen. This is the drawing area for creation of components. A component in this case is defined to be the schematic symbol for any part that will be placed in the drawing. A small library of common symbols is included with the system for the user. Invariably, a symbol will be needed that is not included. That is the purpose of this editor. Once the box appears in the middle of the screen, the Files menu and the Entities menu come into play. Only certain functions may be used in each. The unusable functions will be grayed out and the user will be unable to use them. The Load, Save, New, and Exit functions in the Files menu work as described previously, except that they only apply to the current symbol being drawn. For example, if an AND gate is drawn in this area, saving it will only save the representation of the AND gate and not the overall drawing. The save routine itself is different at this point as well. It includes a short routine that asks the user to outline the symbol with a bounding box before the save takes place. Select the upper left and lower right of the drawing to save. The entire drawing will be shifted to call the upper left corner of the bounding box the origin for later use. The following overview tells how the various Entities commands work and what they do. Their usage here is essentially the same as their usage in the main drawing area. Draw-Line: This function is used to draw lines within the drawing window. At the bottom of the screen, SCAD will prompt the user as to what the program expects. The current coordinates are shown at the bottom right. Select the location of the starting point of the line and click the left or right button. Clicking the left button will anchor the start of the line at the current mouse location. Clicking the right button will anchor the start point at the current point, plus it will draw a connection dot at this point. The dot will not appear until the start and end points of the line have been specified. After clicking the left or right button, the program will prompt for the end point. Click either the right or left button. The buttons have the same effect as when picking the start point. ESC will exit or back up while drawing lines. To draw another line, select this function again. PC-Trace Users Manual 37 Draw-Arc: This function is used to draw an arc of some size. It can be used to draw 1/4 arcs from any start point to any end point and at any diameter. The first prompt is for the center point of the arc. Move the mouse to this location and click a button. The second prompt is for the radius of the arc. Move the pointer to the location that shows the desired radius. A floating line reminds the user as to the current length. The next point is for the start of the arc. Pick this point as before. The last prompt is for the arc ending point. Click on this point. The arc will be drawn from the start point, counter-clockwise, to the end point at the given radius. ESC will back up at any time to the previous prompt or will exit the function. To draw another arc, pick this function again. Draw-Circle: This function draws a circle at some center point and some radius. When prompted, pick the center point and click a mouse button. The second prompt is for the radius of the circle. Click on this point and the circle will be drawn on the screen. ESC will back up to the previous prompt or exit the function. To draw another circle, pick this function again. Draw-Text: This function is used place text on the screen. The first prompt is for the starting location of the text. This point is located at the top, left corner of the text string. Select this point by moving the mouse to the desired location and click a button. The second prompt is for the scale of the text. This number is the size of the text. A value of 0.25 will create a string with characters every 0.25 units. The third prompt is for horizontal versus vertical text. Answering yes will draw the text horizontal and no will draw the string vertically. The letters are always upright, they are not rotated for vertical text. The last prompt is for the text string itself. This string will be displayed on the drawing itself. When entering text pressing return at the end of the string will draw the normal text. If the up-arrow cursor key is pressed instead of return, the text will be drawn with a line over it. This is useful for digital systems when a signal is active low. Delete-Line: This function is used to delete lines from the current drawing area. A line will be highlighted in red and made dotted. If this line is to be deleted press Y for yes. Another line will be highlighted. Pressing Y for yes will delete that line as well. Other options for keys are to press N for no. Saying no will move to the next line, or if no other lines exist, will exit the function. Pressing B for back will back up to the previous line. This was added in the case of many lines on the screen and user inadvertently bypassed the desired line. ESC will exit at any time, leaving the current line shown on the screen in PC-Trace Users Manual 38 the correct color. Delete-Circle/arc: This function is used to delete circles/arcs from the current drawing area. A circle/arc will be highlighted in red and made dotted. If this circle/arc is to be deleted press Y for yes. Another circle/arc will be highlighted. Pressing Y for yes will delete that circle/arc as well. Other options for keys are to press N for no. Saying no will move to the next circle/arc, or if no other circles/arcs exist, will exit the function. Pressing B for back will back up to the previous circle/arc. This was added in the case of