I have a SMD chip that gets pretty warm when operating and I want to try and design a footprint that allows more ventilation and extra copper to keep it in range.

Does anyone know of a tutorial that covers how to make footprints (MOD files) with vias through it?

Have Googled it, but could not find a lot about this topic.

I know that it's possible to manually change the MOD file with a text editor, maybe that's an option.

  • 1
    \$\begingroup\$ I don't use KiCad, but a word of caution. If you're going to do this, pay very close attention to the manufacturer's recommendations. Vias will wick away solder paste, pulling it off the pads into the vias, during the reflow process. Different manufacturers have different opinions on whether that is good or bad. They will all have recommended via patterns, and probably solder mask coverage guidance. \$\endgroup\$ – Matt Young Mar 11 '14 at 2:10
  • \$\begingroup\$ I agree...I have actually seen this issue on some products. \$\endgroup\$ – Bertus Kruger Mar 11 '14 at 18:58

I have done it two ways.

  1. 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.

    Thermal Pad

  2. 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.

    Thermal Pad 2

|improve this answer|||||
  • \$\begingroup\$ Thanks for the quick reply. Very useful tricks to know... ;) \$\endgroup\$ – Bertus Kruger Mar 11 '14 at 18:57

Another way to do it in the footprint: rectangular through-hole pads with the same name and copper on both sides:

Pads with embedded vias

These will be an absolute pain to solder by hand, obviously, but it looks nice in 3D view:

3D view of embedded vias

|improve this answer|||||
  • \$\begingroup\$ Must they be soldered by hand? Is there no way to design the KiCad footprint so that KiCad generates a paste mask that applies solder to the front of the TH pads? And by solder by hand, you mean: from the back apply solder by hand until it wicks to the front and fills between the part and the thermal pad? \$\endgroup\$ – bootchk Aug 18 '15 at 22:04
  • \$\begingroup\$ You can select "F.Paste" in the layer mask for the pads, then the pad should get paste. If not, that is a bug. Ideally, we'd also support plugged vias, but we don't yet. \$\endgroup\$ – Simon Richter Aug 19 '15 at 0:39

Maybe somebody has a better way, but I have always ended up putting them in by hand. You can make the process easier by enabling two dummy layers and setting the via key to flip between them. Otherwise KiCad sees a bunch of extra vias and tries to get rid of them.

Also Matt Young makes a very good point in his comment: don't make your thermal vias too big, otherwise solder will wick out the bottom of the board. I have done that and suffered the consequences.

|improve this answer|||||

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.