Solder seeping out of thermal vias onto the bottom layer copper

Hello,
We have power packages which are hot when running. (they contain power FETs and control circuitry)
I just noticed yesterday that the bottom layer has solder seeped out onto the bottom layer thermal copper...seeped out through the thermal vias in the pad of the packages.
Is this likely to have happened...

1....during production soldering of the board?
2...during some of our testing operations where we run the board?

The bottom copper has no solder resist over it, as it sits on a rubber pad on a heatsink.

Design of thermal vias and particularly the solder wicking problem has been frequently discussed at Edaboard. The described effect is typical for open thermal vias, you can refer to arbitrary previous threads, e.g.

https://www.edaboard.com/showthread.php?t=275722
https://www.edaboard.com/showthread.php?t=322189

Regarding point 2, there are very few semiconductor devices that would tolerate a case temperatures up to solder reflow (and respectively higher junction temperature) in operation, isn't it?

This will happen when the aspect ratio of the holes is small enough. And for thermal vias, it can actually be very desirable since a plated hole filled with solder has much lower thermal impedance than without solder. Though I wouldn't rely on something like that in a production design.

If you need to prevent it, you can plug or fill the viaas. As a cheaper option, you could just tent the vias on the top side (don't tent the bottom side, as it will likely outgas during reflow).

It most likely occured during reflow, although I have had power devices reflow themselves (and survive) when incorrectly operated without a heatsink.

By rubber pad, I'm assuming that you mean thermal pad, as a rubber pad would be an insulator.

If the solder is flowing out where the thermal pad will be, then I wouldn't worry about it, as long as the out-flow doesn't affect your stack-up. Like mtwieg said, filling the vias with solder can have a beneficial effect on your thermal management.

If the solder is interfering with your proper stack-up, then a redesign of your solder stencil may be needed.

problems this causes...if the solder leaks out the via holes...exactly what is left to solder the backside of your semiconductors to the heatsink/pads??? Also, the solder leaking out the back might make a raised bump so that your heat sink no longer sits flat onto the board...a big thermal problem.

I believe you can fill those holes first before soldering.

if the solder leaks out the via holes...exactly what is left to solder the backside of your semiconductors to the heatsink/pads???

Click to expand...

Thanks, that was one of the worries. Hopefully the pcb assembler put loads of solder paste on there in anticipation of the leaking solder through the vias...it wasnt much, but definetely some...fortunately it doesnt put a bump on the bottom, and the slight 'givingness' of the thermal pad accommdates this solder film on the bottom layer.

Hopefully the pcb assembler put loads of solder paste on there in anticipation of the leaking solder through the vias.

Click to expand...

The assembly house (or whoever orders the solder stencil) has limited means to adjust the solder amount
- choosing a stencil thickness
- modifying the size of specific apertures

Finish of thermal pads solder is usually not the first priority in the trade-off. The "loads of solder paste" may well conflict with other objectives.

There are cases where solder spillage on the backside of thermal pads is absolutely forbidden, e.g. on the topside of a double side populated board.

There are two cases of this happening:
First, heating time is too long when you welding
Second, the detection of circuit board heating will let the solder through the welding hole exudation

Don't agree. You can't rely on solder not protruding at open thermal vias. Of course solder amount and reflow temperature affects the thermal via finish. But to avoid solder leaking, you must apply tenting or plugging as discussed in the linked threads.

The other variant, board-self heating up to reflow temperature must be considered as permanent board failure.

Yes, the more solder, the higher the temperature, the more solder penetration of heat through the hole.
Of course, if you have been heating the same place with the solder, it may damage the circuit board (pad)

Hello,
Thanks, I appreciate the related threads in post #2 above.

We have just had 16 prototype PCBs delivered and they have 16 thermal vias in the pad of the D2PAK FETs. These vias are 0.3mm diameter. They are also 1.5mm apart from each other.

***************
Unfortunately, solder has wicked through the thermal vias to the bottom layer…this wouldn’t normally bother us too much, its just that some of the PCBs show a somewhat sharp, pointed bit of solder protruding from the thermal vias on the bottom layer. We are worried about this piercing through our thermal pad and contacting with the heatsink.
***************

We read IPC7093A and this says that 0.3mm thermal vias in pads are OK, so we don’t understand why we have had such problem with solder wicking.

IPC7093A:
https://www.pcblibraries.com/forum/ipc7093a-btc-qfn-solder-mask-defined-thermal-pad_topic2154.html

We understand that we can solve this by plugging the vias, but can’t really afford this.
From what ive read, one option is either to use leaded solder (because it results in the PCB being less heated and so less wicking occurs)…..
However, that is illegal , therefore, the only real options remaining are 1.) - to use a tougher thermal pad (do you know of any that can withstand piercing by sharp bits of solder?)
2). –We could “tent” or cover the thermal via holes over on the bottom layer with solder resist to prevent the solder from wicking through to the bottom layer.
However, this is said to cause a problem with “outgassing”. Do you know what “outgassing” is?

The following discusses “Outgassing”, but its not clear what is meant.
https://www.epectec.com/pcb/wave-soldering-defects/outgassing.html

I cannot see how any problem can be caused by covering over the bottom layer thermal via openings with solder resist?
If it does cause a problem, then do you know what the problem is? Also, if “Tenting” the thermal via opernings on the bottom layer is bad, then is the next best thing to cover the bottom layer with solder resist “around but not over ” the thermal via openings?
Maybe we need to go down to 0.25mm thermal vias in the pad to avoid such wicking though of solder? As discussed, the wicking of solder itself does not bother us, but the sharpish solder protruding out of the bottom of the via opening does worry us because it may pierce the thermal pad.

The pointed solder peaks indicate that not enough flux was used in the reflow, or that the reflow profile was bad. This is a problem with the assembly house, not yours. You should have them address the issue.

Is it really a problem? Does having the flag of the device contact the heatsink cause shorting?

Outgassing is when the flux in the solder flashes to gas while surrounded by solder, which can cause a mini explosion. Another reason to believe that the profile is bad.

The answer is quite simple. If a flat bottom surface of your PCB is required (e.g. as heat sink interface or for successive solder paste printing), you need to fill the thermal vias. Pro an cons of different via fill and plugging techniques have been continuously discussed at Edaboard.

If a flat bottom surface of your PCB is required

Click to expand...

Thanks , it doesnt have to be exactly flat, because the thermal pad is slightly rubbery...but we cannot allow the pointed protrusions.
The big unknown with filled vias is cost. We have five SMD FETs on our board, each with an array of 25 x 0.3mm vias.

Also, if the vias are to be filled, then we might as well make them wider diameter.

Outgassing is when the flux in the solder flashes to gas while surrounded by solder, which can cause a mini explosion

Click to expand...

Thanks, do you know why "tenting" (or covering) the thermal vias on the bottom layer should encourage these exploions?
Even if there were an explosion within a tented via, then surely it would just blow a little hole in the solder resist, and do no harm?

I have reviewed the other discussions in edaboard, and there is some concensus that covering the thermal vias over on the bottom layer (with solder resist) will stop the solder from flowing through and producing these pointed protrusions. However, others said it could cause outgassing, -but we dont see how covering a thermal via with solder resist causes the flux in the solder to explode?