READ.ME file for Protel Autotrax version 1.61 Special Protel for DOS edition (c) 1990-92 Protel Technology Inc. All rights reserved. Warning: this document and the software programs it describes are protected under US and International copyright law. All unauthorized duplication or distribution of this material, in any form, is prohibited. Violators are subject to severe civil and criminal penalties, including fines and/or imprisonment. Installation notes For convenience, the software has been compressed into a special archived format and must be installed using the INSTALL.EXE program, included on the Install diskette. To install the software, you simply type INSTALL and press RETURN... then follow the on-screen prompts. Once the files have been installed, you can re-organize your directory structure if you wish following the same guidelines documented in the original reference manual. The directories that are displayed in the Install program are optional. For example, you need not create a special GRAPHDRV directory. Windows 3.0 and 3.1 Autotrax can run as a DOS application under Windows. This allows you to have multiple applications or documents loaded, memory permitting. For information about setting up Schematic to run under Windows, see your Microsoft Windows Users Guide. Installing a graphics driver Both Autotrax and Schematic use the same graphics drivers. Only only set of drivers needs to be installed. Although the Install program prompts you to create a special graphics directory (GRAPHDRV) this is optional. Keeping all the graphics drivers in a single directory is useful if you regularly use more than one Protel package, (the drivers are identical) or if you wish to change drivers regularly. The reference manual guidelines for installing (or changing) the graphics driver are still valid. Be aware that the single file GRAPH.DRV must either be in the same directory as TRAXEDIT.EXE or you must set the DOS PATH variable to include the directory with GRAPH.DRV. The easiest way to do this is to include a PATH statement in your AUTOEXEC.BAT file. Please refer to your DOS manual. You need not keep the other .DRV files (EGA.DRV, etc.) on your hard disk unless you wish to be able to change drivers conveniently. New Graphics drivers (see the Reference Supplement) Since publication of the supplement, we have added new drivers for the ATI VGA Wonder card, the Paradise EGA480 card and the Trident TVGA card. A complete listing of the current drivers follows: Herc Monochrome CGA Color Graphics Adaptor EGA Enhanced Graphics Adaptor VGA640 VGA Standard, 640 x 480 - 16 color VEGA Vega Deluxe Extended EGA, 640 x 480 - 16 color PARA800 Paradise VGA Pro, 800 x 600 - 16 color GENOA640 Genoa Extended EGA, 640 x 480 - 16 color GENOA800 Genoa Extended EGA, 800 x 600 - 16 color GENOA912 Genoa Extended EGA, 912 x 350 - 16 color EIZO800 EIZO MDB-10, 800 x 600 - 16 color TECM800 Tecmar VGA-AD, 800 x 600 - 16 color EIZO1024 EIZO MDB-10, 1024 x 768 TECM1024 Tecmar VGA-AD, 1024 x 768 VID7800 Video7 VGA, 800 x 600 VID71024 Video7 VGA, 1024 x 768 WOND800 ATI VGA Wonder Card 800x600 WOND1024 ATI VGA Wonder Card 1024x768 PEGA480 Paradise EGA480 chipset cards 640x480 TRID800 Trident TVGA chipset cards 800x600 TRID1024 Trident TVGA chipset cards 1024x768 A number of these drivers are compatible with cards from many different manufacturers. Normally this compatibility is determined by the "chipset" on the card, so some experimentation may be needed to determine the best driver for your combination of graphics card and monitor. In many cases, a card may support the driver at a lower resolution, so if a 1024x768 driver fails, try the 800x600 version. Most current cards will support the VGA640 driver. GRAPHSET This installer has been supplied to make it easy to change the graphics driver after the program has been installed. Type GRAPHSET and press RETURN, then follow the on-screen prompts. Protel Autotrax capabilities Protel Autotrax is a complete PCB layout environment with many attractive features for productive design work. You can use Protel Autotrax as a stand-alone manual board layout. When combined with a schematic capture package (Protel Schematic or other popular software), Protel Autotrax becomes the backbone of a fully-automated, end-to-end design system that features a high degree of design automation and integration. However you use Protel Autotrax, you'll appreciate its ease- of-use and the high degree of flexibility built into this proven PCB design system. Autotrax generates through-hole and SMD designs of up to six signal layers, plus power and ground planes. Board size can be as big as 32 inches (or 81 cm) square. Placement accuracy is to 1 mil (.001 inch or .025 mm). A metric/imperial grid system allows you to work accurately in both measurement systems and the grid can be 'toggled' between metric and imperial modes as you design. Full support is included for popular netlist formats. Importing a schematic netlist allows you to take full advantage of Autotrax's auto component placement, autorouting and design rule checking facilities. For output, Autotrax supports dot matrix, laser, and postscipt printers; pen plotters; and includes Gerber plot and Excellon N/C drill file capabilities. 'Building' a PCB design is a straightforward process of: 1) Selecting the layers that will correspond to the PCB tooling required for your design. These can include a top (component side) layer, bottom (solder side) layer, up to 4 additional mid layers, power/ground plane layers, top and bottom silkscreen layers. Other special purpose layers are also supported; 2) Placing the required component patterns from a component library. Or, if working from a schematic netlist, using automatic component placement to load and position the components into a pre-defined board outline; 3) Connecting the component pads with tracks, manually, with the autorouter, or by combining manual and automatic track routing strategies; 4) Checking your work using Autotrax's built-in design verification tools; 5) Printing or plotting the required manufacturing artwork using printers, plotters, Gerber and N/C drill file output options. Unlike generic 'CAD' drafting packages, Autotrax provides special features that address the unique requirements of PCB design: PCB layout revolves around four basic procedures: placing objects in the workspace - components, free pads, vias, text strings, tracks, area fills and arcs; moving objects; deleting objects; editing, or changing object attributes such as the width of a track or