This file contains important information for PC Board Layout Tools 386+ version 2.22 that was not included in the printed documentation. Please read the first three entries before you install PCB 386+. ****************** !!! IMPORTANT !!! *********************** Please read these first two entries BEFORE installing PCB 386+ ****************************************************************** ------------------------------------------------------------------ Installing PCB 386+ while running 4DOS ------------------------------------------------------------------ Do not run the INSTALL program for PCB 386+ if you have 4DOS loaded as your current command processor. Be sure COMMAND.COM is the active command processor before you run the install program. This is specified in the "SHELL=" line in your CONFIG.SYS file. ------------------------------------------------------------------ Manually updating ORCADESP.DAT using MERGEDAT ------------------------------------------------------------------ INSTALL checks your system to see if the ESP design environment is installed. If ESP is present, then the ORCADESP.DAT files in your design directories are automatically updated. If problems occur during this part of the installation, ESP buttons that display on your PC Board Layout Tools screen will not match those shown in the PCB 386+ documentation. You will need to manually update the ORCADESP.DAT files using the MERGEDAT program. The INSTALL program places PCB386.MRG in the path you specify for the ORCADESP directory (C:\ORCADESP if your directory structure follows the default configuration). If you want all your ORCADESP.DAT files updated for PCB 386+, enter this command: MERGEDAT PCB386.MRG/A This creates the file ORCADESP.DAT in all your design directories. ******************************************************************* ------------------------------------------------------------------ Copying PCB 386+ configuration files to all design directories ------------------------------------------------------------------ After installing PCB 386+ you need to copy the PCB 386+ configuration files PCB.BCF and PCB.CFG from the TEMPLATE or TUTOR design directories to your other design directories. This must be done so PCB 386+ works with all of your design directories. If you used PCB II with other designs, the PCB II configuration files PCB.CFG and PCB.BCF are in the other design directories. You need to rename these configuration files before copying the PCB 386+ configuration files. ------------------------------------------------------------------ Entering numeric values in ESP configuration screens ------------------------------------------------------------------ Do not exceed three decimal places for any numeric value entered in ESP configuration screens. Unpredictable results may occur if values with more than three decimal places are entered. ------------------------------------------------------------------ Configuring module libraries ------------------------------------------------------------------ If you do not have any module libraries configured in the Configured Libraries list box of the Configure PC Board Layout screen, then all module libraries in the Available Libraries list box are searched. If a module library is configured in the Configured Libraries list box, then only the configured library is searched. ------------------------------------------------------------------ Specifying a path for the PCB 386+ template file ------------------------------------------------------------------ In the Miscellaneous Options section of the Configure PC Board Layout screen, you must enter the complete path and filename for the PCB 386+ template file, ORCADPCB._T_, if the file is located in a different directory than your startup design directory. If ORCADPCB._T_ is located in your startup design directory, you can enter just the filename. PCB 386+ specifies the startup design directory path. ------------------------------------------------------------------ Old netlist format files are renamed when you install PCB 386+ ------------------------------------------------------------------ When you install PCB 386+, the install program checks your system for the presence of the following netlist format files: EDIF.CF EDIF.CCF FEDIF.EXE You must use the netlist format file supplied with PCB 386+ to create a netlist that is compatible with PCB 386+. When you install PCB 386+, the install program renames the currently installed netlist format files as shown below: EDIF.CF ------renamed to------ EDIFCF.OLD EDIF.CCF ------renamed to------ EDIFCCF.OLD FEDIF.EXE ------renamed to------ FEDIF.OLD ------------------------------------------------------------------ Display driver problems ------------------------------------------------------------------ EMS error from DRAFT -------------------- If you did not install new display drivers when you installed PCB 386+, you may encounter the error message "EMS error #160" when you attempt to run DRAFT. You must install the new