many circles/arcs on the screen and the user inadvertently bypassed the desired circle/arc. ESC will exit at any time, leaving the current circle/arc shown on the screen in the correct color. Delete-Text: This function is used to delete text from the current drawing area. A text string will be highlighted in red and made dotted. If this text is to be deleted press Y for yes. Another text string will be highlighted. Pressing Y for yes will delete that text as well. Other options for keys are to press N for no. Saying no will move to the next text string, or if no other text exists, will exit the function. Pressing B for back will back up to the previous text. This was added in the case of many text strings on the screen and the user inadvertently bypassed the desired text. ESC will exit at any time, leaving the current text shown on the screen in the correct color. Regenerate: Selecting this function will redraw the current screen. SCAD sometimes creates a little garbage on the screen when adding and deleting lines. This function will clean it up. Set Snap: The Snap function is used to set absolute units and endpoints for drawing operations. If the Snap function has already been turned on, selecting it again will prompt the user that it will now be turned off. If the Snap function is currently off, a text entry dialogue box will appear and the snap value will be given. Common values are 0.1 or 0.25. Any value between 0 and 1 can be entered and used. All subsequent usage of drawing commands will move endpoints of lines, arcs, circles and text to the grid points shown. Scale: The scale menu selection is used to change the size of the current symbol uniformly across its entire area. The value that is entered when the dialogue box opens is multiplied by the dimensions of all the entities in the symbol. For example, if the symbol was 1 unit long and a scale factor of 0.5 was entered, the final length of the PC-Trace Users Manual 39 symbol would be 0.5 units. Pressing ESC will exit with no changes. Shift Space: The shift space routine will move the entire drawing some offset specified by entering a starting and ending point of a line. If a line from 1,1 to 2,2 is drawn, the entire drawing will be shifted 1 unit right and 1 unit down. To draw the line, when prompted, click on the starting point and ending point. After the second click the drawing will be shifted. ESC will exit backwards or out of this routine. Extend/Trim: This function allows a line to be extended/trimmed to/by another line, or a circle to be extended/trimmed to/by a line, or a line to be extended/trimmed to/by a circle. This function is useful for designing symbols whose intersection of points aren't on convenient dimensions. A good example of this is the OR gate. The function works by first prompting to see if the object that will be used to extend or trim with is a line or a circle/arc. Press L for line or C for circle. The software will now use the same procedure as is used for deleting objects to select the extend/trim edge. Once it is selected it will be colored in Magenta. The second prompt is for the object to extend or trim. This is the object that will have its dimensions modified. If the trim object was a line, the program will give the option of a line or a circle/arc to modify. If the trim object was a circle/arc the program will automatically select the second object to be a line. The program will highlight each object in succession until the user picks the desired object to modify. The next prompt is for the user to select a point, with the mouse, near the end point of the object to modify. One more prompt exists if a circle is one of the affected entities. This prompt is to pick a point near the projected intersection. At the end of the prompts the entity will be modified as per the user instructions. A regeneration may be required as well to clean up the screen. The tools that have been described above should be adequate for drawing most objects. Sometimes some creative usage of the Snap function and Extend/Trim is required. Placing Components/Symbols: This function is used to place symbols on the main drawing area. This area is separate from the previous area and has no limits in size for practical use. The only limiting factor is the amount of available memory. When a set of graphic symbols are put together to make a meaningful electrical symbol, they are grouped as an object. They can only be edited by choosing from the Components menu the PC-Trace Users Manual 40 Place Component command. The Move, Delete, and other commands in the Entities section only affect the objects that have been drawn not using this menu selection. When Place Components is selected with the mouse or keyboard a window will appear in the center of the screen. If no components have been entered, only two choices will appear: N to exit or A to enter new symbols. ESC will also exit the function. A-Enter new Components: This function will clear the window and prompt for the name of the symbol that will be placed. This name will not appear on the symbol itself and is used only to tell the designer exactly what the part is. The second prompt if for the part designation. This is later placed on the name of the part and is used by PCTRACE to specify autorouter connections. This designation need not be unique as it must be in PCTRACE. The reason for this is that some parts, such as AND gates like the 74LS08 have more than one part in them. This allows the user to connect multiple parts under one name. No automatic provision is provided for specifying which part of the overall part is being connected to, other than the