Allowing Swapping Pins on the FPGA in Capture 17.2 Hotfix 57

You are using the later Part / Symbol Editor version, look on the right hand side of the screen for the Property editing sheet, Edit Pins and the Pin Group column is probably what you need.

Hi oldmouldy

Thanks for your quick reply.

I did what you suggested and when I assigned -1 to pins which I didn't want to be swappable, the software threw an error that 'Pin Group may only be defined as an integer from 0 to 126. ERROR(ORCAP-5049)'.

Do you know the solution to it?

Regards

Atin

I don't think that "-1" was mentioned anywhere for the Pins that you don't want to swap. The Pin Group value for the Pins that you don't want to swap should be "empty", no value assigned, in the Library Part.

Aaaah, right I was mixing earlier practice with the current practice. Thanks so much oldmouldy.

I've modified the -1's to blanks. When my layout engineer does the layout, I'll get to know if I did it right.

Regards

Atin

How are you backannotating the pin swaps? By hand, or automation? I've been trying to figure out how to backannotate pinswaps to a multi-section symbol. At the moment I have a clean way of "easily" moving the offpage connections around on the swapped part, but it's still tedious.

There should be no need to touch the schematic as the backannotation process works on all part types.  Yes, it moves the pins on the symbol but no need to move offpage connections.  Did I miss something in your comment or are you trying out something unusual?

Unfortunately my schematic looks like this, and is one of 10 180-pin headers. The engineer doesn't want the Slot ID (e.g. S15_DP_000) moved. So I can't just backannotate the pin numbers, since that would re-arrange the symbols.

Unfortunately my schematic looks like this, and is one of 10 180-pin headers. The engineer doesn't want the Slot ID (e.g. S15_DP_000) moved. So I can't just backannotate the pin numbers, since that would re-arrange the symbols.

Ok, I get that.  That becomes a "beautification" task when the task at hand is to get the layout done properly.  Best to address while the board is in fabrication when there's downtime.

When this particular case needs to be addressed, we complete the layout and then do a manual rearrangement so the schematic is pretty -- which does count for a lot, I get it.

I just disconnect the offpage conns by selecting with ALT key applied so I can move them away, update the symbol with the original pins,  and then chisel away at moving the off-page connectors back to the correct location.

Try building the connector next time as a homogeneous part and then make a symbol that is a single pin equivalent in height.  You can then stack the "slices" on top of each other and get something very reasonable looking.  That's another topic for another thread...