display drivers supplied with PCB 386+. Using GENDRIVE to create a new display driver --------------------------------------------- PCB 386+ may freeze when it attempts to use a custom display driver created with an old version of GENDRIVE. PCB 386+ uses the display driver file creation date to verify that the display driver is a new and compatible driver. The program freezes if the driver passes the creation date requirements, but is not compatible with the display driver requirements for PCB 386+. Use version 4.40 or later of GENDRIVE to create custom display drivers for use with PCB 386+. ------------------------------------------------------------------ Loading libraries from previous releases ------------------------------------------------------------------ For most efficient operation, load all of your existing libraries from previous releases into PCB 386+ and save them out to new names. Note: Converted library files won't be 100% compatible with previous versions of PCB 386+. Modules can't be deleted in the old version and some menu dialog options may be missing. ------------------------------------------------------------------ Loading routed boards from previous releases ------------------------------------------------------------------ When loading routed boards from previous releases the initial load may take several times longer than normal. This is due to updating of the database to the new release version. Once saved after loading this will no longer occur. Note: Converted board files won't be 100% compatible with previous versions of PCB 386+. Modules can't be deleted in the old version and some menu dialog options may be missing. ------------------------------------------------------------------ Limits for pads and modules in autorouter functions ------------------------------------------------------------------ The following limits apply only when running the autorouter for routing or DRC checking. They do not apply in the editor. The limit on the number of pads per module has been increased from 750 to 1000. Note that this limits a board loaded as a module to having 1000 pads. The combined limit of modules + test points has been increased from 1800 to 2500. ------------------------------------------------------------------ Dealing with board objects that are off the work surface ------------------------------------------------------------------ When you load a board file, PCB 386+ checks for objects that are outside the visible screen limits, called the 'work space.' If the board file has objects outside the work space, PCB 386+ displays the Objects Outside of Work Space dialog box, which contains the following options: * Delete * Delete All * Do Not Delete * Do Not Delete All The type of object and the location of the object displays below the options. You can selectively delete objects, delete all objects, or retain all objects outside the work space. NOTE: If you retain all objects, and you have many objects outside the work space, the board file size can become large. Also, the board file may require more memory for some functions because all objects are considered. If you encounter low memory conditions, you may want to delete objects outside the work space. You can recover modules from outside the work space using the PLACE Module command. Follow these steps: 1. Select PLACE Module to display the Place Module dialog box. 2. Select the name in the Module Name list box for the module that is outside the work space, then select OK. The module is attached to the pointer. 3. Move the module to its new location. ------------------------------------------------------------------ Loading a netlist containing duplicate time stamps ***** CAUTION ***** ------------------------------------------------------------------ PCB 386+ cannot process a netlist containing duplicate time stamps. If duplicate time stamps are encountered, an error message displays. Versions of SDT prior to SDT 386+ v1.10 are able to create schematic parts containing duplicate time stamps. In these pre- v1.10 versions the BLOCK Save command copies sections of a schematic to a buffer. The BLOCK Get command retrieves the items in the buffer and copies them to the worksheet. The copied schematic parts have the same time stamps as the original source parts. To avoid duplicating time stamps, perform a BLOCK Export of the section of the schematic you wish to copy, then do a BLOCK Import of the file into the worksheet. The schematic parts in the imported file receive new time stamps. ------------------------------------------------------------------ Engineering Change Order (ECO) layers for PCB 386+ ------------------------------------------------------------------ Edit Layout has two board layers commonly used for Engineering Change Orders, or ECOs. You enter engineering change information on these layers, such as routing revisions or information about modules that need to be changed or added. You specify routing changes by drawing with outline segments. Do not use