Help me open an old PCAD pcb file

Hi all,

I have to open a .pcb ascii file. It must be an old DOS PCAD file, since the file starts like this:

Personal CAD Systems, Inc.

PC-CARDS Database file version : 1.04

I tried several viewers and import tools, but no luck... Any ideas how to open this file? I do not want to be able to edit the file, just view it to verify the design.

Thanks

pcad pcb

Convert DOS PCAD files to Windows PCAD files
PCB and SCH files can be read into Accel EDA/PCAD 2000 .as is. but to have the intelligence shared between them and in order to make changes, you need to follow these steps to get them into true Accel EDA/PCAD 2000 form.


1. In the PCAD Library Management module, create a library1.slb file containing your .syms (symbols) and create a library 2.plb containing your .prts (parts).

2. In the PCAD PCB module, run PDIF Writer and create PDFs for your library1.slb and library2.plb. Make sure that you have selected the Indented option and set the Scan Reserved Characters option before you create the files.

3. Open Accel Library Manager. Go to the Library pull down and select translate. For the Source file format, select PDIF. Click on the Source Library button and select library1.slb. Click on the Destination Library button and enter library1 for your new library name. If you used a PCAD cross reference file to define power and heterogeneous gate information, then you will need to click on the PDIF Cross Reference button and select the file. (If you defined your power using the PWGD attribute on the gate and if you have only homogeneous components, you do not need to worry about a cross reference file.) Click on the Translate button at the bottom. Next you will get a dialog box asking about layer mapping. Unless you used some custom layers, you can click on the OK button to accept the default. Translating will continue and you will be given the option to view the log file at the end. I would recommend doing this and maybe even printing it out if you have a lot of errors.FYI- it will flag power pins as duplicates if you used the PWGD attribute on your gates. This is because it is reading the attribute for EACH gate. Technically, this is not an problem just Accel flagging something it thinks is wrong. Follow the same steps to translate your library2.plb file. When you translate your .plb, it is possible that you will get a warning that looks like: Warning: The number of components pins created for AD637 does not match the number of PIN_DEF entries near line 176. Power pins might be missing. Again, this is Accel flagging something that it thinks is a problem.

4. Once you have your two files translated, it is now time to merge them. From the Library pull down, select Merge Patterns. For your destination library, select your library1.lib file. For your source library, select your library2.lib file. Now, click on Merge. When it is done, it will kick up a log file of problems. Print this out and use it to clean up your newly created library of components. I would recommend going through your entire library to verify that everything translated correctly. An important thing to note, when you translate your patterns or footprints, it will create padstyles for your through hole components that are 60 mil round pads with no holes. Surface mount pads translate correctly so no need to worry about them. For your through hole components, you have two options, one- modify and rename the padstyles or two- leave it be and fix your pads in the PCB editor.

5. Now that the hard part is over, it's time to bring in and clean up the schematic & PCB AND get the two to agree. First, open the Accel EDA Schematic editor. In Library Setup, make sure to specify the library file you created above. Open your PCAD schematic file. (If you used a PCAD Cross Reference file, specify that during the opening of the file.) Once the file opens, do the following: Delete all the PRT and PWGD attributes; turn off the pin numbers on the discretes; correct any font problems and clean up your power rails. (You may also want to cut & paste it onto a current format.) If you are converting a multi sheet schematic from PCAD, open your first sheet, create any additional sheets using the Options, Sheets. Then open your other PCAD schematics and add them to the Sheet one file using the Cut & Paste options. Once cleanup is complete, generate a netlist.

6. Open the Accel EDA PCB editor, and got to Library setup. Clear what's there and set it to your library file. Now, open your PCAD PCB file. Select Embedded Aperture Table in the Convert Pad Definitions box. (This will create padstyles for your through hole components that are all defined as 60 mil round with a 38 mil hole. If you select Create from Pad graphics, unless you have created absolutely dead on pad graphics, you will get odd size padstyles. Selecting the Embedded Aperture option tends to be a lot less clean up.) If you specified a PCAD Cross reference file in step three above, you will need to do it here also. Click OK to continue reading in your file. Once complete, view & print out your log file and correct any real errors there.

7. Open up one of the format files and cut & paste your PCB into it. Save your file as a new name and close the old PCB file without saving it.

8. Clean up the PCB file by doing the following: Delete all the component names from the Silkscreen and Top Assembly layers; Fix the padstyle definitions; Verify font style for reference designators; Update drawing format to contain the same information contained on the existing drawings(fab and assembly). The fab drawing can be quite helpful while fixing the padstyles as it contains the hole size information. If there are numerous unfilled copper pour areas on the top and bottom layers, review them to see what net they are assigned to and if they are all part of the same net, such as ground, create one large copper pour that encompasses the area occupied by the smaller pours. Delete the numerous smaller pours and the straps that are there. Assign the copper pour to the appropriate net and pour it. Verify that it is as it should be by comparing it to the hard copy of that layer.

9. Run a Compare between the two netlists (Schematic & PCB). Fix any errors or warnings that you can and continue this process until the two match with no errors and no warnings (if possible).

p cad pcb

it was really worth information. Can you upload any detailed PDF?

accel schematic to pcad

sorry,i dont have other files about this topic.

*.pcb file

Wow, thanks for the info! But all that is provided that I will be able to open the file.

I had tried PCAD 2004 with no success, and now I am on to PCAD 2000