pin number. The program will notify the user if a duplicate designation is specified to verify that this is desired. The next prompt is a filename for the actual parts layout information. This is the same file as that used by PCTRACE to specify pad locations. The program will pop up a small window with lists of names that are available for use. Enter the name of the part without the extension and the program will display it on the screen in a small window. Information about the part appears on the bottom of the screen. If it is correct press Y for yes or click in the Yes box. If it is not correct, click on the No box or press N, the program will reprompt for the name. This entry is not significant for drawing the schematic itself, but is needed for export to PCTRACE. The next prompt is for the Pad size. Enter 1 for 0.05, 2 for 0.06, 3 for 0.07 and so forth. The last text prompt is for the name of the schematic symbol that will be drawn on the main drawing area. The program will open a window showing a list of valid diagram files. Enter the diagram file with no extension and it will be drawn to check for user approval. Answering Y will move to the main drawing area for placement, and N will go back and reprompt for the diagram file name. Once the diagram file has been selected the text window will disappear and two crosshairs will be shown on the screen. This is the size of the part that has been selected and is being placed. Moving the mouse to the desired location and pressing a mouse button will anchor the location of the part. The next PC-Trace Users Manual 41 prompt appears at the bottom of the screen and asks for the location of the text. The text that will be drawn is the designation name entered earlier. Remember that the point selected is the upper left corner of the first character in the string. The next prompt is for the text scale and is the actual size, in units, of the characters that will be drawn. The last prompt is for horizontal text. Answering Y for yes will draw the text in a horizontal line and N for no will draw the text vertically. At this point the user is prompted as to whether or not they want to enter another component. Click on the appropriate space. Answering Y will start the process again, and N will put the user on the last entered component and give other options as well as display the current data. At any point in the previous component entry routine, ESC will back the user up. From a Display of Component Data: Once a component has been entered various editing options can be used on it. Those options are discussed below: E - Edit Component: This will allow the user to change things such as the name, designation, pad size, actual part layout filename, location of the diagram, orientation of the diagram, and the location of the text that is associated with this component. The letters that do each of these are discussed below: A-Name: This will prompt for a new name, enter the new name or press ESC to leave it unchanged. B-Designation: This will prompt for a new designation name, enter the name or ESC to exit. C-Definition: This will prompt for a new component pad layout definition. Enter the new file or ESC to exit. D-Pad Size: This will open a window with three different pad sizes. Enter the desired value. E-Move Comp: This will allow the user to move the current symbol to a new location. The crosshairs will appear and mouse will move them. Click the button on the location for the new location. ESC will exit. F-Rotate: This function will rotate all elements associated with this component. The device can be rotated 90, 180, or 270 degrees counter-clockwise. It may require some movement of text to make everything look right. PC-Trace Users Manual 42 G-Move Text: This function allows the user to first select the text, using the previously mentioned method or moving forward, backward, and selecting. A box appears that is the outline of the text. Using the mouse, move the text to the desired location and click a mouse button. The new text location will now be at this point. H-Exit Edit: Selecting H, will exit the edit function. A-Enter new Components: This function allows entry of more components and is the same routine that was discussed at the beginning of this section. Delete: This function will allow deletion of the component that is currently on screen. The entire component can be deleted or just the text. Enter the number that is desired. An entry of 3 will exit with no deletions taking place. If the component is deleted, all associated connections will be deleted as well. Search: This will allow the user to search from the current location to the end of the list of components. Only the Designation can be searched on. Follow the prompts to do either. + - Next: Pressing the + key will display the next component on the screen. If at the end of the list, the first component is displayed. - - Previous: Pressing the - key will display the next component on the screen. If that the beginning of the list, the last component is displayed. Text Entry: This function allows text entry that can be placed on the main drawing area. This text will be linked in to the component that is currently displayed. This text entry should only be used for text that is associated with the component. It can only be modified from this component. More general text entry should be done from the Entities menu while running in the main drawing area. PC-Trace Users Manual 43 N to End Component Entry and Editing: N or ESC will move the user back to main drawing area. All work will be held in memory. Connection Entry: Only one choice exists from the Nconnections