Thermal disapation through PCB Inner layer?

[jwhitmore]

Hello all,

I'm using an LM5088 for a DC DC converter in a project. I want to potentially push it a bit so want to keep it cool. there is a ground pad under the IC and the footprint includes the corresponding ground pad on the under side of the board.

That's all good but the board is going to be a 4 layer board and I'm wondering could I put another 2 ground fills in the inner layers to conduct the heat away as well. I can't find information on whether that can be done or whether it'll cause problems in the PCB? I can't think of any reason why it'd cause a problem because it'd be 4 ground layers stacked under the LM5088. Having said that soldering the thermal pad might be an issue given all the thermal conduction away from the pad.

Perhaps a better solution would be to wind a piece of copper wire into a coil and solder that into a hole and have it flapping in the breeze beside the IC That'd look like an Antenna and confuse people.

[T3sl4co1l]

I'm more concerned that you weren't intending on using the inner layers for ground fill as it is!

Tim

[bugrobotics]

Here's a good app note from TI about using multiple layers with DC-DC converters.

http://www.ti.com/lit/pdf/snva424

[mr_darker]

MCPCBs or Ceramic PCBs are good for thermal dissipation within a board.  Expensive though and not really standard pcb services.

Hand soldering you just turn the heat up so it melts before the heat dissipates, 1 second and no melting is too long and not hot enough.  Reflow soldering is de way to go if you're not doing that.

I'd say just take a few gallons of mineral oil, fill up yer bath tub, and toss her in there.  Liquid cooling.

[ajb]

You can and should use an internal layer as a solid ground plane. 

Internal layers can help with thermal dissipation, but not a lot.  The thermal conductivity of the fiberglass that surrounds the internal layers is high enough that once heat spreads into the internal layer it doesn't really have anywhere else to go.  PCB copper layers are thin enough that the thermal resistance in the lateral direction limits the effectiveness of lateral heat spreading.  The best thing you can do (short of adding an actual heatsink) is run a bunch of vias from the top side thermal pad to a copper area on the bottom layer.  With enough vias you can get reasonably low thermal resistance from top to bottom, and then the bottom copper can radiate into the ambient. 

[T3sl4co1l]

To put some numbers to that: a 1oz 4-layer 0.06" board will have about 2-4 times more lateral (heat spreading) conductivity when all four layers are mostly filled with copper, versus bare board.

The thru-plane conductivity of bare board is something like 1/5th that of its lateral figure.  So, spreading heat out into wide areas first, then through the board, is very effective.  Vias are also very effective.

The thermal and electrical (DC) capacity of vias is also about doubled when filled with solder, if you can accommodate that in the design (e.g., large diameter vias in a wave soldering process).

Beware, via-in-pad can be a solderability issue for paste-and-reflow process.

Mind, soldering is basically free-for-all if you're hand soldering and inspecting.

Tim

[SiliconWizard]

Heat dissipation is significantly reduced on internal layers compared with external layers, but of course internal planes will help. Just don't count on internal layers *only*.

[jwhitmore]

Thank you all for your help. I'm picking up some of the practicalities as I go along and for some reason I was using a Ground fill on the top and bottom layers of the four layer board but not the internal layers. I didn't realise that was stupid till now. Oops.

Thanks again, I'll correct that mistake and see how I get on with it.