How to build a NSMD footprint in KiCAD

Hi, I am now building a footprint WLCSP-6x6-0.4mm pitch of altera MAX10 10M02. In a WLCSP package manual, it says that NSMD is preferred over SMD. In NSMD, the clearance of pad to mask is 0.075mm, while in SMD the overlap of pad to mask is 0.050mm.

How could I build a NSMD pad by providing negative clearance ?

1 Like

Ummmm . . . I don’t believe you’ll get a “NSMD” (non-solder mask defined) pad by specifying a negative clearance.

I believe that NSMD pads is the usual way we expect KiCAD to operate - leaving an opening in the solder mask that is slightly larger than the exposed copper pad. The amount of clearance is specified with a positive value. Simply set the solder mask parameters for (positive) 0.075mm (3 mils). You can set a global value in the “Dimensions” > “Pads Mask Clearance” drop-down menu. (I don’t know why this isn’t under “Design Rules”, or even “Preferences”.) You may also over-ride the global value on a footprint-by-footprint basis in the “Footprint Properties” menu (move the cursor over a footprint and press “E” for “Edit”), or set a value for each individual pad in the “Pad Properties” > “Local Clearance Settings” menu (press “E” with the cursor over a pad).

To get an “SMD” (solder-mask defined) pad, specify a negative clearance.

The PCBNew “Help” file discusses this in section 11.5

Dale

3 Likes

Thanks ! Yes you are right.

I disabled F.Paste and F.Mask in pad properties, when reenable it, the clearance of solder mask works as expected. Thanks!

BTW: I found that WLCSP package requires solder paste printed after bake the board at 125°C for 24 hours. So in the footprint, should I enable F.Paste or not ?

It is not a question of enable/disable F.Paste. You will always need the F.Paste layer.

It is a question about where do you want to define the F.Paste margins for this footprint:

  • At every pad individually level
  • At footprint level
  • At board level

Think of board level as the default settings. If you need different clearances for a particular footprint, change the settings for this footprint.

Pedro.

2 Likes