KiCad : How can I create a footprint with thermal vias?
I have done it two ways.


Don't change the footprint file but draw a zone on the top solder mask the size you want the metal to be.  Then draw a zone on the copper layer that is connected to the same net as the SMD pad.  It is especially convenient if that pad connects to ground.  Change the zone properties to Pad connection: Solid so that it will fill completely.  Now you can add vias to this area, if you are connecting between the top and ground that will give you more metal to dissipate heat.  You might want to remove the preference Delete unconnected tracks, and any others that deal with deleting redundant tracks.


Do it from the footprint.  Just add more pins (through hole) with the same pin number as the smd pad number.  These will act as your thermal vias so size them appropriately.