Protel for Windows PCB Design System Version 1.5 - Readme text file This file covers the following products: Protel for Windows PCB design, plus Advanced PCB option; Advanced Place option; Advanced Route option. Note: When using this README file, please refer also to your Reference Manual, Reference Supplement booklet and to the On-line Help system. We recommend that you make a hard copy print of this file for convenient use. ---------------------------------------------------------------------------- Copyright Notice Software, documentation and related materials: Copyright (c) 1992-93 Protel Technology Inc Copyright (c) 1991-92 Protel Technology Pty Ltd All rights reserved. ---------------------------------------------------------------------------- The following files have been installed onto your destination drive and directory which was supplied during installation: PFW.EXE - Protel for Windows application PFW.HLP - On-line help file PFW.LIB - component pattern (footprint) library file PFW.XRF - component type to pattern (footprint) cross reference PFW.PAD - Pad Type File DEMO1.PCB - Unrouted small demonstration PCB file DEMO2.PCB - Unrouted large demonstration PCB file RDEMO1AP.PCB - Routed autoplaced small demonstration PCB file RDEMO2AP.PCB - Routed autiplaced large demonstration PCB file DEMO1.NET - Netlist file for small demonstration PCB file DEMO2.NET - Netlist file for large demonstration PCB file README.TXT - this text file Following is a list of features and commands that have changed since the Reference Manual and Reference Supplement were printed. CHANGES FOR VERSION 1.5 Software Protection system If upgrading from an earlier version, please note that PCB version 1.5 uses the same access codes as your previous installation. 32-bit design system Version 1.5 provides full 32-bit design and database support at all levels. System resolution is now .001 mil (0.000001 inch). All dimensions are stored and calculated to .001 mil. All user-definable dimensions, e.g. grid or track width, can be defined to .001 mil. All database coordinates and dimensions are stored in the numeric format: "000000.000mils" and metric units are now stored in the format "00000.00000mm". Boards can now be up to 100x100 inches or 2540mm square. This feature is evident at several levels when using the software. For example, the Status line now displays coordinates from 0-100000.000 mils or 0-2540.00000mm with the unit of measure (mils or mm) displayed. Fractional (.001 mil) definitions can be applied to track widths, grid, routing grids, pad size, etc. Please refer to the routing models on 202-204 of the Reference Manual for examples of the ways in which fractional grids can be applied to specific routing problems. A new shortcut for toggling between metric and imperial units has been provided. Press the "Q" key to change the measurement system, which will be reflected on the Status Line coordinate display. Improved Copper Pour (Polygon Planes) New options allow you to easily remove (Edit Delete Polygon) or change (Edit Repour Polygon) copper pours. This is especially useful when you wish to place an item inside an existing polygon. For example to place a track through a polygon, just place the track across the existing copper, select the polygon then choose the Edit Repour Polygon command. The Place Polygon dialog box opens and you can change any of its attributes (e.g. polygon grid or track width). The polygon will then be re-poured around any new items on its layer. On-line DRC As you manually place or move any primitive, Protel for Windows will check for clearance violations based upon user-defined settings (Netlist - Clearances command). When moving or placing an item, that item (and at least one colliding item) will highlight when the minimum airgap is crossed, assuming that the primitives are associated with nets that have different names. If the net names are the same, or if the net name is "nil", no violation is detected. Moving "offending" items outside the minimum airgap will reset (hide) the highlight. Pen Plotting A new Plot command (for pen plotting) has been added to the File menu, which by-passes the Windows plot drivers (and their associated problems). We recommend that you use this option if you are plotting to a vector pen plotter. To use this new plot routine, choose the File-Plot command. When this command is chosen, a dialog box opens, presenting the plot options. These routines support the HPGL (Hewlett Packard) and DMPL (Houson Instruments) plot languanges which are compatible with many plotter types. The generic use of these plot languages will be compatible with most plotter models that support these languages, although some specific features may not be available for a particular model. Setting up your plotter to support one of the available languages may be necessary. Consult your plotter documentation for details. It is also possible to plot via the File-Print command, if your device is properly supported by the available Windows plotter drivers. User Interface changes The user interface of the software has been updated and no longer matches many of the illustrations in the Reference Manual and Reference Supplement. However, he function and use of these features have not changed, except as documented in this file. The Toolbar has been re-designed and now includes buttons for 23 commands. When the cursor moves over a tool button, its function is displayed on the Status Line at the bottom of the workspace window. Dialog boxes have also been updated and we have re-designed the Status bar to include the Layer Manager button and layer name / color. This allows the toolbar to be "hidden" without losing access to the Layer Manager. A new color palette system