the ROUTE command to place tracks on the ECO layers. Use a color that distinguishes the ECO layer from the other layers. Select PLACE Text to enter text on the ECO layers. ------------------------------------------------------------------ Determining the filename of the current board file ------------------------------------------------------------------ Before you select QUIT Update Board File to save the current board file, you can determine the filename it will be saved to by following these steps: 1. Select QUIT Initialize Board File. The filename of the loaded board is highlighted in the Files list box on the Initialize to Board File dialog box. 2. Select Cancel to close the dialog box. ------------------------------------------------------------------ Deleting a copper tool in PCB 386+ ------------------------------------------------------------------ If you attempt to delete a copper tool that is still used by an object, you receive a notice stating that the copper tool is being used and it cannot be deleted. If you assign a different copper tool to the object but you still cannot delete the original copper tool, check objects that remain in the undelete buffer. If an object in the undelete buffer uses the copper tool, permanently delete the object or select QUIT Flush Undelete Buffer to remove all objects from the undelete buffer. You should be able to delete the copper tool. Another possibility is that the copper tool is used as a default for something in the Current Settings dialog which also prevents deletion. This same situation can occur when deleting pad stacks or drills. ------------------------------------------------------------------ Working with planes in PCB 386+ ------------------------------------------------------------------ Planes: General information --------------------------- When a layer is enabled as a plane and assigned a net name, the plane does not display in PCB 386+. You can select a different display color for the plane layer, but the plane is invisible. Starting with PCB 386+ v2.21 you can place fill zones, nofill zones, and tracks on plane layers. Connectivity and thermal relief is automatically created between the plane and all through-hole pads and vias assigned to the same net. SMT pads are connected to planes when they are autorouted using the Dispersion option. Suggested autorouting procedures are described below for boards that use planes and have already been dispersion routed: 1. Select GO TO FUNCTION, then select Net Property Editor from the menu. The Edit Net Properties dialog box displays. 2. Select the net in the Net Names list box that is assigned to the plane. 3. Enable Do Not Route Net and Lock Existing Routes, then select Selected Net. If necessary, select additional nets and options and select Selected Net for each net. Select OK to accept the new settings and close the dialog box. This prevents the autorouter from routing the selected net - it is already routed to the plane. 4. If desired, display the Copper Colors/Enables/... dialog box and disable the plane layers if no autorouting barriers are on them. This saves autorouter time and memory. NOTE: If you do this, be sure to enable the plane layers before you plot the board. 5. Select GO TO FUNCTION Autorouter. 6. Select Set to display the Autoroute Options dialog box, then select autorouting options and select OK. 7. Select Whole Board, then select Autoroute Whole Board from the menu to route the remaining nets. Maximum number of characters for a netname assigned to a plane -------------------------------------------------------------- Do not create a netname containing more than 21 characters for a net you intend to assign to a plane. If a netname has more than 21 characters it cannot be selected as a plane in the Copper Colors/Enables/... dialog box. The netname does not display in the netname droplist box for a plane layer because the netname becomes the layer name, and layer names cannot be longer than 21 characters. Display of plane layer names in layer droplist boxes -------------------------------------------------------------- In layer droplist boxes layer names for planes are shown with a preceding number such as " 1 - " or " 2 - " to distinguish between having more than one plane layer assigned the same name. ------------------------------------------------------------------ PCB 386+ zone information ------------------------------------------------------------------ Z-Order --------------------- You can place fill zone within fill zones if you use Z-Order. Refer to the Z-Order option in the PC Board Layout Tools 386+ v2.20 Update Guide. Overlaying fill zones --------------------- Do not place a fill zone within another fill zone. No isolation is created between the zones if they are assigned different nets. See Z-Order above. Placing a fill zone on the All External Copper layer ---------------------------------------------------- Do not place a fill zone on the All External Copper layer. The fill zone on each external copper layer