How to make solder mask defined pads in KiCAD

(not asking for you to design a footprint, but asking instructions on how to design one properly myself).

TI recommends pads 7-13 on the TPS63070X be solder masked defined. Link to datasheet.

I tried to do this by adding a rectangle over the pads on the F.Mask layer, but I’m not sure if this will do what I expect. Is this the proper way to make a pad solder mask defined?

Use a negative solder mask expansion in the pad properties. Draw the pad geometry to the metal shape.

For pad 7-8 and 12-13, since the solder mask shape is not a simple offset of the copper shape, draw the copper pad with no solder mask (uncheck F.Mask in pad properties) and then draw a custom shape on the mask layer.

1 Like

A combination of Solder mask defined pads and “Non Solder mask defined pads” in a single footprint makes my eye brows frown. Add to that that each pad is on a 0.5mm pitch which is not extreme.

Have you read slua271? (See note from page 40 of the datasheet)

Note: 3. For more information, see Texas Instruments literature number SLUA271 (

I would not do this, but use an “aperture pad” instead. An aperture pad in KiCad, is a pad without copper or pin number, but you can use it to make custom sized apertures in other mask layers such as solder mask and solder stencil. With an aperture pad it is also easy to make rounded corners for the solder stencil, and this improves paste release, and thus a more uniform amount of paste on the pad.


Good idea, this will improve the output data

Thank you for the reply.

I haven’t read the app note yet, but I’ll make sure to do so since I’m not sure why mix of SMD and NSMD would be a problem.

With respect to aperture pads, would I uncheck all layers except F.Mask and then draw a custom shape to conform to pins 7,8 and 12, 13?

It may be a problem, because there is always a placement tolerance between different layers, and when you are working with features that are 0.25mm small, then avoiding stackup of tolerances is always something to try to accomplish. If all pads of a footprint are defined in the same way, then the part will self align during the soldering process. If you use these different types of pads, yo at least have to look up the tolerances that your PCB manufacturer uses between those layers, and that is also likely to be different for 2-layer and multi- layer PCB’s. It’s just an extra complication, and I see no valid reason for wanting to add that complication.

I dunno. What do you want the solder stencil to look like? Do you want it modeled after the aperture pads, or like the copper pads?

1 Like

I dunno. What do you want the solder stencil to look like? Do you want it modeled after the aperture pads, or like the copper pads?

I’d want the stencil to model after the aperture pad. I’m assuming an aperture pad only on the F.Mask layer