thermal via and powerpad

[buenos]

hi guys,

where do you put the thermal vias for a dissipating IC with power pad?
are there real hard reasons to do it in a particular way?

I wanted to put under the power pad, but my colleagues in my new job said "we dont do it that way here". i know the tin flows and so on, but cooling is more important.

 

[majnoon]

I always put it as in A under pad in middle of PADDLE and never had problem.

Purpose is not only Cooling but proper connection to PWR plane.
Sometimes data sheets have info regarding Drill size of vias but if not you can use 12 to 15 Mil drill holes.
Tell your colleague that it is recommended by device manufacturer and assembly shops know how to handle this.

Regards,

M

 

[FvM]

You'll remember, that we recently had a discussion regarding via tenting. I mentioned the Amkor application note that mainly discusses different ways to carry out the "A" variant.

If small (0.01" - 0.012") open vias are acceptable, they are the most simple solution. They are most effective, if more than one plane is available to transport the heat. If the thermal vias are connected to a single plane only, thermal resistance with variant "B" isn't much higher, so it could be used as well. But variant "A" may be necessary also cause there's no room around the thermal pad.

 

[buenos]

thanx.

i talked to one of our production (smt / soldering / assembling) engineers, he said I could use 0.15mm finished hole vias under pads, vithout tenting/plugging them. (I like it because these small holes have more copper in them) The appnotes what I found, all of them mention 0.3mm-0.33mm via holes with 1mm-1.3mm pitch.

all of our boards, have more than 1 gnd plane.

 

[FvM]

I also think, that this is the optimal technique (if not using plugged and copper plated vias). An assembly house has kept me from using it with chip scale packages for a customer. They feared solder shorts when parts are sagged by solder wicking.

I wonder, if the issue was ever observed with 0.15 mm (6 mils) vias? If so, a possible solution is in using even smaller via drills with effectively zero finished diameter. They can be used even on BGA pads without plugging. But they are limited to thin substrates because of the maximum drill aspect ratio.

 

[difflvl]

Method A is better. I've never had a problem with solder even with larger holes .3-.35 mm. If anything you can always tent the vias.