contains isolation for both Component Copper and Solder Copper objects. Instead, create two separate fill zones. ------------------------------------------------------------------ DRC checking ------------------------------------------------------------------ DRC checking on tracks constructed with arc segments ---------------------------------------------------- DRC checking in Edit Layout may report a clearance violation between a copper object and tracks constructed with arc segments, even though no violation exists. To guarantee proper clearance between arc tracks and other copper objects, follow these steps: 1. Select SET to display the Global Options dialog box. 2. Enable Show Highlight Guard. This displays the copper-to-copper spacing for highlighted copper objects. You can also enable Show Copper and Guard While Drawing to display the copper-to-copper spacing for all copper objects that are already on the board. 3. Enable Show Copper And Guard While Routing. The copper-to- copper spacing for the arc segments displays while you route. 4. Select OK to close the dialog box. 5. Zoom in on the area you are routing with arc segments and use the displayed guard bands as a visual guide to determine if you are routing too close to another copper object. Deleting DRC violation markers ------------------------------ Do not select Delete DRC Violations in the Autoroute Options dialog box to delete DRC markers. Selecting Delete DRC Violations deletes the offending tracks during autorouting. Instead, follow these steps: 1. Correct all DRC violations. 2. Select GO TO FUNCTION Autorouter. 3. Enclose the corrected area within a block. 4. Select Spacing/DRC Check Block. The Finished dialog box displays the number of DRC violations. Select OK. If the number of violations is zero, all DRC markers are deleted. If DRC violations are still reported for areas containing arc tracks, and you know there is adequate clearance, follow these steps to delete those DRC markers: 1. Select LAYER to display the Layer dialog box. 2. Select Comment Layer, then select OK. When the Comment Layer is active, you can delete DRC markers without accidentally deleting other objects. 3. Place the pointer on the DRC marker and select DELETE. You can prevent PCB 386+ from displaying the DRC markers using this method: 1. Press to dismiss the Autorouter menu. 2. Select SET to display the Global Options dialog box. 3. Disable Show DRCs, then select OK. DRC markers do not display. ------------------------------------------------------------------ Matching PCB 386+ plots and NCDRILL files ------------------------------------------------------------------ PCB 386+ mirrors plots on the Y axis if the Mirror Y button in the Advanced Printing and Plotting Options dialog box is disabled. If you enable Mirror Y, plots are not mirrored on the Y axis. To create matching artwork and drill files, follow these procedures: Unmirrored plots and drills --------------------------- 1. Plot the board file with the Mirror Y option enabled. The plot will not be mirrored. 2. Run NCDRILL without the /FLIP Y option. Mirrored plots and drills ------------------------- 1. Plot the board file with the Mirror Y option disabled. The plot will mirror. 2. Run NCDRILL with the /FLIP Y option. ------------------------------------------------------------------ Running NCDRILL_ on a board with disabled layers ------------------------------------------------------------------ When you run NCDRILL_.EXE with the /ENTIRE switch, it looks at all of your enabled copper layers to determine where your drill holes start and stop. Any copper layer on which you placed a pad, a trace, or a zone should be enabled before you run NCDRILL. If you have a one layer board, you should enable both the Component Copper and Solder Copper layers before running NCDRILL. ------------------------------------------------------------------ Flipping modules ------------------------------------------------------------------ Setting proper SMT pad angles for flipped modules ------------------------------------------------- SMT pads may not be oriented at the correct angle when a surface mount module is flipped to the other side of the board. To orient the pads properly, you rotate the module to the desired angle after you flip it to the other side of the board. Preventing the shifting of flipped modules ------------------------------------------ When you flip a module the module may shift its relative position. The shift occurs because the pointer becomes the center point for the flip function. To make sure that the module does not shift, select the module from its center, if possible. Also, the module does not shift if you block select the module so it is centered within the block. ------------------------------------------------------------------ Mirroring objects in the board editor ------------------------------------------------------------------ Be sure Allow Move/Edit/Delete of Module Elements is disabled in the Global Options dialog box before you