I'm trying to organise to output a drawing showing the pin numbers on the pads of a device that is placed on a board. I'd also like to show the net names as well (you know, like when you zoom in enough on your pcb & you can see it).
To my knowledge, no version of Protel creates plot or print outputs showing pad numbers or nets. These are display options only.
However, it would not be difficult to generate the information as text on a mechanical layer, which could then be printed; with appropriate choices of size (on the layer) and, in the print definitions, layer priority and color, the text would always be readable.
I'll describe a manual procedure in rough outline:
1. Place a piece of text with the desired size of text on the mechanical layer you want to use. Use a distinctive piece of text so you can search and find it in your spreadsheet or text editor.
2. Save the PCB file as ASCII and, if necessary, export it.
3. Open the PCB file in Excel or other spreadsheet, using | as the field separator.
4. Extract all pad and net records. As I recall, nets are identified by number in pad records, then net records associate the number with the name.
5. Extract the sample text record you created in step one.
6. Copy the text record as necessary so that there are twice as many new text records as there are pad records.
7. Copy the pad locations and pin numbers from the set of pad records to the first half of the set of created text records, into the appropriate fields.
8. Copy the pad locations and net numbers from the set of pad records to the second half of the set of created text records.
9. Sort the text records with net numbers by net number and use techniques I won't describe here to find and copy the net names over the net numbers. (This is the only complicated part of the procedure, it will take some skill with a spreadsheet to do it; I don't have the exact method off the top of my head, I just know it can be done because I've done this kind of thing in the past with Excel.)
10. Offset the pad locations for the net numbers by an appropriate value so that the pad nets will not be on top of the pad numbers, but rather raised or lowered according to text size. (I do this kind of thing by creating a new spreadsheet column with a formula to add the offset, then copying and Paste-Specialing the new values over the former ones, then the extra column is deleted.)
11. Insert the created text records into the ASCII PCB file. (This may require massaging a dump of the spreadsheet records from tab delimited text as dumped to pipe-delimited ["|"] as needed by Protel.)
12. Reload the PCB file into Protel. If there is data in the binary file form that is lost by export to ASCII, then copy and paste the new mech layer from the imported file to the original file.
This extraction and insertion process could easily be automated; just because I know the language well, I'd use QuickBasic. Step 9, a tad complex in Excel, would be easy with a QuickBasic program.
Programs like this could be developed by the user community... But Altium could, of course, also easily create a tool to do it within DXP. The layer, text size, selection of pad name and/or pad net, orientation, and offset would be options in the tool.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *