Odd shaped pads

I'm not quite familiar with what Layout does. Allegro uses shape symbols (.ssm) for any custom/irregular shapes that will be used in a pad stack. A rough outline of the implementation:

1. Create the custom/irregular shape, as a shape symbol, in the drawing editor. For most cases the shape should be on etch/top and the origin of the drawing (0,0) needs to reside within the shape extents. Note: Allegro only allows one shape in the pad shape drawing.

2. Create the pad stack using the shape with the following:

o Regular pad geometry: = shape
o Shape: = shape you created in step 1

3. Create your package symbol using the pad stack created in step 2

It may be that you just need to create the shape and the pad stack and then replace the pad stacks in your translated part.

Trykon is 100% correct on the way irregular shaped pads are handled in Allegro and it is the preferred way of defining the symbols. If you don't do it this way they you will have manually draw shapes for solder mask reliefs an solder paste apertures for each pad location which would be a pain.

As a side note, If you define copper shapes inside of the symbol file .dra you will always see DRC markers between the pin padstacks and the shapes areas because there is no netlist present inside of the symbol file. Once you place the symbol in Allegro layout .brd it will automatically associate the copper shapes to the net name of component pin it overlaps as long as the shape overlaps the center of the pin. (of course if a netlist is present.)

Hope this helps,
Mike Catrambone
UTStarcom, Inc.