the contents of a text string. Autotrax has the ability to edit and print or plot the individual layers that correspond to the manufactured board. Whether your design is a simple single-sided PCB, or a multi-layer board with power and ground planes, you will be able to layout every item exactly as it will be assembled. A key feature of PCB is the way electrical connections between the elements in your design are recognized. This concept of connectivity is the basis of automatic component placement, autorouting and design rule checking and extends to modifying your layout. For example, you can drag components and the connected tracks will stretch, or rubberband, without being broken. The application stores connection information which can be used to generate a netlist directly from a routed PCB. This netlist can be used to facilitate checking of the completed design. PCB will also generate reports, such as a Bill of Materials listing the components used in your design. Autotrax provides layer support and library component patterns for both through-hole and SMD technology designs, accepts netlists directly from Protel Schematic, and supports other popular schematic netlist formats. Component libraries A comprehensive library of pre-defined SMD and through hole components is included in the Autotrax package. The Protel system also includes a complete set of commands for creating, editing and using library components. The user can create different component libraries for various uses quickly and easily. Pad types Pads are organized into libraries, similar to components, with each Pad Type having a predefined size, shape, layer assignment, hole size and power/ground plane status. One Pad Type from the open library is always the 'current' type, selected using the Current Pad Type command. Netlists Netlists are common to most electronics design environments. Simply stated, a netlist is a summary of all the connections (or networks) that comprise a circuit. These netlists are usually generated by a schematic capture package but can also be created manually. Netlists are generally simple ASCII text files. The typical netlist format includes descriptions of components, such as the designator and package type combined with the pin-to-pin connections that define each net. Loading a netlist into a PCB layout package automates many of the tedious and error prone operations inherent in PCB design. In Protel , netlists allow you to automatically load all components into the workspace and display all the pin-to-pin connections, called a ratsnest, prior to routing the board. Netlists allow the designer access to auto component placement and autorouting. Physical PCB design Setting up the workspace layers Layers should be assigned to different colors to provide maximum differentiation between them. As you make color assignments, it is important to make sure that your assignments don't conflict in some way that will obscure vital details when you edit your layout. It is recommended that you start with the Background and Highlight assignments, if you wish to change a number of the defaults. Some layers are not displayed during the Design Process, but are Generated automatically when printing or plotting. For example, the Solder or Paste masks. Remember that although several layers can be 'active' and displayed simultaneously, only one layer can be the 'current' layer. Single layer items such as tracks, fills, arcs or text are always placed on the current layer. Defining a board One of the first operations performed, would normally be to define the physical outline of the PCB. There are several ways that this can be accomplished in the Protel system. If you are using auto component placement and autorouting (from a schematic netlist), you must use the special Keep Out layer to define the perimeter of the usable board area and any 'no go' zones where components and/or tracks are to be excluded when these automated operations are performed. Now that a work space exists the board is ready to be designed. Please go to the Tutorial chapters in the reference manual for a step-by-step introduction to the layout processes and other tools for generating finished, professional quality board designs. CORRECTIONS/UPDATES - Reference Supplement Page 3 As documented in the cover note, installation now is performed using the special INSTALL program. Copy Protection The hardware lock device (or "dongle") referred to in the manual is no longer required to run Autotrax. You can make unlimited copies for your own use per the conditions of the Protel Software License Agreement, enclosed with this package. Page 5 Curved Tracks Placement. Select the Curved option from Setup/Options/Track Mode, not Current/Track Mode. Page 8 Question Delete option. Default is 'Off'. Route Display option. This option has been removed. TIPS, HINTS and REPORTED PROBLEMS Since the manual was originally printed, a great number of changes have been included during upgrades and revisions to the original TRAXEDIT and TRAXPLOT files and a number of utilities have been added or enhanced. A list of reported software problems (including some errors and product limitations) has been included. Most of the known problems described in this section can be avoided or overcome by using the work- arounds documented below. TRAXEDIT version 1.61 File Quit Yes command When quitting, you are prompted "Save changes to PCB file." If you choose "Yes" and the file was previously saved, the prompt "PCB File Exists, Confirm Overwrite" appears. If you respond "No" the program will not prompt for another filename, but exits from the program without saving changes to the current file. To avoid this problem, use the File Save command if you wish to re-name the current workfile, prior to quitting Autotrax. If you forget to do this, or accidentally respond "No" to the Confirm Overwrite? prompt, you may be able to recover most of your work by re-loading the .ABK or .BAK (auto back- up) versions of the file. Highlight command Highlight Connection or Highlight Net fails to highlight the entire connection or net. This is due to a fixed recursion limit in the highlighting algorithm and will occur in large complex connections. It is sometimes possible to work-around this limit by selecting a starting point near the middle of the net, which limits the recursion necessary to trace and highlight each segment. Highlight Connection command Final connection to pad is not highlighted on connections with 3 or more track segments connected to a square component pad. You