block select an area of your board and attempt to mirror the objects within the block. When Allow Move/Edit/Delete of Module Elements is disabled, modules inside the block do not mirror with the rest of the objects. ------------------------------------------------------------------ Memory problems while running PCB 386+ ------------------------------------------------------------------ Configuring a PIF file to avoid PCB 386+ low memory in Windows -------------------------------------------------------------- When PCB 386+ is run from DOS it displays a low memory error message if the available RAM and virtual memory swap file disk space is almost completely consumed. The error message does not display if PCB 386+ is run under Windows. Unexpected behavior can occur if insufficient memory is available. If you do not use a unique PIF file to start PCB 386+ under Windows, Windows uses the memory settings in DOSPRMPT.PIF. The default memory settings in DOSPRMPT.PIF may be insufficient. You can increase the amount of available RAM if you create a new PIF file, enter the necessary parameters to run PCB 386+, and increase the values in the KB Required and KB Limit entry boxes for XMS Memory. For example, if you have 8 megabytes of RAM, enter 4000 (4 MB) in the KB Required entry box and enter 8000 (8 MB) in the KB Limit entry box. Save this PIF to a new filename, then select the PCB 386+ icon, select File Properties, and enter the new filename in the Command Line entry box of the Program Item Properties dialog box. Virtual memory availability while running PCB 386+ under Windows ---------------------------------------------------------------- When you run PCB 386+ under windows the configured PCB 386+ virtual memory swap file is disabled and PCB 386+ uses the Windows swap file. This reduces the speed of some operations. You may encounter low memory situations if you edit a large board and the amount of virtual memory is insufficient. The Windows swap file does not dynamically increase its size as program demands increase. Virtual memory capacity warnings -------------------------------- To successfully load a board file, the virtual memory swap file size (in bytes) must be at least twice the size of the board file. PCB 386+ issues a warning if the swap file size is less than three times the size of the board file. Acquiring more virtual memory ----------------------------- To prevent low memory conditions, provide as much contiguous free disk space as possible for the swap file. Delete files and defragment the disk, or place the swap file on an empty partition. Do not save a board file when "Out of Memory" displays ------------------------------------------------------ Do not try to save your board file if an "Out of Memory" message displays in PCB 386+. The Phar Lap virtual memory swap file is corrupted because of insufficient disk space. EMS message for PCB 386+ utilities ----------------------------------- If you do not have enough EMS memory while running a PCB 386+ utility program, you may encounter a message similar to these: EMS error, code 8A from function 0044 EMS handle 5 ERROR (FROMPCB2), Error accessing EMS, requested output will be incomplete The code, function number, and EMS handle number varies depending on system conditions. The utility encountering the EMS memory problem displays in parentheses. Out of memory messages from PCB 386+ utilities ---------------------------------------------- Use the /Page_Size switch to provide additional memory for processing. The following utilities use the /Page_Size switch: COMPNET_.EXE FIXTIME_.EXE REANNO_.EXE MODLOC_.EXE ---------------------------------------------- See Appendix A in the PC Board Layout Tools 386+ Reference Guide for information about these utilities and the /Page_Size switch. You select the /Page_Size switch in ESP by enabling Specify RAM page size, then selecting 4096, 2048, or 1024. ------------------------------------------------------------------ Abnormal program termination: Device Not Available message from PCB utilities ------------------------------------------------------------------ If the time stamps of the ASCII (PCB.CFG) and binary (PCB.BCF) tool set configuration files differ, then PCB386.EXE or its utilities will attempt to run the program PCB_C.EXE to compile the ASCII tool set configuration. On systems with early (pre-1990 versions) of system BIOS (Dell Phoenix or AMI American Megatrends Inc.) running with memory managers (early versions of Quarterdeck's QEMM or current versions of Microsoft EMM386), the programs will abort and report: "Abnormal program termination: Device Not Available." To avoid this problem, use the ESP Design Environment, Configure PC Board Layout screen to manipulate the PCB 386+ tool set configuration, or run the command line: PCB_C/B to compile the ASCII tool set configuration. ------------------------------------------------------------------ Running under Windows 3.1 ------------------------------------------------------------------ Running