has been included in this version, which now provides over 240 pre-defined colors. If you have 8-bit or 24-bit color graphics, a wide range of solid color values will be displayed by this system. This system by-passes the standard Windows Palette Manager, but is fully compatible with other applications which use the Palette Manager. PROTEL FOR WINDOWS - ADVANCED SCHEMATIC A number of special features and "links" have been provided to enhance the interoperability of Advanced Schematic and the Protel for Windows - PCB layout system: ReAnnotation and BackAnnotation ReAnnotation refers to re-labeling the component designators, based upon their physical location in the PCB layout. BackAnnotation refers to updating schematic sheet file component labels, based upon changes in the PCB layout ReAnnotaton of the PCB: Version 1.5 adds a ReAnnotate command to the File menu. When you choose this command, a dialog box opens. Three methods of reannotation are available: X then Y - updates left-to-right starting from the top-left component; Y then X - updates top-to-bottom starting from the left side; Name from Position - re-names components with abbreviated coordinates, derived from the position of the component reference (usually the center of pad # 1. In other words, a coordinate of 1500x3900 would result in a designator of "U015_039". When you use this command a ".WAS" file is generated. Advanced Schematic uses this file to Backannotate (File menu) the schematic sheet. Cross Probing of the PCB and the Schematic: Cross Probing refers to on-line "links" between PfW PCB and Advanced Schematic. These links are available when running the two packages with a circuit design (sheet or project) and board layout file open at the same time. Options include: Cross Probe PCB - this Schematic command cross probes from a schematic part to a PCB component footprint; Cross Probe Net - this command cross probes between a schematic net label and a PCB (physical) net. The PCB net is highlighted. PCAD files Most PCAD files can now be loaded directly, using the File Open command. The translator works transparently on PDIF 5 and 6 format files. Some limits are imposed on handling pad stacks - because PfW uses a single pad description for the Multi layer. If the PCAD file pad is described as multi-layer, no special handling is neccessary. If the stack includes a Top layer and Bottom layer pad, the Top layer pad shape is assigned to the PfW Multi layer. Hardlock .CDE files In previous versions of Protel for Windows the access codes for each software module were stored in a file called PFW.CDE located in the Windows directory. In version 1.12/1.5 this file will be identified by the Protel for Windows serial number, e.g. S1000999.CDE, etc. This system allows the access codes for each license to be kept either on the server's Windows directory, or on the node's Windows directory. By having multiple .CDE files in the Windows directory allows the use of different hardlock licenses on the same machine, without having to rename and copy the individual PFW.CDE files. Modifications to Report Generation When you choose the File Report command, or click the Report button from the Library Components dialog box, or load a netlist, you will be presented with two options for the report format: The first is standard Protel output and the second is in the CSV output. CSV stands for Comma Separated Values. This is a file format that can be loaded into most spreadsheets and databases. Both options generate reports in ASCII text format. For example Microsoft Excel will open a CSV format text file, when the Text option in the File Open dialog box is selected. Change the Column Delimiter Value option in the dialog box to "Comma". Hot key shortcuts for Auto pan and Zoom If you are using Auto pan (for example, while dragging a component), holding down the shift key will pan the display at 4X the normal rate. When using Pgup and Pgdn to zoom, holding down the shift key will zoom at .1 unit the normal rate (slow zoom). Net status in Change (primitive) commands When editing a track, a via, pad, fill, or arc, the name of the associated net (if any) will be displayed in the dialog box title bar. Using "File/Gerber/Gerber In" and "File/Gerber/Batch Load" (Advanced PCB) The "File/Gerber/Gerber In" and "File/Gerber/Batch Load" commands do not incorporate file integrity checking (see the Protel for Windows Version 1.1 reference Supplement). This enables Gerber files to be viewed without modification. However this may lead to difficulties if non Protel for Windows Gerber files are saved without taking a few precautions. If the workspace appears empty after opening a Gerber file, the data may exist beyond the legal boundaries). This situation can be confirmed by viewing the "PCB Information" dialog box (Choose "Info/Board Status..."). "Board Dimensions" beyond the 0 to 99999.900 range and quantities greater than zero for "Physical Items on PCB" are indications that data exists beyond the workspace boundaries. Data can be moved within the boarders of the workspace by using the following method: Choose "Edit/Select/All". Choose "Edit/Move/Move Selection". Select a Reference Point near the upper right corner of the workspace. Place the selection near the lower right corner. If this procedure was successful the screen will redraw with the data in view. If not, try moving the selection in another direction. When this is complete, save the document using the text format then open this file. Integrity checking will take place as the text format file is opened. Integrity checking ensures that invalid data can not cause application or system errors. Automatic aperture file generation If Protel for Windows is used to automatically generate