can overcome this by temporarily changing the pad shape (you can also use global feature to change all square pads). Return the pads to the square shape before generating artwork. Netlist Route command The completion percentage shown on the Status line does not include prerouted tracks and not reach 100%, even if all ratsnest connections have disappeared from the display (i.e. the route is finished). Netlist Route Board command Using Route Board with the Process Pre-Routes pass enabled and all other passes disabled causes "via stringers" to be routed to SMD pads. When using SMD components, do not run Process Pre-Routes without having other passes activated. See the Reference Supplement section of the manual for information about SMD stringers. Netlist Route Board command Autorouting sometimes creates a "T-junctions" that do not use a vertex (break) in the track at the top of the T. Later, dragging of tracks, blocks or components will break the connection at this point. You must manually re-connect at the "T", if this happens. Netlist Route Manual route Option Netlist Route Manual command When manually routing connections from a loaded netlist, you can Show a selected net. The 'ratsnest' will 'follow' the tracks that are placed, making it easier to see your progress to the destination pad. This works for individual connections or an entire net. New separation option in the autorouter A via-to-pad separation clearance has been added to the router. This will prevent via placements which block access to pads during subsequent routing attempts and should result in overall improvements to the completion rate and quality of autorouter results for many boards. The default clearance is 13 mils. Smoothing options Users have the option to apply smoothing passes, such as via minimization, etc. to pre-routed tracks, if Smooth Pre-Routes is selected. Autotrax identifies pre-routes as any connections completed by the user. Connections made by the autorouter are not regarded as pre-routes and automatically smoothed. Autorouter Wave routing A routine has been added to the router which allows the placement of short 45 degree 'wave' segments, to allow the router to pass obstacles without changing the search axis. The user can specify the maximum number of waves permitted in a connection. Select Netlist Router Route Variables and specify a number 0-9999. The default is 1. Arc replacer pass in autorouter Users can select Arc Replacement as an autorouter smoothing pass. This option will replace 90 degree corners with arcs. The arc line thickness used is determined by the track size selected in the Netlist Route Route Variables option. Make sure that you select Smooth Pre-routes 'On', if you want these tracks processed. SMD routing for Ground Power planes The problem of autorouting Surface Mount components with internal ground power planes has been simplified by the addition of 'stringers' + short track pad segments which provide a 'thermal relief' connection to internal power or ground planes. Place External Plane command Does not consistently calculate the clearances around pads, and will not always be able to completely fill corners, etc., leaving an irregular structure. You may want to manually clean-up these areas in complex polygons. External planes do not automatically tie to a specific net (e.g. GND). However, if you manually connect the plane to a primitive on a net, the plane will be recognized by connectivity features, such as highlighting and DRC. The current version does not 'cap' diagonal portions of the fill with an 'outline' track. It will cap all horizontal or vertical tracks. You can specify a small track size/grid to minimize the 'scalloped' diagonal effect, or manually place smoothing tracks after the fill is defined. Repeat Place command If you are using the Repeat Placement feature with some fractional metric grids, the Offsets applied to repeats can result in some unexpected placements. This is because the metric value must be rounded off to two decimal places. For example the default 25 mil imperial grid is equal to approx .625mm, rounded-off to .63 mm by Autotrax. If you attempt a repeat placement of a row of pads, this rounding-off will result in a cumulative error in spacing as successive pads are placed. The solution is to use even multiples of the current snap grid as offsets OR to work on a 'natural' grid pitch, i.e. .5 mm or .6 mm OR to stay on the imperial grid, rather than switching to metric prior to repeat placement. Cursor key array (AT style keyboards) Left or down cursor keys randomly causes cursor to move two grids instead of one. You can use the numeric keypad cursor keys, change the Snap grid setting or Zoom-in and use the mouse to get to the correct grid point. Moire pad shapes A Moire pad with a diameter less than .140" or 3.55 mm is not displayed on the screen, but can still be selected and edited. The pad will be printed or plotted normally. Move Drag Track End command Curved sections of track may not move in the display, until it is placed in its new location. It then appears, along with the original image of the curved track. Press End (or use a Zoom command) to re-draw the screen. Grid options When setting a metric Snap grid of 0.03 mm, after moving the cursor four times in any direction, it stops and cannot be moved the fifth time. The x, y coordinates displayed on the status line are not always a multiple of 0.03 mm - it is a display and cursor control problem only. No work-around is available except to choose another Snap grid value. This does not effect placement accuracy. Design rule checking (Netlist DRC option) False Clearance errors between pads and vias will sometimes be reported. If you can visually confirm that no actual violation exists, you can ignore these warnings. Memory management If memory is a problem, make sure that your operating system is as 'bare' as possible - disable network software and any TSRs (other than EMS Mouse drivers), etc. If memory is still a problem you may need to consider additional EMS (Autotrax supports up to 4MB). Unverified TRAXEDIT problems The following problems have been reported by users, but have not been reproduced by Protel Technical Support staff: Highlight Make netlist generates duplicate nets. (Users can scan the printed netlist (.NET) file to check for any duplications.) DRC produced a 24 page printout, 90% of all reported violations did not exist when the .PCB file was examined. Running Netlist Route Process Pre-routes or a DRC caused some quadrants of arcs on the Keepout layer to