Ali,
I'm pretty sure that is correct.
In order to swap a pin with allegro, the pins have to be part of the same
ref-des,
AND they must be part of the same schematic symbol (if the part is
fractured into multiple symbols)
Allegro is looking at the pstchips.dat file for the part to determine what
is swappable.
I am pretty sure they must be the same pin-type too...
when we build the schematic symbols for an fpga with pin swapping enabled,
we make sure to override the pintypes to inout.
I think the reason for this is so that allegro can feedback the pin-swaps
to the symbols in the schematic tool. It would be very difficult to do that
across reference designators and across schematic symbols. (because nets
would have to move)
I think there might be a way around some of those limitations with the
dalTools addon, but you would be responsible for fixing
the schematic side once you made the swaps
We have always bypassed the automatic feedback step. We would generate a
swap report between the pre-swapped netlist and the post-swap netlist and
then update the symbols based on the changes we find in there. (We have not
swapped between ref-des in those cases)
Thanks,
Bill
Bill O'Leary
Founder/Lead Developer
CadEnhance EDA Productivity Tools
(214) 280-8804
*-Your EDA Tools.... @The Speed of CadEnhance*
www.CadEnhance.com <http://www.cadenhance.com/>
On Mon, Mar 20, 2017 at 5:59 AM, Ali <dmarc-noreply@xxxxxxxxxxxxx> wrote:
Hi Group,
I read about pin swapping in Allegro by defining pin group in Orcad. My
question is if we have two instances of connectors say J1 and J2, is it
possible to swap pins between two different reference designators?
I tried in Allegro and got below message
Pins must be on the same gate in order to swap them ... pick again.
