• State TI Thinks Resolved
  • Locked Locked
  • Replies 4 replies
  • Answers 1 answer
  • Subscribers 41 subscribers
  • Views 573 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

CC3220MODA: PCB requirements for Thermal Vias

Nick Price
Expert 2235 points
Part Number: CC3220MODA

Hi

I'm currently layout on my board for the CC3220MODA module. The recommend layout specifies 4 via's in each thermal pad on the base of the module. Each via being 0.2mm (Typ). (see image below)

I guess this pad is there to wick up excess solder, so the module will sit down flat on the pcb.  Now this via must be kept clear of solder resist , so the solder can wick down.

My pcb suppliers are unable to guarrantee a via with a hole size of 0.2mm will remain clear after the solder resist process. In fact they are asking me to open up the via holes to 0.45mm, which they can guarrantee.

Now, I know I can pay a lot more money, and change the processes on pcb manufacturer to obtain this. But we are using these modules on low cost products, and we need to back to get low cost PCB manufactuer.

We like to try and stick to TI recommend pad and holes sizes, because our products are built and tested by sub contractors. If there are issues they always go back to Manufactures recommendations.

Please comment

Regards

Nick

  • 0
    TI__Mastermind 27605 points
    Hi Nick,

    The only thing I can think of right now is thermal conductivity to lower layer increasing which could affect reliability.. maybe.

    -Aaron
  • 0 in reply to made4engineering
    Intellectual 270 points
    Hi Nick,

    I can't speak for TI but I think 0.2mm typ is just a recommendation but not critical. In my opinion, changing those vias to 0.45mm will not impact thermal design in any significant way.

    But more importantly, as I see from the TI supplied design (which says "solder mask defined" for the green outlines; see legend below), the thermal pads including the four vias are by design meant to be clear of solder resist. Your PCB supplier seems to have misunderstood the spec.

    Yes, excess solder can be a concern. The PCB designer/supplier can address that by undersizing stencil holes over thermal pads so that only a manageable volume of solder paste will deposit there. This is normal practice.

    Hope this is useful to you.
  • 0 in reply to user1818910
    Expert 2235 points

    Yes, the via's are to be free of resist. But the manufacturing process (i'm told) , they flood the whole board with Resist. Photo the board, and then wash away what is not needed. Because the whole are so small, they can't wash out the 0.2mm via's. So they will not wick up the excess solder.

    I think I will have to increase the via holes to 0.45mm, and change the positions around.

  • 0 in reply to Nick Price
    Intellectual 270 points
    According to the figure, the nine squares are to be totally free of resist. This is similar to the "via on pad" situation which is usually accepted in most pcb process. I recall that for 8mil (0.2mm) vias-on-pads, to one had to pay a little bit more to have them plugged (for different reasons, to prevent solder flowing down/out). Maybe a different kind of process.

    I believe the primary function of these vias is to conduct heat into the inner or bottom layers. In any case, as the MOD is on top while your board is getting cooked, these vias can't wick "up" solder but can at best allow excess solder to flow out (down).

    Irrespective of that, I would recommend stencil undersizing in these areas so as to reduce the print volume of solder paste -- you don't want excess solder if you can help it.