disappear from the screen. Edit arc confirmed that these quadrants are on but the display is impossible to restore without reloading the file. TRAXPLOT - version 1.61 (note: please see special supplement on Gerber plotting after this section) Automatic .TOL file generation (new feature) The .TOL file is a list of N/C drill tools, which are matched to the holes in pads or vias. Previously, you had to manually edit the .TOL file using a text editor. Now, a .TOL file can be automatically generated, using the holes defined in your .PCB file. You still have the option to assign any existing .TOL file. To use this feature: Select Setup/NC Drill, then choose the Method option. Select Generate. A tool assignment will be made for each hole in the PCB file with a defined size >0. The .TOL file will be given the same name as the .PCB file. If the SMD Single Layer Pad Holes option is 'ON', any SMD hole > 0 will also be assigned. Up to 64 unique hole sizes can be assigned. Metric .APT (aperture) files for Gerber plots You can use the same process for .APT files as for .TOL files to specify metric units. See page 33 of the Reference Supplement. Roland 1000 Series plotters A new plot driver has been added for these plotter models (DXY 1100, 1200, 1300, etc.). It is called ROLAND RD-GL I. This supersedes the information on page 28 of the Reference Supplement. However, you should make sure that all communications parameters are matched between the program and the plotter. Improved Path Handling in Traxplot When you select the Setup Plotter, Printer or PostScript Type, to choose a driver, a window opens allowing you to specify the directory. The default directory is now always the Traxplot home directory. Naming of output files: The name of the current .PCB file is automatically applied to output files, as when plotting to a filename (rather than directly to a port). The same procedure is applied to generated .TOL files, etc. Power and Ground (Plane) Enlargements The default circular area 'cleared' for pins passing through these special midlayers is derived from the associated pad size. If the pad is asymmetric, i.e. 50x80 Rectangular, the smaller dimension sets the default clearance, in this case a 25 mil radius from the hole center. If you increase the Enlargement by 10 mils, the radius would be 35 mils. If Gerber plotting, a Round 70 mil 'flash' aperture would match the cleared area. PostScript printing The following PostScript options are supported by the current version of the plot program: PS300A4 A4 sheet 300 dpi resolution PS300A3 A3 sheet 300 dpi resolution PS400A4 A4 sheet 400 dpi resolution PS600A4 A4 sheet 600 dpi resolution PS1200A4 A4 sheet 1200 dpi resolution PS1200A3 A3 sheet 1200 dpi resolution PSLINOA4 A4 sheet 1270 dpi Linotronic PSLINOA3 A3 sheet 1270 dpi Linotronic PS300B5 B5 sheet 300 dpi resolution PS300LT US letter 300 dpi resolution PS300LE US legal 300 dpi resolution PSA4GEN Generic 11x8 inch 300 dpi resolution PSA3GEN Generic 16x11 inch 300 dpi resolution QMS Drivers These drivers support the QMS (laser) printers when used in LaserJet (HP-PCL) emulation mode, rather than PostScript mode. REPORTED PLOT/PRINT PROBLEMS Prints don't fit properly on the sheet Printed output does not tile properly onto multiple pages. some pages have just small strips of output. These problems can have multiple causes, depending upon the target printer. In some cases, the print is not scaled to fit within the available print area between the device margins. In other cases, a primitive has been placed outside the apparent boundary of the board or the board has been created away from the 0,0 (lower left limit) origin of the workspace. Use Information Board Dimensions or Zoom All to verify the area to be printed. Traxplot calculates the print area based upon the difference between the absolute 0,0 coordinate and the highest x and y coordinate present in the file. If the board has been created away from the lower left corner, use the Block Move command to move all of the board close to the lower left corner of the available workspace. You may also need to try another scale for your print or printing without the Title block to fit on a particular page size. Sometimes data is missing between paneled pages (HP LaserJet and DeskJet). Suggest using alternate driver or changing print scale (as above). Traxplot does not recognize EMS from EMM386 (DOS 5.0), Traxedit works fine with DOS5. You may need to substitute another EMS driver with Traxplot. Traxplot will not generate a drill drawing legend when pen plots are rotated using Traxplot 1.61. If legends are required, you will have to use the non-rotated orientation. Mouse becomes inactive when ploting or printing to the same serial port as the mouse, even is the plot or print has been aborted. You may need to restart Traxplot. SMD pads with holes are not recognized on the PWR GND planes, Even with "Surface Mount Pad Holes" enabled. This is a limitation in the program. Rounding off problems with metric units. Example: Drill drawing table will show pad hole being 0.99mm, however pad hole was defined as 1.00mm in Traxedit. This is because dimension is stored in imperial units, to accuracy of 1 mil and has no effect on accuracy of tool assignments. Board dimensions given in the Information window do not match with Traxedit's Information Board Dimensions when boarder of PCB is offset from origin, EG. (1000, 1000). HP-GL driver. When ploting a rotated PCB, flipping a plot layer causes "top to bottom" flip, not a "side to side" flip as happens with a normal, (not rotated) plot. Postscript works fine. Solder Mask plots, unable to produce a plot without vias, vias are displayed even if the Options Vias is turned off. HPGL.DRV & RDGL-I.DRV - Ploting in draft mode, arcs are plotted in final quality. Final quality mode is not effected. Cannot control the Roland plotter pen speed, using RDGL-I driver. Setup Pens Plotter Pen Speed - has not effect. Unverified Traxplot problems: RDGL-I driver, using a DXY 1300 plotter. After plotting about 1 2 a PCB successfully in final plot mode, the plotter switches to draft mode, and completes the rest of the board. NEC 5200 and Epson LQ 500 printers. Epson 8" (72) driver works, but produces low resolution, distorted print. Epson 8" (216) and LQ 8" drivers produce a higher resolution print, but only do the first printing pass. HP laser jet plus series II. Little notches appear on printout where tracks are connected together. GERBER FILE GENERATION - Special Supplement Generating reliable Gerber files depends upon