an aperture table, this should be done after setting all output options and Gerber setup parameters. Mirroring Gerber Layers Currently in version 1.12 the rounded ends of tracks and pads are painted incorrectly if the layer is mirrored by using the output options, layer mirroring command. To mirror a layer use the select inside area command and move selection. When moving the selection press the 'X' key on the keyboard to flip or mirror the pcb. Once your design has been flipped then proceed to Gerber Out the desired layer(s). Note: the problem only occurs if the tracks or pads are painted with a smaller sized aperture. Example 1: 50mil track, painted with a 10mil aperture will cause the ends of the track to be painted incorrectly. Example 2: 50mil track, stroked with a 50mil aperture, the track ends will be stroked correctly. Gerber layer naming conventions The following extensions are automatically used when generating Gerber files. The format is .GTL (for the top layer, etc): Top (component side) layer .GTL Mid (signal) layers 1-14 .G1 (-14) Bottom (solder side) layer .GBL Top Overlay (silkscreen) .GTO Bottom Overlay (silkscreen) .GBO Top Paste mask layer .GTP Bottom Paste mask layer .GBP Top Solder mask layer .GTS Bottom Solder mask layer .GBS Internal Power Planes 1-4 .GP1 (2,3,4) Drill Guide Top/Bottom pair .GG1 Drill Guide Top/Mid1 pair .GG2 Drill Guide Mid2/Mid3 pair .GG3 Drill Guide Mid4/Mid5 pair .GG4 Drill Guide Mid6/Mid7 pair .GG5 Drill Guide Mid8/Mid9 pair .GG6 Drill Guide Mid10/Mid11 pair .GG7 Drill Guide Mid12/Mid13 pair .GG8 Drill Guide Mid14/Bottom pair .GG9 Keep Out layer .GKO Mechanical (fab & assy) layers 1-4 .GM1 (2,3,4) Drill Drawing Top/Bottom pair .GD1 Drill Drawing Top/Mid1 pair .GD2 Drill Drawing Mid2/Mid3 pair .GD3 Drill Drawing Mid4/Mid5 pair .GD4 Drill Drawing Mid6/Mid7 pair .GD5 Drill Drawing Mid8/Mid9 pair .GD6 Drill Drawing Mid10/Mid11 pair .GD7 Drill Drawing Mid12/Mid13 pair .GD8 Drill Drawing Mid14/Bottom pair .GD9 Pad Master .GPM Autotrax Moire and Target pad and aperture types If you load and Autotrax board which has a moire or target pad then these pads will be converted to free primitives of arcs and tracks. These items will be painted when generating Gerber plots and not be converted back into special moire or target apertures. Loading of library and pad files When PFW is started, the library files PFW.PAD (containing pad descriptions) and PFW.LIB (standard footprint library) are automatically loaded. You can re-name a custom library as PFW, and this will become the (automatically loaded) default. Thermal Reliefs Thermal reliefs on PFW are drawn with the gaps in the arcs at 45 degree angles rather then horizontal and vertically. Unless you are using 45 degree oriented components, this will keep gaps as isolated as possible from one pad to the next. Manual routing If you use the Auto Manual Route command, the size of the tracks and vias used will be those set in the Auto Setup Auto Route dialog box, not the settings in the Current menu. You can backtrack from the current routed position by pressing the backspace as you route. Each press of backspace will remove one segment, restoring the ratsnest for that connection. Pre-Router pass This pass now recognizes and properly handles partially routed nets. Previous versions would route over completed connections because the Pre-Router could not re-optimize the connections in partially routed nets. Router improvments (Advanced Route v 1.5) Advanced route features significant improvement when routing SMD or single sided boards. Fractional grids are now supported. User can specify grids of x.75, x.67, x.50, x.33 and x.25 in the Setup AutoRoute dialog box. You can type other fractional values, but these will be automatically rounded-off to the nearest available value (as listed above). See page 202 of the Reference Manual for details. Hint: Maze Router pass will run faster is the routing grid is always equal to (or greater then) the routing track width + clearance. Notes on Unrouting (Advanced PCB) You cannot use the Auto Un-route command to remove placed tracks from the board unless they were routed from the current netlist (routed using the autorouter or Auto Manual Route command). If you load Autotrax boards, they cannot be unrouted, there is not sufficient information in the Autotrax file format to enable this to occur. If you wish to unroute all of the tracks and vias on an Autotrax board, use the Auto Unroute All command which will turn all of the connections on the board to unrouted, then use the Select commands to delete all the free primitives. Route priority The route priority field (part of the attached netlist portion of a .PCB file) is now implemented in this version of PFW. You can set the priority from the Netlist Edit Net command. You can view .PCB files after saving them using the Protel Text format option (Save; Save As... command). Loading PADS-PCB files Users may experience problems loading some PADS-PCB files. This is due to ambiguities in the .ASC format that cannot be resolved by Protel for Windows. For example, Protel for Windows cannot translate PAD-PCB files that contain numeric net labels of four or less characters, because there is no inherent identification of these strings as net labels. PADS-PCB provides the user with many options when generating files in PADS .ASC format. Some of these options may yield a file that is incomplete or otherwise unreadable to Protel for Windows. If you experience difficulty in loading PADS-PCB files, try re- generating the file using the PADS default (include all) output options. Problems can also occur when PADS 2000 files are imported into PADS-PCB, then re-exported in .ASC format, then loaded into PfW. rev 3/93 (end)