Copper over footprint pins

You can create odd shaped pads using Allegro. Use File - New - Shape symbol (ssm) and design your shape with copper. Save the file then use Pad Designer to build your padstack. When you go to pick the pad shape use Shape instead of Circle or Square and then browse to your shape (ssm) file. Then add pins as you would normally.

There is a property that can be applied to symbols that effectively says nodrc_sym_same_pin which when applied will no give pin-pin drc's on that footprint. This may also help.

 Add the SMT pins.  Add a shape to the symbol that encompasses the pins. (you will need two shapes...)

Build the schematic symbol such that the pins get the correct net name.

The shape will take on the net name when it comes into the board.

Be sure to consider the paste / soldermask you will need for the shape.

If you get stuck post a zip with your schematic symbol and Allegro symbol...

Hi

There's a little trick to doing paste and soldermask shape symbols if they need to be over or undersized.

Since you cannot have more than 1 shape in a shape symbol you cannot use z-copy as long as the symbol type is shape symbol.

So save a copy of the shape symbol (whatever the name of the paste or soldermask shape symbol should be)

Setup->Design Parameters->Design and change type at the bottom to Package

Now do a z-copy to generate your paste or soldermask shape

delete the original shape

Change back to shape symbol using Setup->Design Parameters->Design

Save off the shape symbol and reference the paste or soldermask shape from the respective type in pad designer.

Best regards

Ole

Thanks for replies.

When I create SMD padstack that uses "shape", I use the same shape to define pad on top, solder mask top and on  solder paste top layers. No problems here.

When I add copper to the footprint, I add it as etch on top layer and next as package geometry solder mask top and solder paste top. No problems here as well.

The only "problem" I'm concerned about are DRC errors between footprint pins and footprint copper that overlaps partially these pins.(these copper is not in padstack definition. It is placed over the footprint pins as "etch, top". On top of it I placed package geometry solder mask top and solder paste top.)

The errors were transferred to the pcb when I just added manually symbol footprint to the board (no nets connected to the footprint pins).

Allen, I understand from your reply that DRC errors will not apper on the board after net list has been transfered to it and components have been placed.

If this is tru, it solves my "problem".

I can't verify it because I'm on learning stage now and I don't have any net list ready that I can transfer to the board file.

Olek

Olek, 

When defining the copper shape in the footprint make sure to extend the shape beyond the center point of each of the pins.  You will see DRCs in the footprint but when you place the component in a design the DRCs will disappear as long as the two pins have the same physical net name.  Make sure to load the logic prior to placing the component so the shape automatically adopts the net name of the pins it crosses. If these pins are not connected to a common net on the schematic or if you place the component directly from the library without a netlist then DRCs will exist where the pins cross the shape.

Hope this helps,
Mike Catrambone