PCB design: multiple layers vs heavier copper

[willDavidson]

TL;DR Summary

I am considering if I should use heavier copper or additional layers if thermal issues are a concern

I am designing a board which will have relatively high current. The options are to use heavier copper (4 oz), use two layers (2 oz), or 4 layers (1 oz).

Are there any benefits to using one configuration over the others?

 

[hutchphd]

In general I go with heavier copper mostly for thermal reasons. The mitigating factors are whether this is an isolated portion of an otherwise low power board and possibly cost. And of course all of the usual EM issues which may or may not be at work here

 

[willDavidson]

This will be a power plane so no traces on it. Only cutouts for clearance purposes. Is it better thermally basically a lower number count typically means less insulation which means less trapped heat within the board? I'm new to this. What kind of EM issues would you consider?

 

[Joshy]

The vias on multilayer also have a maximum current they can handle even if you put a bunch of vias on there the current distribution is usually not uniform... meaning that it's possible without careful placement for most of the current to go through a small number of vias.

 

[willDavidson]

Ok thanks I'll make sure to pay attention to the current in the vias. Does having heavier copper somehow help current sharing in the vias?

 

[Joshy]

Heavier copper will be better for your application so you will definitely want to do that no matter your choice, but it will not help with current sharing.

 

[Baluncore]

Are there any benefits to using one configuration over the others?

Yes.
Avoid internal layers that will trap heat. (Rules out 4 x 1 oz ).
Use a two sided board so heat can be radiated from both sides. (Rules out 1 x 4 oz ).
Only the 2 layers x 2 oz remains.
Run wide tracks for high current on both sides where possible.
Use component leads to connect between the two sides.
A field of vias (that are filled with solder) may be used to transfer heat between the two sides.

 

[willDavidson]

A field of vias (that are filled with solder) may be used to transfer heat between the two sides.

I read about conductive epoxy filled vias. Is somehow adding solder to them better at conducting heat? I know that having them filled with conductive epoxy will be more expensive so I'm not considering that for now.

 

[DaveE]

I read about conductive epoxy filled vias. Is somehow adding solder to them better at conducting heat? I know that having them filled with conductive epoxy will be more expensive so I'm not considering that for now.

I've never seen this in practice for power circuits. You will be better off with normal vias to the outside (not buried vias) with no solder mask so the solder fills the vias. However, if your PBCA is all surface mount then you need to be sure that solder paste is applied to the vias you care about.

I think @Joshy already implied this, but I'll rephrase. Be careful about breaks in the plane layers that concentrate current. It's not just the thickness that transfers heat it's also the width. This can be a difficult issue near devices with lots of interconnects because of the trace vias that break the plane. If you know that your heat flow is mostly in one direction, try to line up your trace vias parallel to that direction instead of across it.

I think your question is good, but, In my experience, the problem with heat generated inside a PCB isn't the local heating, you can fix that with more Cu to spread it out, as you have suggested. The bigger problem is getting the heat away from the PCB. Unfortunately the fiberglass in PCBs is a poor heat conductor. If you have a large PCB with only a few hot places, then this may not be a problem.

One technique is to reserve the edges of the board for lots of Cu and lots of thermal vias to outer Cu layers and mount with a heat conducting path (like a heatsink of some sort) to get the heat out. Electrical insulation is probably needed; there are good thermal conductive films available for this, as you might use for power transistor mounting, for example.

If/where you can add Cu to the outer layers with thermal vias to the internal planes to allow convective cooling. However, don't expect a dramatic improvement. Convective cooling down at the board level is often poor.

For extreme cases there are people who make ridiculously large Cu layers (like 20 oz.). Here is a link that I chose at random about this sort of PCB: https://www.epectec.com/articles/heavy-copper-pcb-design.html

Finally, for questions like 2x 2oz. layers vs. 4x 1oz. layers, I have found that the good PCB fabricators can be a valuable source of information. They understand better than us the cost and manufacturability issues involved.