multiple sessions of ESP under Windows 3.1 ------------------------------------------------------- You can run multiple sessions of ESP under Windows 3.1 and Windows for Workgroups, but not under Windows 3.0. SHARE.EXE must be loaded. You will need to monitor memory consumption if you use the PCB 386+ autorouter. Suspending to DOS from PCB 386+ while running in Windows -------------------------------------------------------- If you are running PCB 386+ from Microsoft Windows and you need to access the DOS command line, it is recommended that you do not select Suspend to System from PCB 386+. Suspending to system from PCB 386+ while running it in Windows may cause an abnormal program termination when you exit from the DOS session and return to PCB 386+. This may occur if you run certain applications that detect 386/486 processors, such as the new versions of PKZIP and PKUNZIP. Instead, display the Program Manager and double-click on the MS-DOS Prompt icon to start a DOS command line editing session. After you run your DOS commands, leave the DOS session open if you may need to enter commands later, then switch to PCB 386+. Selecting an OrCAD icon in Windows ---------------------------------- When you install PCB 386+, an OrCAD icon (ORCAD.ICO) is installed in your ORCADEXE directory. You can use this icon for your OrCAD applications that are installed in the Windows Program Manager. Follow these steps to change the icon to ORCAD.ICO: 1. Select the icon for the OrCAD application you wish to change. 2. Select File from Program Manager. The menu displays. 3. Select Properties... to display the Program Item Properties dialog box. The current icon displays in the dialog box. 4. Select Change Icon... to display the Change Icon dialog box. The path for the icon displays in the File Name entry box, and the current icon displays in the Current Icon select box. 5. Select Browse... to display the Browse dialog box. 6. Change the directory to your ORCADEXE directory. 7. Select ORCAD.ICO in the File Name list box, then select OK. The dialog box closes and the new icon and directory path displays in the Change Icon dialog box. 8. Select OK. The Program Item Properties dialog box displays, and the new icon displays in the dialog box. 9. Select OK. The dialog box closes and the new icon displays for the OrCAD application. ------------------------------------------------------------------ Communicating with invalid devices or ports in PCB 386+ ------------------------------------------------------------------ PCB 386+ uses various functions which communicate to devices, such as floppy drives, network drives, and serial/parallel communication ports. If the device or port is inactive or invalid you may encounter problems. For example, you may direct PCB 386+ to write a file to a floppy drive that does not contain a floppy disk. You could also direct PCB 386+ to plot a file to the COM port assigned to your mouse. If you run PCB 386+ from DOS, an error message displays for either of these cases. The error message describes the status of the device, such as "Write fault error writing device COM2." The error message also displays "Abort, Retry, Ignore, Fail?" as choices of action. Please choose the action carefully. CAUTION: Selecting "Abort" causes PCB 386+ to halt operation and return to DOS without saving the current state of your board. You will need to reset your computer. If at all possible, do not select Abort. It is a good idea to save your board file before attempting to access different devices. If you can correct the problem, such as placing a floppy in the empty floppy drive, select "Retry" and the process will continue normally. If you cannot correct the problem, such as directing PCB 386+ to print or plot to the COM port that your mouse uses, select "Fail." This option halts device access, but PCB 386+ continues operation, displaying a "Printer output error" message. Your mouse is disabled, so you will need to press to dismiss the error message. You can use the cursor keys and shortcut keys to move the pointer. Select the commands to save your board file and quit PCB 386+, then return to DOS. Reload your mouse driver, if necessary. If you run PCB 386+ under Windows 3.1 and perform the same actions, the "Abort, Retry, Ignore, Fail" error message does not display. However, the "Printer output error" message does display. Use the arrow and shortcut keys to save the board file and exit to the Program Manager, then restart PCB 386+. The mouse will be restored. ------------------------------------------------------------------ Printing to a serial port ------------------------------------------------------------------ If your printer is connected to a serial port, you need to run the DOS MODE command before you start PCB 386+ and attempt to print to the serial device. MODE configures the communication settings for the serial port. If your printer is connected to COM1, and your other communication parameters are 9600 baud, no parity, 8 data bits and 1 stop bit, you