the user understanding some of the principles of the Gerber format. Please refer the Manual Supplement pages (front section of the manual) and also the chapters on Printing plotting and Gerber file generation. Once you understand the basic concepts, your photoplotting bureau is the best source of information. A good bureau will guide you in preparing your design for efficient, accurate plotting on their equipment. Some bureaus will be set-up to generate your Gerbers directly from your .PCB files, eliminating most of the risk and difficulty of doing the job yourself. In simplest terms, photoplotters paint your design on photographic film, using a beam of light. Two things are needed for the plotter to render finished artwork. A Gerber file that describes the plot using a special language (RS-274A) and an aperture file. It may be helpful to think of the aperture file as a set of paintbrushes of differing sizes, shapes and uses. Each "brush" can render a different shape on film, e.g. a 40 mil aperture with a "flash" use can be used to generate a 40 mil pad or via. If the "use" is "line" the aperture can be used to "stroke" a 40 mil (or wider) line. Line apertures can also be used to "paint" a solid fill. There are two basic types of photoplotter. A vector plotter uses fixed apertures (usually mounted on a wheel or slide) and operates like a pen plotter, stroking lines and flashing shapes (round or square pads, etc.). When targeting a vector plotter, you have to use an aperture table that matches the available apertures only. A raster plotter is more flexible, as it can synthesize the shapes described in the aperture table. Raster plotters scan the plot, similar to a raster video image. If your bureau uses a raster plotter, you can define a much wider array of apertures. This can allow you to generate more efficient, compact Gerber files that will generate and plot more quickly. In either case, you need to know the limits and any special requirements for the target plotter BEFORE you generate your plots. This special supplement provides numerous additional tips and insights regarding Gerber preparation. We strongly advise that you study this material in conjunction with the relevant Manual Supplement and Reference Manual sections. Contents of this supplement include: Part 1: APERTURE TABLES Part 2: SETTING UP FOR GERBER PLOTS Part 3: MATCHING DRAFT CODES Part 4: GERBER FILE FORMAT Part 1: APERTURE TABLES An "Aperture table" containing all Draft codes or "D" codes needed to photo-plot a design must be created. "D" codes are the exposure sizes that will be used to make films. All aperture tables must have the file extension ".APT". Autotrax comes with several sample aperture tables; before using any of these it is recommended that they first be checked to ensure all necessary apertures are included in a given table. If all needed apertures for a particular design are not found in any one of the tables provided, a custom table should be generated. The aperture files are ASCII text and therefore can be edited or generated from scratch very easily with most Text Editors or Word Processors. Be sure to follow the file format in the aperture tables provided with your package (see sample bellow). It is a good idea to check with the photo- plotting bureau to be certain that all the apertures in the table will be available. If not, make the proper substitutions. To avoid last minute changes in a design due to unavailability of certain apertures, it is best to design with manufacturing in mind! Each Aperture table can contain a maximum of 255 "D" codes; numbers D10 thorough D265 should be used. The following is a sample of an aperture file for Autotrax. Please note all comment lines start with a semi-colon (;) and no blank lines are allowed unless preceded by semi-colon (;). ; APERTURE FILE FORMAT ; ; ; ; EXPLANATION OF PARAMETERS ; ; Code assigned to this aperture, e.g. D14 ; Note that this code must start with 'D' ; followed by the code number. Code numbers ; 1 - 9 are not available. ; ; Can be any of the following shapes: ; CIRCULAR ; RECTANGULAR ; SQUARE ; OCTAGONAL ; ROUNDRECT ; CROSSHAIR ; MOIRE ; ; size of aperture in the x direction in ; mils (thous). ; ; size of aperture in the y direction in ; mils (thous). ; ; size of hole in aperture in mils (thous). ; zero if no hole in aperture. ; ; specifies the aperture user. ; There are three possible settings: ; LINE can only be used to draw lines ; FLASH can only be used to flash pads ; MULTI can be used for either, ; blank defaults to MULTI setting ; D10 CIRCULAR 4 4 0 LINE D11 CIRCULAR 100 100 0 LINE D12 CIRCULAR 13 13 0 D13 RECTANGULAR 20 20 0 D14 OCTAGONAL 50 50 0 FLASH D15 CIRCULAR 25 25 0 D16 ROUNDRECT 30 30 0 FLASH D17 CIRCULAR 62 62 0 D18 CIRCULAR 10 10 0 D19 CIRCULAR 40 40 10 D70 CROSSHAIR 500 500 0... Part 2: SETTING UP FOR GERBER PLOTS Please see AUTOTRAX manual, pages 161 - 170, for instructions on executing the Traxplot program, loading your .PCB file, etc. Once a .PCB file is loaded, options should be set up for Gerber file generation. Select Setup from the Main Plot Menu, then choose Gerber. Output File This setting defaults to your .PCB file path and name. If you would like to change either the path or the name of your output file(s), select the Output File option and type in the new information, then press . The file extensions Traxplot will use for Gerber files are as follows: Layer Plotted Gerber File Extension Top Layer .GTL Mid Layer 1 .GM1 Mid Layer 2 .GM2 Mid Layer 3 .GM3 Mid Layer 4 .GM4 Top Overlay .GTO Bottom Overlay .GBO Bottom Layer .GBL Power Plane .GPW Ground Plane .GGD Top Solder Mask .GTS Bottom Solder Mask .GBS Top Paste Mask .GTP Bottom Paste Mask .GBP Pad Master .GPM Keep Out Layer .GKO Drill Drawing .GDD Drill Guide .GDG Example: the resulting Gerber file generated for the Top Layer of a board called DEMO.PCB in the Autotrax directory, would be C:\AUTOTRAX\DEMO.GTL if all file defaults were left unchanged. X and Y Offset Offsets can be selected, in inches, for the X and or Y axis each time a plot is generated. Different offsets may be selected for the X and Y axis. Once chosen, offsets should be kept the same for all layers of a design for proper alignment. Aperture Table The proper Aperture table for the files about to be plotted must be selected. (See Part 1, "APERTURE TABLES"). Any Aperture tables in the Traxplot directory will automatically appear in the list to choose from when this option is selected. The path for aperture tables can also be changed at this point if the desired table