Allegro changing/editing footprints in the board editor on the fly. ? can it be done 

Hi guys and a happy new year. In the older layout product there was an option to "Allow Editing of Footprints" in the layout tool. With this option checked a user could have a footprint in Layout and then on the fly while routing a board move the positions of pads/silkscreen etc while still retaining net information from the corresponding symbol in capture.

Is there a way to do the same in "Allegro/Orcad PCB" ?

Or any possible work-arounds to accomplish moving pins in a packaged symbol when laying out a board.

Thanks Scott. 

When I had to use PADS against my will, layout ECO changes were cool until they vanish the next time the schemo is merged.

 After changing the footprint on the fly, won't that change the part number on the BOM?

I understand that in really dense designs, a smaller footprint is needed.

Gate/pin swapping is a better approach to keep the schematic accurate across design spins. 

Silkscreen clipping needs to be done in CAM.  If it can be done in layout, great.  But, in Cam, silkscreen clips match future design changes.

Hi Robert

In the old Layout tool if you had a footprint on the board you could click on a pin of that footprint or the silk etc and simply move it. You are not really changing the footprint but simply editing it as you would do if you were creating a footprint.

I  agree this can lead to problems if care is not used and typically I rarely used this feature in Layout but for some things it was handy if a pin just needed to be nudged one way or the other. Saved the time of re-creating the footprint.

Part of my reason for asking about this is in Capture I have a symbol for a coax cable. Now making the footprint for this is kind of difficult as the coax cable will be formed on the board in a sudo S circular way. What I would love to be able to do is have my coax symbol that has 4 pins in capture but on the layout side of things have those 4 pins as individual pads that can be moved but still retain the net info from the schematic.

It is kind of a mechanical issue, I am just trying to find the best way to represent that coax in a footprint. The hard part is if you create a footprint that has pins that are 4" apart you kind of got a issue as your footprint becomes huge. I think what I am after cant really be done from the perspective of a footprint but am certainly open to ideas

Thanks Scott

As long as you are not changing the number of electrical pins then yes, there is a simple method: edit->properties

select the symbol on the board, check the property "Unfixed Pins", and apply

Now you can edit->move, find pins, and happily reposition the pins for that symbol.  Does not affect library.

Hi Red

That works like a champ, thanks for the tip : )

 Scott