Mechanical pins disappear after ECO on translated board

In OrCAD Layout all pins had pin numbers, mechanical pins were flagged with "not in netlist". In PCB Editor, pins with pin numbers are connect pins and must be included in the netlist, you don't have the mounting holes in the netlist, so they get deleted from the design. Use File>Export>Libraries, dump all the symbols into a "symbols" directory under the board file location - this keeps things neat and "symbols" beneath the design directory is part of the default symbol search path. Open the DRA for the mounting hole in PCB Editor, set only the Pin Number subclass visible and delete the text, this will now be a mechanical pin. In Setup, Design Parameters, Design tab, change the drawing type to Mechanical and save the symbol "as" to get a new name. Open the board, go to Place>Manually,in Advanced, select Library, in Placement List, pick Mechanical symbols and pick the new symbol from the list, place the symbols "somewhere" in the canvas, right-click>Done to end. Then use Place>Swap>Components, click on the original Mounting hole location and on the "new" symbol to swap their locations, the "old" mounting holes will disappear when the netlist is loaded.

You will have to remove the symbol from the board and then add the new mechanical symbol in again. Because the symbol typw has changed from package symbol to mechanical symbol PCB Editor won't like this. Once the symbol is in the board file as a mechanical symbol you will be able to run your ECO (File - Import) successfully.

Thanks oldmoudy!  You are the Man!

I have one question though: I followed all your instructions and it worked, no problem.  Howver, I am wondering what to do with the reference designator text.  What should I do about that?  I tried to edit the text but got the error "E- (SPMHA1-502): Can't change the refdes of an unassigned component.".  I tried to assign the reference designator and got: "E- (SPMHGE-30): Refdes was not found."

OK, so I thought.  Maybe I don't actually have to do this.  Maybe it serves no purpose to have a reference designator for a mounting hole since it isn't actually a part.  So, I tried deleting the reference designator text altogether.  PCB Editor didn't complain and the mounting hole is preserved at subsequent import logic.

So my question is: Is this OK?  Will there be any problems?

Hi steve,

 Thanks for your input.  That is pretty well what I ended up doing before I got the reply from oldmouldy.

However, before he replied, I didn't know how to change the symbol type from "package" to "mechanical" via the setup menu so instead I just re-created the symbol all over again as a mechanical symbol, recorded the locations of the old symbols in the board file and placed new mechanical symbols in those locations (the only thing I didn't need to re-invent was the padstack itself).

I'd certainly like to get this stuff right for the next translation I have to do - I have a whole bunch of designs to translate from Layout to Allegro.

Thanks again.

Cheers,

Allan

Apologies, I overlooked the RefDes placeholder, you can safely remove this, probably best if you delete this in the Package Symbol, but deleting it in the design won't cause any issues.

Take a look at the supplied "MTG" parts, in the share\pcb\pcb-lib\symbols directory of the installaton, they have no RefDes placeholders.