menu and that is to make connections between existing components. The input routine was created to minimize the amount of time spent typing and maximize the ease with which connections are drawn and recorded. When the selection is executed it automatically starts entry of a new connection. The first prompt is to pick a point inside the source component. The crosshair will show on the screen under mouse control. Place the crosshair in the "bounding box" of the source component and click a button. When prompted for the destination component do the same thing. This will tell the program the source and destination components. The next step is to tell the program the source pin number. Enter it at the bottom of the screen when prompted. The second step is to use the mouse to specify the starting point of the number just entered. The third step is to enter the scale of the pin number. The destination pin number is done exactly the same was as the source pin. The source and destination pin number that are entered during this process will be normal text. The source number will become part of the source component object and will not be editable from the main drawing area. It will be necessary to go into the Place Components section to edit or move the text. One reason for this is to move the pin numbers or change the letters to have an overline. The same is true for the destination number, it will be attached to the destination component. After both the source and destination have been entered, a dialogue box appears to show the user that source and destinations that have been chosen. If the information is incorrect click on the No box or press N, the connection entry will be restarted at the beginning. If yes is selected the line draw routine will started and the user can draw the connection with as many straight lines as desired. The e key for endpoint and right mouse buttons are active for finding endpoints and making connection dots. The lines drawn will be attached to the current connection object. Deleting this object will remove the lines that are associated with this connection. The only other difference between connections and components is that the lines drawn in a connection can be edited in the main drawing area. After the last line has been entered, pressing ESC will end the line drawing routine. After pressing ESC, the program prompts asks if the user wants to enter another connection or not. Answer yes to restart this procedure and create another connection. No will put the user at the connection editing facilities. PC-Trace Users Manual 44 Connection List Menus: Several options are available from this point. A list of commands is shown as the last line in the window. The edit command allows the user to change the source and destination names and pin numbers. Changing this information will not change the graphic data that was entered. To change the graphic representation of the number that are on the drawing will require finding the component that they are associated with. A)enter new will allow entry of other connections are described above. Delete will delete the listed connection and the lines that are associated with it. Search will prompt for a designation name and search from the current location to the end of all connections for a matching source or destination designation. '+' and '-' move to next or previous connection entry. These keys loop from start to end or end to start depending on the key. Line will allow the user to draw lines in addition to those that were drawn during the initial connection entry. These lines are drawn the same as during connection entry. ESC will exit the line drawing routine. N for end or ESC will exit this menu and return the user to the main drawing area. Drawing Entities: Draw-Line: This function is used to draw lines within the main drawing area. At the bottom of the screen, SCAD will prompt the user as to what the program expects. The current coordinates are shown at the bottom right. Select the location of the starting point of the line and click the left or right button. Clicking the left button will anchor the start of the line at the current mouse location. Clicking the right button will anchor the start point at the current point, plus it will draw a connection dot at this point. The dot will not appear until the start and end points of the line have been specified. After clicking the left or right button, the program will prompt for the end point. Click either the right or left button. The buttons have the same effect as when picking the start point. Another option for selecting the desired point is to press 'E' while the program is asking for the start or end point. Pressing 'E' at this time will draw a small box on the screen. Placing this box at or near the endpoint of another line will select the exact endpoint of that line or arc. The mouse buttons have the same effect. This function is active much of time when in the main drawing area and should PC-Trace Users Manual 45 be tested whenever it is needed. ESC will exit or back up while drawing lines. To draw another line, select a start and end point again. This function will continue this sequence until ESC is pressed to exit it. Draw-Arc: This function is used to draw an arc of some size. It can be used to draw any length arc from any start point to any end point and at any diameter. The first prompt is for the center point of the arc. Move the mouse to this location and click a button. The second prompt is for the radius of the arc. Move the pointer to the location that shows the desired radius. A floating line reminds the user as to the current length. The