enter the following command at the DOS prompt: MODE COM1: 9600,N,8,1 After you enter the command, run PCB 386+ and select COM1 in the Output Configuration dialog box to print the pages in the board file. If the port has not be set up correctly and your layout is large enough to overflow the COM port buffer, you will see the message: Unable to write printpath. MS DOS Error #14 Disk is Full If you are running under Windows, you will need to enter this command before invoking Windows. The most convenient way to make sure that this command is issued is to put it into your AUTOEXEC.BAT file. If you prefer to enter the mode command after Windows is running, you need to go to the Windows Control Panel for Ports. Click on the COM port in question, and then Settings. Change the control flow setting to hardware. Now entering the mode command in a DOS prompt window will change the setting. ------------------------------------------------------------------ Gerber viewer problems ------------------------------------------------------------------ Some Gerber viewers may inaccurately display pad orientations or connections between some pads and planes or fill zones. The situation occurs because some viewers may not properly interpret data in Gerber (274-X) files, while others may misrepresent Fire 9xxx or Gerber (274-D) files. If your present Gerber viewer displays unexpected pad orientations, or shows other objects in unusual ways, view the Gerber files with another viewer. Shareware versions of both DOS and Windows-based Gerber viewers are available on the OrCAD bulletin board. Downloading a demo Gerber viewer from the OrCAD bulletin board --------------------------------------------------------------- Both Windows and DOS versions of Gerber viewers are available on the OrCAD bulletin board. You can download these files from the Customer Contributed Programs section of the Board Layout Tools area. The phone number for the OrCAD bulletin board is (503)671-9401. Lavenir Gerber viewer settings for arcs ---------------------------------------- Arcs in Gerber files produced by PCB 386+ may display enlarged or distorted when the Gerber file is displayed in a Lavenir Gerber viewer. Select "Quadrant interp" from the Lavenir viewer options. Arcs will display correctly after selecting the option. ------------------------------------------------------------------ Printing circles placed as four arcs ------------------------------------------------------------------ When you place a circle as a circle, you get a circle object. When you place a circle as four arcs, you actually create an outline object that contains four arcs. The outline object prints as an outline. Enable Outlines in the Printing and Plotting dialog box to print circles placed as four arcs. ------------------------------------------------------------------ Corrections to the PCB 386+ printed documentation ------------------------------------------------------------------ The following entries are corrections to the PCB 386+ printed documentation: PC Board Layout Tools 386+ User's Guide --------------------------------------- Addendum -------- Chapter 3 (begins on page 19). This chapter describes how to transfer a design from OrCAD's Schematic Design Tools to PCB 386+. The procedures and figures depict version 4.30 of the ESP design environment and version 1.10 of Schematic Design Tools 386+. The following figures shown in chapter 3 are unique to ESP v4.30: * Figure 3-2. Design Management Tools screen, Design View. * Figure 3-6. The Schematic Design Tools screen. * Figure 3-8. Partial view of the Configure Schematic Design Tools screen, Library Options section. * Figure 3-12. The Configure Update Field Contents screen. The following menus shown in chapter 3 are unique to ESP v4.30 or above: * Configuring INET, Local Configuration * Configuring ILINK, Local Configuration * Configuring IFORM, Local Configuration The following changes apply if you use SDT Release IV and SDT 386+ v1.0X: In the section "Viewing key fields," there are no preconfigured key field entries in the Configure Schematic Design Tools screen. The key fields must be defined by the user. In the section "Updating Field Contents," TUTOR.STF is not selected from the Files list box. The name of the update file must be entered in the Update file entry box. Also, Part Field 8 is not automatically selected in the Field to be updated section of the Configure Update Field Contents screen. The part field must be defined by the user. In the section "Checking design integrity," there is no Check Design Integrity tool to configure and incrementally execute Cleanup Schematic, Cross Reference Parts, and Check Electrical Rules. The processors must be selected individually. The following changes apply if you use SDT Release IV only: In the section "Creating the netlist," the "Configuring IFORM" procedures describe selecting FEDIF.EXE in the Netlist Format list box. You select .CF or .CCF in this list box. Errata ------ Page 38. The picture does not match