is in a different directory. In some cases more than one Aperture table may be required to plot all the layers of a given board. If this is the case, the proper table should be selected in this menu before proceeding with the plot for each layer or set of layers. Match Oversize, Match Undersize These settings are the "margin of error" allowed the program for the draft code selection when the exact size aperture is not available. This variation is defined in mils. Example: The program is looking for a draft code to match a 62 mil circular pad. If you do not have a 62 circular draft code specified in the aperture table, and your Match Oversize is set to 3, the program can select a draft code of 65 mil circular to plot the pad. If this aperture appears in your table the program will select it automatically. For fine line boards, this should be set to 0 to avoid clearance violations or under sized copper. G54 command Some older Gerber plotters require that a G54 command is given before each aperture change. In most cases this should be set to OFF. Before generating Gerber files it is a good idea to find out from the bureau if G54 is required. Software Arcs and Arc Quality Some photo-plotters are capable of plotting a hardware arc while others require that arcs be drawn with a series of short line segments - this is called a software arc. If Software Arc is turned ON, the Arc Quality setting gives you control of the segment length used to draw arcs in your files. The shorter the line segment, the better the quality of the arcs and the larger the file. This setting is in mils, and the default is 5. If you decide to change this, select Arc Quality and you will be asked to enter the Chord Length. The minimum is 2 mils, and anything over ten is not recommended as the arcs become more like octagons. Options This is a sub menu and may be accessed from either this menu, the SETUP PLOTTER, SETUP PRINTER, or MAIN menu. Each contains the same set of options, some of which you may need to change for each plot. Select Options at this point. Type of Plot Select the layer to be plotted. If you choose Batch Mode to plot multiple layers, remember to go to the Setup Batch Mode menu and turn on the desired layers before you proceed with your plot. NOTE: The Check Plot option should not be used for Gerber plots, if a Gerber plot is attempted with this option the message "Cannot do Gerber CheckPlot" will appear, press the key to return to the MAIN menu. Board Layer This layer usually has the board outline on it, and should be left On if the outline is needed on the plot. Pads, Vias and Strings Each of these may be turned On or Off as needed. Default is On for all three. Title Block If the Title Block is turned on, it will appear in the lower left hand corner of the plot, and consist of the file name and the type of plot. The setting for the Title Block option should remain unchanged for each layer of a design since it does offset the plot if turned on. Single Layer Pad Holes This option is for pen plots only, and should always be set to Off when creating Gerber files. Pad Hole Guide Size This option is also designed for pen plots. This should be set to 0 when creating Gerber files. Drill Draw Symbol Size This settings allows the user to define the size of the symbols used in the Gerber drill drawing, in mils Solder Mask, Paste Mask, PWR GND Enlargement Clearances for pads and vias will be increased (in mils) when an enlargement is specified for any of these layers. All three can be set to different numbers. If no additional clearance is needed on Solder Mask, Paste Mask or Power Ground Planes, leave the setting at 0. Example: If additional clearance is needed for unconnected pins and vias on Power and Ground Planes, you can Specify 10 for PWR GND Enlargement. All 62 mil pads will plot 82 mils on these planes, all 50 mil vias would plot as 70 mil... The number specified will be the annular enlargement in mils on the plot. NOTE: "D" Codes must be provided in the Aperture table to match the sizes of your pads and vias after enlargement, as well as their original sizes. If three different enlargements are specified for the above layers, four "D" codes will be needed for each size pad and via in the PCB file. Tracks are not effected by these enlargements. All options should now be set correctly. Part 3: MATCHING DRAFT CODES To proceed, return to the Main menu, and select Gerber Plot. A window will appear at the top left of the screen to confirm Gerber plot No Yes, and one on the right side of your screen with information on current settings. This is an opportunity to check all options before proceeding with the plot. Select Yes if ready to proceed. NOTE: If Batch Mode is selected as the Type of Plot, all layers turned On in the Setup Batch Mode menu will be plotted with the same options settings. Therefore, if options must be changed for certain layers before they are plotted, these layers must be turned Off in the Setup Batch Mode and plotted individually as the correct options are set. At this point, several messages will be displayed which do not require user interaction - "Loading Gerber Driver" and "Preparing For Draft Match". These messages may go by too fast to read depending on the processor (8086, 80286...) and the size of the .PCB file about to be plotted. Matching Of Shapes - Automatic Manual The user may select Automatic or Manual. It is recommended to use the Automatic option unless the user needs the ability to assign particular items to apertures other than the exact match. Automatic If Automatic is selected, all items on the PCB will automatically be assigned to "D" codes from the aperture table which either match in shape and size exactly, or are within the allowed oversize or undersize. If a match is not found within the set guidelines the user will be prompted to select a match manually from the available apertures in the table. Manual This option will require that the user select a match for every shape in the PCB. This process allows complete control over the Gerber process; however, this can be a very lengthy procedure for a design with many different shapes and there is always more room for err with this method. Always Confirm Paint Match For Shape - No Yes A paint match would be used for a shape if an exact match was not found (see description of Flash, Stroke, and Paint below). Paint match is appropriate for large and or odd shapes which are not used many times in the PCB, but it may not be appropriate for a pad or via used a hundred or a thousand times or more