0.3mm thermal vias in DPAK pads have failed badly

[treez]

Hello, This thread speaks of using 0.3mm thermal vias in the pads of DPAK power FETs…
https://www.edaboard.com/showthread.php?t=275722

We have 12 thermal vias equally spaced under the drain pad of the DPAK

…we have now tried this, and unfortunately some (not all) of our PCBs come back from the PCB assembly factory with sharp “shards” of solder protruding out of the bottom of the thermal vias.

This is disastrous, as it pierces the thermal rubber pad that the PCB sits on, and contacts with the earthed heatsink.
Post #7 of the above thread speaks of putting solder resist on the bottom copper layer, with an opening just wider than the thermal via opening. I wonder if this will solve our problem?
Alternatively, I wonder if we should just add solder resist over the entire bottom copper, so that the bottom of the thermal vias is covered up, and might stop solder from leaking out?
I wonder if using leaded solder would also help solve the problem?
I also wonder whether the solder bath of the reflow oven was too hot? Also, I deeply suspect that just maybe the DPAK FETs were actually hand soldered on, because of the difficulty in getting the reflow solder bath the right temperature for all the 0402 resistors, and also the big DPAK FETs. As such, the hand solderers (if they were hand soldered, we don’t know) might have been responsible for the protruding solder?
-Maybe its just impossible to get the reflow solder bath the right temperature for a board which contains both ‘teeny’ tiny 0402 resistors, and also ‘big’ DPAK FETs?

 

[barry]

Solder bath in a reflow oven? I think you're confusing wave soldering with reflow soldering. Regardless, your assembly house should resolve this problem; if they can't, get a new assembler. This is done ALL THE TIME, if your assembler doesn't even know how to inspect and rework boards, they are incompetent.

 

[treez]

Thanks i see what you mean, but if we can help it along by just putting solder resist covering the openings of the thermal vias on the bottom layer, then i think we should do that ...is there a reason why this may be a bad idea though?

 

[SLK001]

The "sharp shards" of solder indicate that the board is being jostled during the cool-down portion of the reflow cycle. This is causing the drips that are in the solidifying stage. It also implies that the solder stencil is allowing too much solder to be placed for the DPAKs. At worst, you should be seeing a little solder wetting the copper on the back side. This bleed-thru should be small enough that your thermal pad doesn't have an issue with them. I agree with barry that this problem is one caused by your assembly house and they should be able to correct on their own.

 

[FvM]

It has been often mentioned that solder protrusion must be expected with open thermal vias, thus in all cases where it can't be accepted, e.g. double side SMT boards with the second assembly pass on the backside of thermal vias or PCB designed for heatsink mount, the vias should be plugged or tented.

An open thermal via as discussed in post #15 of this thread https://www.edaboard.com/showthread.php?t=275722 can prevent excessive solder drain, but it can't guarantee a flat surface.

 

[mtwieg]

Tenting just the bottom side won't help. During reflow, solder will plug the top side, and the via will outgas through the bottom.

Tenting on the top side, directly under the thermal pad, is a better option. The bottom should not be tented in order to prevent outgassing.

The tenting on the top may increase thermal impedance a bit. I haven't seen any documented comparison though.

 

[barry]

Tenting just the bottom side won't help. During reflow, solder will plug the top side, and the via will outgas through the bottom.

Tenting on the top side, directly under the thermal pad, is a better option. The bottom should not be tented in order to prevent outgassing.

The tenting on the top may increase thermal impedance a bit. I haven't seen any documented comparison though.

I REALLY don't think you want soldermask under a thermal pad.

 

[treez]

I REALLY don't think you want soldermask under a thermal pad.

Thanks , the thing is, if the rest of the bottom layer copper (the non-thermal copper) has solder resist on it, then you risk a tiny air gap if you dont also put solder resist over the thermal pad copper bit. Do you agree?

Tenting just the bottom side won't help. During reflow, solder will plug the top side, and the via will outgas through the bottom.

Thanks, surely it will outgas whether or not the thermal vias bottom side is covered in solder resist?
What i mean is, the spread (wicking) of solder to the bottom layer, going through a thermal via, will be less if the via is initially covered in solder resist?

 

[betwixt]

It involves a little manual labor but in low volume production runs in the past I've just placed a Kaptan square over the vias to prevent solder blobbing under heat sinked devices. It does allow the bottom of the via holes to take up some solder but the trapped air under than tape prevents it reaching the top side.
It's an issue the assembler has to deal with and may not be feasible in your situation.

Brian.

 

[marce]

Firstly the vias have NOT failed, it is the assembly that is the problem.
IPC-7093 is a good place to start.

 

[mtwieg]

I REALLY don't think you want soldermask under a thermal pad.

I've done this a few times in the past with larger QFNs, as described in the manufacturer's app notes. This was on a design for which my minimum via hole diameter was 15mil. My preference would have been for 10mil vias without tenting, if it was my call...

- - - Updated - - -

What i mean is, the spread (wicking) of solder to the bottom layer, going through a thermal via, will be less if the via is initially covered in solder resist?

Possibly. I don't know if tenting the bottom will hurt or help overall.

 

[fishbowlfx]

Since you already received the batch of PCB assembled, then it would be costly to ship back and redo. Best you can do is hand solder the issue since I presume the bottom copper directly under the pad is exposed. Then highlight with photo evidences and then request for discount on your next order. You can also revise your design because 0.3mm is a big hole thermal via then it should not be tented but plugged to reduce solder voids/protrusions. This costs money so weigh your options.