4-layer PCB for increased heat dissipation

[derGoldstein]

I have a few 2-layer circuits with a bunch of SMD components that get quite hot (mostly we're talking mosfets for voltage regulation and motor driving). As it is right now I put a lot of vias around them and have something on the bottom of the board that can carry the heat (sometimes just an aluminum plate attached by thermally conductive silicone does the job).

When going over various eval board layouts I noticed that some of them are 4-layer boards that clearly don't need the internal 2 layers. Instead the internal layers are just copper fills that connect to the ground planes on the top and bottom layers with a bunch of vias.
Does this help with thermal conduction? Would you add them to a circuit that only needs 2 layers just to improve heat dissipation?

Thanks in advance.

[DutchGert]

What kind of eval boards are you looking at?

In case of a MCU board or something it is probably to have a little bit of semi impedance controlled tracks and to provide good un-interupted return paths for signals.

On DC-DC boards it is also to provide low impedance return paths and 'solid' grounds.

More layers can help spreading out the heat and transfering it to another spot where you interface the board to a heatsink but usually more layers are added for the reasons above and nog solemly to improve thermal behaviour.

Just increasing the mass of the board by adding more layers can remote hotspots a bit and slow down the temperature rise but in the end you still end up with a very hot board

Also, have a look at IMS boards (https://www.google.nl/search?q=ims+pcb).

[tszaboo]

Yes, it helps, but it might not be needed, and be more expensive than alternatives. Vias are much more effective if they are in the pad, under the metal tab of the component. outside that, the third row of vias makes almost no difference. Also, small vias are better, go for 0.3mm. Also, it helps nothing, if your entire PCB is hot.
Post a picture of your PCB, power dissipation figures, I'm sure we can give you some ideas.

[derGoldstein]

What kind of eval boards are you looking at?
On DC-DC boards it is also to provide low impedance return paths and 'solid' grounds.

Yeah, quite a few DC-DC converter boards seem to do this. What does "solid grounds" mean in this context?

Also, have a look at IMS boards (https://www.google.nl/search?q=ims+pcb).

I've checked them out, but they're absurdly expensive. I haven't found a fab that doesn't charge 10 times for a metal-core board.

Yes, it helps, but it might not be needed, and be more expensive than alternatives. Vias are much more effective if they are in the pad, under the metal tab of the component. outside that, the third row of vias makes almost no difference. Also, small vias are better, go for 0.3mm. Also, it helps nothing, if your entire PCB is hot.
Post a picture of your PCB, power dissipation figures, I'm sure we can give you some ideas.

I'm mainly trying to avoid hotspots. The bottom of the board is flat (the through-hole components are near the edges) so I want to dissipate heat through the bottom.

I was asking more in general, but I can give an example of one board that's a good representation (attached). It's a PAM2422 boost converter. The chip is a soic-8 with a metal bottom. I tried staying close to their example/eval board since this is a first iteration.
So most of the heat is generated by this tiny footprint, and I need to spread it out as much as I can. I think the vias are a bit large, they're 1mm.

[sanwal209]

I think you have done pretty good PCB design with consideration of heat exchange. You have left alot of space on top left and right, you could pour copper over there with alot of vias connecting with bottom layer. That's all you can do with two layers in that particular design.

Furthermore you can do following things to increase thermal conduction:
1. Make PCB more thinner
2. 370HR PCB Material is similar to FR4 with higher temp but is available in 0.020 thickness at a very reasonable up charge which will triple conductivity .

Regarding 4 Layer: Outer layers are better for heat sinking as they are in contact with the air. Yes inner layers can reduce thermal resistance for heat to travel from source to outer layer.

[T3sl4co1l]

Yes.  Copper dominates PCB conductivity.  A four layer board, with more-or-less solid copper on all layers, will be something like 70% more conductive than a two layer board of the same thickness.

Note that that's lateral conductivity, i.e., the ease of getting heat out from under a part, over to where it can be dissipated (by air or heatsinking).

Conductivity through the board, from one side to the other, is still poor -- and worse to begin with, because laminate.  Dense vias will about double this conductivity, and solder-filled vias make it triple.

Doing everything possible, and heatsinking on top and bottom, you can effectively get about 10W from a power (D(2)PAK say) SMT device on a PCB.  Of course it may not be the cheapest option (which might be using THT, or more board area with more devices in parallel).

Tim

[tszaboo]

Actually, for a boost converter, a lot of the heat will be coming from the diodes, dissipating their 0.7V*current. Or the inductor, dissipating Dcr*current. Realistically, you get some 10-12W from that circuit, and 80+ efficiency, so you have some 2W dissipation. That is not a lot.
That being said, I would reduce the via size, and place more vias. As I said, 0.3mm is ideal. The ones, which are not below the SOIC package are kinda pointless. Make sure that most of the bottom is ground. Thats it.