in a design. Knowing when such a match has been made for a pad, via or track is very helpful in preventing an excessively large Gerber file; choosing Yes is recommended. Fill Perimeter Match - Automatic Manual If fills have been used in a design it is unlikely that an exact aperture exists for every fill - there could be hundreds of fills, each a different size. Choosing Automatic will allow the software to assign apertures for fills automatically, assigning these manually can be tedious. As explained in Part 1, APERTURE TABLES, the table should contain a "D" code for each size of pad, via, track and string line on your PCB. If this has been done and Automatic was selected for the Matching of Shapes option, the Matching Draft Codes process will automatically assign a "D" code for every shape found in the PCB. (completion times will vary with CPU speed, .PCB file size and number of layers being plotted). If a match is not found for a shape within the specified Match Oversize or Undersize, or if Manual was selected for the Matching of Shapes option, a window will pop up displaying a description of the item from the PCB database being matched [i.e. "Pad Circular (60 x 60)], and a second window displaying the closest "D" code matches found for that item for each of the plot methods. The aperture and plot method to be used must now be selected. There are three possible plot methods - Flash, Stroke and Paint. Flash Method This is primarily used for pads and vias when a single exposure of an aperture will create the desired image on film. This is the most efficient way of plotting pads and vias, therefore an exact match in the aperture table for pads and vias is preferable. If the Power and Ground planes are used in a design and there are pads relieved to the planes, the reliefs should be plotted with the Paint method, see below, using a ten mil circular aperture. Stroke Method This method is primarily used to draw tracks or text on the film. A 10 mil wide track would be "drawn" with a 10 x 10 circular aperture from the starting point of the track to the end point. The program will automatically select the Stroke method for tracks when it does find a match, and it is a good idea to use only this method when manually assigning tracks. The Stroke method also can be used when plotting Rectangular or Roundrectangular pads. This can be done when an aperture exists to match one dimension of the pad perfectly. Example: A Roundrectangular pad 120 by 50 mil is being plotted. There is no Roundrect 120 x 50 mils in the table, but there is a Circular 50 x 50. The 50 x 50 aperture should be assigned and the Stroke Method should be selected. This will basically draw the pad on the film in the same way tracks are drawn. The same could be done for a Rectangular pad of 120 x 50, using a 50 x 50 square aperture. NOTE: this is not the preferred way to plot pads, if at all possible an exact match should be in the aperture table for each pad type to allow the use of flashes for pads. Paint Method This method is used for creating shapes on the film that are non-standard or simply have no matching draft codes in the aperture table. The Paint Method will "Flash" and or "Stroke" the assigned draft code as many times as necessary to create the desired shape in the Gerber file. This method is very flexible, however, it is inefficient and tends to increase the size of Gerber files dramatically. Therefore, this method should only be selected manually when it is not possible to use the other two methods. An aperture is displayed next to each plot method; this is the shape and size that will be used to plot the item currently appearing in the top window. If an aperture other than the one displayed for a given plot method is needed, an alternate can be chosen from the table currently selected. To see a list of available apertures for any of the plot methods move the highlight bar to the desired plot method (choose the appropriate method for the shape being matched, i.e. Flash for pads, Stroke for tracks, etc.) and press . A third window will pop up displaying the list of available apertures. Move the highlight bar to the desired aperture and press . The selected aperture is now displayed next to the plot method. To select a plot method and allow the use of the aperture currently displayed next to that plot method to plot the current shape press the corresponding number key on the keyboard: <1> for Flash <2> for Stroke <3> for Paint This can also be done by moving the highlight bar to the appropriate choice and pressing . NOTE: This procedure will be repeated for every shape in the PCB if Manual was selected for the Matching of Shapes option. When all items in the PCB file have been paired with a draft code from the aperture table, a window will pop up displaying the message: Match File Generated [path and filename].MAT Press any key to continue The match file (.MAT) is an ASCII file, containing a complete list of all matches made by the program, and can be examined at DOS level. The Gerber file(s) will now be generated and saved to the hard disk using the path and filename defined under the Output File option (see above, Setting Up For Gerber Plots). Gerber File Format Each Gerber file is divided into blocks which are exactly 512 characters long. There are 510 characters of data followed by a carriage return character then a line feed character. Each block consists of a number of short Gerber records; each record is terminated by the asterisk (*). A block contains as many complete records as will fit into 510 characters. The remaining characters in each block (including the final block) are spaces (hex 20). The records may refer to an absolute location or a draft code which changes apertures. Thus a record might be: X800Y775* which instructs the plotter to move to a particular location; or D16* which instructs the plotter to select a different aperture. The particular draft codes vary according to the photo-plotter being used, but usually the following codes always have the same effect. Some modern plotters have a greater range of apertures available. D01 Turn the light source on. D02 Turn the light source off. D03 Flash the light source. D10-D19 Select apertures 1-10. D70-D71 Select apertures 11-12. D20-29 Select apertures 13-22 D72-73 Select apertures 23-24. On some older plotters the special code G54 needs to be sent before each change of aperture code. The last Gerber record is terminated by the special record M02*. After this block, there is one more block which contains the character hex 08, then 