the software. Part Field 8 has been renamed Module Value and the two "Convert" options have been rephrased. Page 39. Step 8 is not needed. Page 47. The picture should show that the Ignore Warnings option has been selected. Page 48. Step 6 should read, "Select the Ignore Warnings option. Then select OK." Page 55. The Driver Prefix shown in the picture should be C:\ORCADESP\DRV\ Page 116. Step 5 should read "Place the pointer in the center of 'module', as shown at right." Page 139. Step 1 should say to select OK after selecting ORIGIN. After selecting OK the origin changes. Page 143. Steps 7 and 8 repeat information from the bottom of page 142. Page 259. Step 2 says that 32 pens can be configured. The correct number is 31. NOTES: The Module Value key field and Part Field 8 are one and the same. The module footprint for U2, U3, and U4 on DEMO.BD1 and PLACED.BD1 is incorrect. The part is a 22V10, which should be a narrower footprint. The incorrect module footprint is also in TUTOR4.MLB, the module library that is used when you load a netlist in Chapter 6: Placing the TUTOR board. PC Board Layout Tools 386+ Reference Guide ------------------------------------------ On page 135 the heading "Copper Tool" in the edit zone dialog should actually read "Zone Boundry Copper Tool". In addition the width should be displayed to the right of the copper tool selected. Page 137. This information should be added to the discussion of Fill Pattern Type option on the Edit Zone Properties dialog box. There are six fill pattern types available. They are: Horizontal Vertical (the default) Cross hatch (both Horizontal and Vertical) Left 45 degree Right 45 degree Cross hatch 45 degree (both Left 45 and Right 45) On page 214 the netlist load option "Delete unconnected Test Points" should read "Delete Test Points". When this option is selected Test Points which have no net assignment, or those in a net which is removed during the netlist load, are deleted. Figure 6-1 on page 304 in Chapter 6: Create NC Drill File should contain a radio button for "Excellon trailing zero suppressed", the radio button for "Excellon leading zero" should read "Excellon leading zero suppressed", and the buttons to specify the RAM page size have been removed. ------------------------------------------------------------------ PC Board Layout Tools 386+ version 2.21 Update Guide Errata ------ On page 7: The proper command line under Modify Modules is: MODMOD_ my.bd1 my.asc /all /version 2.00 (Note the placement of spaces, and the use of the /all switch.) ------------------------------------------------------------------ Importing plots into Microsoft Word ------------------------------------------------------------------ The documentation shipped with Microsoft Word states that it will import HPGL files as pictures embedded within your document. Microsoft Word actually imports HPGL2 files. Note that because of limitations in the graphic filters shipped with Word, the pads will not be filled and all lines will be printed one pixel wide rather than at the width indicated in the plot file. Beginning with release 2.00, you may embed Postscript files from PCB 386+ as pictures within Microsoft Word. The pictures will print from within your document smaller than the original plot but will otherwise be perfectly rendered in every respect. While editing your document, the embedded postscript picture will appear as a simple frame with only the identifying text displayed on the screen. If the file is sent to a Postscript device, it will be plotted correctly and both the frame and the identification text will vanish. If printed to a raster printer, the plot will appear exactly as shown on your screen which is effectively worthless. OrCAD has verified that as documented in the Microsoft Knowledge Base, PSS ID Number Q104557, embedded Postscript files will not display their graphic contents under Windows NT version 3.1 no matter which output device is selected from within Word. However, embedded postscript files appear to print properly from within Word running under Microsoft Windows 3.11. ------------------------------------------------------------------ How to interrupt a copper pour ------------------------------------------------------------------ If Show Copper Pour has been enabled from the Set Global Options menu zone fills can be interrupted pressing the key. ------------------------------------------------------------------ Loading of .PFG file can cause temporary unit switch. ------------------------------------------------------------------ Loading a .PFG(Print/Plot Configuration File) that has been set for inches into a board that has the 'Display Metric Dimensions' option set, can cause the display to temporarily revert back to inches after exiting the Printing and Plotting menu. To restore the units back to millimeters, re-enter the Global Set menu and select OK. Then go back to the Printing and Plotting dialog and re-save the .PFG file setup, it will now match the setting in the Global Set Menu.