Create 1:1 SM expansion for copper pad

How do you create a 1:1 SM expansion for a copper pad? If I leave the Solder Mask clearance as 0 in the Footprint Properties, it takes the value of the global Solder mask Clearance.

The global Solder Mask Clearance is set to 0.1mm, which is desired for every other component except one, which requires a SM expansion to be 0(Size of SM = Size of copper pad). This component instead adopts the global clearance(as it is designed to do).

Is there a way to set the clearance =0 in the FP properties and have it not adopt the global clearance?

I’m guessing here, but I think that if you set the Solder Mask expansion to any non-zero value in the footprint, then it overrides the global settings.

A workaround is to set it to a very small value. KiCad works with nano meter accuracy, which is far smaller then the tolerances of any PCB fab.

Thanks @paulvdh for the quick response.

Yes, I did think about that, but I wanted to know if there was a way to actually set it to 0, and not have it read the global clearance values.

Just trying to keep the library integrity by not specifying random small values(and keeping it matched to the datasheet specs).

If you look at the properties of a pad in the Footprint Editor, then it explicitly tells you the value is inherited from somewhere else if set to zero:
image

Using a small value as a workaround is an ugly hack, but I do not expect a better implementation in the current KiCad.

Maybe I’m wrong and somebody else can amend to this thread.

The “official” solution is to switch off the mask layer from the copper pad and create another aperture pad with only the mask layer. This works in v5.1 and later because the values aren’t inherited for aperture pads. I agree that using zero as a special value for inheritance isn’t good but it’s a historical decision and was kept for compatibility reasons. The behavior was explicitly changed for aperture pads exactly to allow using zero without side effects.

Ah indeed, I did not think about separate pads for solder mask apertures.

There is not much for this in the manual. I believe you have to completely remove the pad number for these aperture pads.

When in doubt, then search through the KiCad libraries for examples.

Thanks for pitching in @eelik.

The behavior was explicitly changed for aperture pads exactly to allow using zero without side effects.

Noted.

I guess this is the way to go in v5.