509 spaces, then a carriage return and a line feed. The following extract from a Gerber file shows the first and last blocks. Notice that on the first line, the draft code D16 selects a particular aperture and then D01 and D02 codes are then used to turn the light on and off at various locations on the film. Because there are no D03 records in the first block it is likely that the aperture is a line aperture used for drawing tracks. X0Y375*D16*X0Y125*D01*X60Y125*D02*X80Y145*D01*X60Y12 5*D02*X80Y225*D01*X80Y145*D02*X60Y245*D01*X80Y225*D02 *X0Y245*D01*X60Y245*D02*X20Y245*D01*X0Y245*D02*X20Y2 45*D01*X20Y125*D02*X120Y245*D01*X120Y125*D02*X120Y245 *D01*X200Y245*D02*X120Y245*D01*X200Y245*D02*X120Y245* D01*X120Y185*D02*D01*X160Y185*D02*X120Y185*D01*X160Y1 85*D02*X120Y185*D01*X120Y125*D02*D01*X200Y125*D02*X24 0Y245*D01*X240Y125*D02*X240Y245*D01*X280Y165*D02*X320 Y245*D01*X280Y165*D02*X320Y245*D01*X320Y125*D02*X360Y 245*D01*X360Y125*D02*X360Y245*D01* . . D03*X3075Y3950*D03*X3075Y4050*D03*X3075Y4150*D03*X3075 Y4250*D03*X3075Y4350*D03*X3075Y4450*D03*X3075Y4550*D03 *X3075Y4650*D03*X3075Y4750*D03*X3075Y4850*D03*X2650Y41 50*D03*X3075Y4950*D03*X3075Y5050*D03*X5575Y2650*D03*X5 125Y2350*D03*X5125Y2250*D03*X5125Y2150*D03*X5125Y2050* D03*X5125Y1950*D03*X5125Y1850*D03*X5125Y1750*D03*X5125 Y1650*D03*X5125Y1550*D03*X5125Y1450*D03*X5125Y1350*D03 *X5125Y1250*D03*X5125Y1150*D03*X5125Y1050*D03*X5575Y17 50*D03*D02*M02* Arc Quality and Gerber plot files If you are preparing Gerber files that include small 'Paint' matches forround primitives, you should select the Hardware Arcs option, if it is supported by the target photoplotter. If you need to use Gerber Software Arcs, then make sure that you set an Arc Quality of 5 mils or less (chord length). Arc Quality determines the number of strokes used to 'paint' any round primitives that are not exact matches with an available aperture.Too high of Arc Quality setting will result in inaccurate plots. Solder mask/Paste mask generation & Gerber plotting. When painting a rectangular pad with solder/paste mask enlargement factors,the program may calculate different X & Y enlargements around the pad. It is advised to check the generated Gerber plot files with a Gerber viewer, before sending the files off to be photoplotted by your bureau, alternatively you can manually flash these pads with an appropriate sized aperture. Example: - 8 mil Solder mask/Paste mask enlargement, Rectangular Pad 50*60mil. - If the pad is flashed with 66*76mil aperture, solder/paste mask is ok. - However if pad is painted with 50*50 aperture, solder/paste mask is 66*68. GERBER PROBLEMS The following are known problems which can occur during Gerber file generation. Many of these errors are rarely reported and can be the result of some unusual combination of events. Most of these can be avoided, if known. Remember, there are a great many variations in Gerber hardware and software, with a wide range of "acceptable" variations in the way the Gerber format is expressed. It is always recommended that you check Gerbers, using a viewing utility, prior to submitting the files to your bureau. This will allow you to catch (and correct) many human, as well as system errors which can creep into this complex process. Some bureaus will generate Gerbers directly from your .PCB files -- a safer option if your experience is limited. Vias on internal power plane layers flashed the wrong size. User's example file used 50 mil vias that were manually matched with 62 mil circular flash aperture on plane layers. Some vias are flashed correctly, others received a 50 mil flash instead. Program selects the first aperture in the table that lies within the tolerances. Even if it is not the closest match. (This will not cause plotting problems, but can result in a less efficient file). Fills are not painted accurately if rectangular apertures are used. (Restricting the use of rectangular apertures will allow you to avoid this problem.) Plane clearances incorrectly painted. User's example: 100 mil square pad with 10 mil enlargement. If 120 mil round aperture does not exist, Traxplot strokes 110 circular apt with 0 length resulting in undersized enlargement. (Can be avoided by providing an appropriate Flash match) Traxplot is generating hardware arcs (G02) with negative I and J commands. Gerber specs call for an absolute value for I and J commands. If this is a problem for a particular file (or bureau), user can specify software arcs when generating Gerbers. Drill drawing symbols and text in legend are automatically assigned the same aperture as tracks placed on board layer or targets. Therefore, using .020" tracks on board layer, to define the PCB outline or trim, will cause drill drawing symbols to be unreadable if symbol size is set to 50 mils or less. Workaround: use smaller tracks for outlines/targets or larger text size. Unverified Gerber errors The following errors have been reported, but not confirmed by Protel Technical Support staff: Gerber plot "paints" tracks, even if a Stroke match has been selected. e.g. 13 mil track would be painted 13 mil, even if a stroke match of 12 mil was manually selected. Hardware arcs, Gerber output is generating wrong D-codes for "end of arc". Inserts a G75 instead of G74. (This could be corrected in each file by a simple global edit of the Gerber ASCII text.) UTILITY PROGRAMS There are three new utility programs supplied with this upgrade (listed below). It is now possible to install these programs into a separate directory, or to skip this installation if the utility programs are not required. PCBTODXF File Translator (New) This program converts an AUTOTRAX PCB file to the AUTOCAD Drawing Interchange file (DXF) format. Please read the associated document file called PCBTODXF.DOC for further information. If primitives are hidden in the .PCB file, those primitives will be included in the .DXF (AutoCAD) file. To overcome this limitation, you will need to either un-hide, then delete these items in a temporary version of your .PCB file or delete hide these items in AutoCAD. 2NET Netlist Translators The 2NET program allows you to translate EDIF (OrCAD), SCHEMA and PADS-PCB format netlist files into Protel Netlist format. Please read the associated document file called 2NET.DOC for further information. NET2EDIF Netlist Translator (New) The NET2EDIF program allows you to translate Protel format netlist files into EDIF (OrCad), version 2.00 standard Netlist format. Please read the associated document file called NET2EDIF.DOC for further information. (end - rev 7.92be)