next point is for the start of the arc. Pick this point as before. The last prompt is for the arc ending point. Click on this point. The arc will be drawn from the angle of the start point, at the selected radius, counter-clockwise, to the end angle. ESC will back up at any time to the previous prompt or will exit the function. To draw another arc, pick this function again. Draw-Circle: This function draws a circle at some center point and some radius. When prompted, pick the center point and click a mouse button. The second prompt is for the radius of the circle. Click on this point and the circle will be drawn on the screen. ESC will back up to the previous prompt or exit the function. To draw another circle, pick this function again. Draw-Text: This function is used place text on the screen. The first prompt is for the scale of the text. This number is the size of the text. A value of 0.25 will create a string with characters every 0.25 units. The second prompt is for horizontal versus vertical text. Answering yes will draw the text horizontal and no will draw the string vertically. The letters are always upright, they are not rotated for vertical text. The third prompt is for the text string itself. This string will be displayed on the drawing itself. The last prompt is for the starting location of the text. This point is located at the top, left corner of the text string. Select this point by moving the mouse to the desired location and click a button. When entering text pressing return at the end of the string will draw the normal text. If the up-arrow cursor key is pressed instead of return, the text will be drawn with a line over it. This is useful for digital systems when a signal is active low. PC-Trace Users Manual 46 Move-Line: The move line is used to change the placement of an existing line. When this selection is made, the program will highlight lines in succession until the user responds with a Y for yes. At this point the user will be asked to select, with the mouse, a base point of movement. Click on that point. E is active to select the endpoint of the line, or any other, for movement. After the basepoint has been selected and the mouse button clicked, the entire line will move with the movement of the mouse. Position the line at the desired location and click a button to permanently place the line. E is active to select an endpoint. ESC will back up or exit the function. Move-Circle/Arc: The move circle/arc function is used to change the placement of an existing circle/arc. When this selection is made, the program will highlight circles and arcs in succession until the user responds with a Y for yes. At this point the user will be asked to select, with the mouse, a base point of movement. Click on that point. E is active to select the endpoint of the arc, or any other, for movement. After the basepoint has been selected and the mouse button clicked, the entire circle/arc will move with the movement of the mouse. Position the circle/arc at the desired position and click a button to permanently place the circle/arc. E is active to select an endpoint. ESC is active to back up or exit the function. Move-Text: The move text function is used to change the placement of an existing text string. When this selection is made, the program will highlight text strings in succession until the user responds with a Y for yes. At this point the user will be asked to select, with the mouse, a base point of movement. After the basepoint has been selected and the mouse button clicked, a box representing the text will move with the movement of the mouse. Position the text box at the desired position and click a button to permanently place the text. E is active to select an endpoint. ESC is active to back up or exit the function. Delete-Line: This function is used to delete lines from the main drawing area. A line will be highlighted in red and made dotted. If this line is to be deleted press Y for yes. Another line will be highlighted. Pressing Y for yes will delete that line as well. Other options for keys are to press N for no. Saying no will move to the next line, or if PC-Trace Users Manual 47 no other lines exist, will exit the function. Pressing B for back will back up to the previous line. This was added in the case of many lines on the screen and user inadvertently bypassed the desired line. ESC will exit at any time, leaving the current line shown on the screen in the correct color. Delete-Circle/arc: This function is used to delete circles/arcs from the current drawing area. A circle/arc will be highlighted in red and made dotted. If this circle/arc is to be deleted press Y for yes. Another circle/arc will be highlighted. Pressing Y for yes will delete that circle/arc as well. Other options for keys are to press N for no. Saying no will move to the next circle/arc, or if no other circles/arcs exist, will exit the function. Pressing B for back will back up to the previous circle/arc. This was added in the case of many circles/arcs on the screen and the user inadvertently bypassed the desired circle/arc. ESC will exit at any time, leaving the current circle/arc shown on the screen in the correct color. Delete-Text: This function is used to delete text from the current drawing area. A text string will be highlighted in red and made dotted. If this text is to be deleted press Y for yes. Another text string will be highlighted. Pressing Y for yes will delete that text as well. Other options for keys are to press N for no. Saying no will move to the next text string, or if no other text exists, will exit the function. Pressing B for back will back up to