5
\$\begingroup\$

I'm looking for a good solution on how to design a thermal pad that is good for solderpaste assembly.

PCB fab that I'm using can't place any soldermask on vias like in this example:

enter image description here

And I'm not practic to design this pads. As I read on some documentations this vias, with solder on them, can suck solder creating problem on IC fixing and possible solder short circuits.

I tought about placing vias on the corner and with a solder stencil place solder only on the inside of thermal pad. But I don't know if it's good.

Can someone advice me a good method?

Also, I've an additional question not really related to this. I've read about decoupling (Decoupling caps, PCB layout) that every ground local plane should have only one spot to main ground plane, but in this case we have a lot of them, it can create problems?

\$\endgroup\$
5
\$\begingroup\$

TI recommends using solder-mask-defined thermal pads without solder mask around the thermal vias. Solder going though the holes and causing voids (not shorts) is said to not be a problem if the via hole diameter is kept to 0.3mm or less. Spacing of 1mm is suggested, and of course the vias should not have thermal reliefs.

enter image description here

Putting vias just in the corners would degrade the thermal performance.

If cost is no object, some fabs can plug the thermal via holes with copper.

If the pad is actually used to carry significant current then the usual considerations apply, you can split the plane or do other things to control current flow, but it is not usually necessary, especially on a mostly digital board. You really can consider all the thermal vias a single connection to the ground plane for most practical purposes- an exception might be if you had some insanely sensitive amplifier very close to the thermal pad so that it caused voltage gradients in the ground plane- but that would be bad layout practice to have such things too close to each other and without some kind of isolation moat etc.

\$\endgroup\$
  • 1
    \$\begingroup\$ See also: PowerPAD Thermally Enhanced Package and PowerPAD Made Easy. \$\endgroup\$ – Tut Jul 9 '15 at 12:31
  • \$\begingroup\$ What do you mean with split the plane? Create a single plane for each via? Or just isolate thermal pad from any other ground and create something like thermal local plane? \$\endgroup\$ – Singe Jul 10 '15 at 9:00
  • \$\begingroup\$ @Singe Anything from a straight or L-shaped cut in the plane that forces currents to go around to two or more sections of plane on the same layer. Be careful with this- it's generally a bad idea except when necessary- a solid ground plane is best for simple situations. Running a trace across a break in the ground plane will tend to radiate EMI for example. \$\endgroup\$ – Spehro Pefhany Jul 10 '15 at 10:27

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.