the previous text. This was added in the case of many text strings on the screen and the user inadvertently bypassed the desired text. ESC will exit at any time, leaving the current text shown on the screen in the correct color. Regenerate: Selecting this function will redraw the current screen. SCAD sometimes creates a little garbage on the screen when adding and deleting lines. This function will clean it up. Set Snap: The Snap function is used to set absolute units and endpoints for drawing operations. If the Snap function has already been turned on, selecting it again will prompt the user that it will now be turned off. If the Snap function is currently off, a text entry dialogue box will appear and the snap value will be given. Common values are 0.1 or PC-Trace Users Manual 48 0.25. Any value between 0 and 1 can be entered and used. All subsequent usage of drawing commands will move endpoints of lines, arcs, circles and text to the grid points shown. Zoom In: This function requires the use of the mouse to pick a bounding box for an area to zoom in on. Click the mouse on one corner of the area to zoom in on and click the mouse on the opposite corner. SCAD will show the boxed in region on screen as the full screen while maintaining the aspect ratio. Zoom Out: The Zoom out function prompts for a zoom out factor. Enter a value. A value of 2, for example, will double the area being viewed. A value of three will triple the area and so forth. Zoom Total: The Zoom Total will zoom out so that all of the drawing is shown on the screen. This function finds the overall size of the drawing and adjusts the viewing area accordingly. Shift Space: The shift space routine will move the entire drawing some offset specified by entering a starting and ending point of a line. If a line from 1,1 to 2,2 is drawn, the entire drawing will be shifted 1 unit right and 1 unit down. To draw the line, when prompted, click on the starting point and ending point. After the second click the drawing will be shifted. ESC will exit backwards or out of this routine. Extend/Trim: This function allows a line to be extended/trimmed to/by another line, or a circle to be extended/trimmed to/by a line, or a line to be extended/trimmed to/by a circle. This function is useful for designing symbols whose intersection of points aren't on convenient dimensions. A good example of this is the OR gate. The function works by first prompting to see if the object that will be used to extend or trim with is a line or a circle/arc. Press L for line or C for circle. The software will now use the same procedure as is used for deleting objects to select the extend/trim edge. Once it is selected it will be colored in Magenta. The second prompt is for the object to extend or trim. This is the object that will have its dimensions modified. If the trim object was line, the program will give the option of a line or a circle/arc to modify. If the PC-Trace Users Manual 49 trim object was a circle/arc the program will automatically select the second object to be a line. The program will highlight each object in succession until the user picks the desired object to modify. The next prompt is for the user to select a point, with the mouse, near the end point of the object to modify. One more prompt exists if a circle is one of the affected entities. This prompt is to pick a point near the projected intersection. At the end of the prompts the entity will be modified as per the user instructions. A regeneration may be required as well to clean up the screen. Keyboard Summaries for SCAD When Entering Text on the schematic: RETURN - enters the text normally Cursor Up Arrow - overlines the text When drawing points, lines, arcs, and text: E - gives user box to find endpoints R. Mouse Button - puts connection dot on point of line PC-Trace Users Manual 50 Conclusion: The PCTRACE circuit design system was written by Doug Ehlers for use by himself. This was done without ever having used another design package. The decisions made were chosen to be intuitive to the author. The program is under constant refinement, so the user should try and maintain contact with the author through one of the previously mentioned support methods. As always the author is interested in user input on the software. The program has evolved as it has through the input and support of its users. In the words of a famous gentleman (almost) "Thank you for your support." PC-Trace Users Manual Appendix A .NLT File Format The file created by the export function of SCAD and read by the import function of PC-TRACE can be used as a mechanism for importing netlists from other CAD software. It is currently not feasible for the author to offer this support. If conversions are written by users, they are encouraged to let the author know so that they can be shared by other users. The -> signifies a line in the file. The following is the file format: ->Number of Components in list Each component looks like: ->Name of component 15 characters ->Component Designation 5 characters ->Definition file name 12 characters ->Pincount & Padsize 2 Integers with 2 spaces between Pincount is an integer signifying the number of pins in the file. The Padsize is a 3 bit number in the 5th, 6th, and 7th bits of the number. 0 is 0.05, 1 (=32) is 0.06, and 2 (=64) is a 0.07 inch diameter pad. The lower five bits of Padsize should be zero. The bit 0 signifies if the component has been placed on the board yet. ->Number of Connections in list Each Connection looks like: ->Source Designation 5 characters ->Source Pin Number Integer ->Destination Designation 5 characters ->Destination Pin Number Integer