High Power PCB Layout Considerations

Thread Starter

TechWise

Joined Aug 24, 2018
54
I am designing a PCB Layout for a variable frequency motor drive. It runs from a 100Vdc input and max 30A per phase output. It's a simple 6-mosfet layout using the internal diodes.

My thoughts were to have two filled areas on the top layer for the +Vdc and -Vdc connections. Planning to split the top layer in two and just have two large rectangular pours for this purpose. Planning to do something similar for the bottom layer except splitting it into three large rectangular pours for each phase. This leaves me thinking that the gate drive connections and shunt measurement Kelvin connections can be routed in two internal layers. Is this wise? I was thinking of keeping the power traces to the outer layers for better heat radiation but it does mean I'll have vias all over the place for the signal connections

Also, I'm planning on using isolated gate drivers and transformer isolated power supplies. Also, I'll be using isolated error amplifiers for the current sensing. If I go with my proposed layout I'll have to position these components relatively far away from the power traces. Is this good practice?
 

DickCappels

Joined Aug 21, 2008
5,882
At 30 amps you might find bus bars to be much more practical than just copper on a PCB. 30 Amps can heat up a lot of copper fast.
 

Thread Starter

TechWise

Joined Aug 24, 2018
54
At 30 amps you might find bus bars to be much more practical than just copper on a PCB. 30 Amps can heat up a lot of copper fast.
I did consider this as a back up option but I reckoned I would just about get away without them. According to the trace width calculator, for an ambient temperature of 25deg (never reached here in Scotland :cool:) and an allowable temperature rise of 25deg, using 2oz copper and carrying 30 amps for 75mm, I would need a trace width around 9.5mm. I'm hoping to use a pour around 75mm long and 20mm wide for each phase on the bottom layer and a pour 75mm long and around 30mm wide for the +Vdc and -Vdc.

Should the layer stack up be ok with power on the outside layers and signals in the inside layers? I can't really see any other way to do it :confused:
 

DickCappels

Joined Aug 21, 2008
5,882
That sounds pretty good. Just keep bus bars in the back of your mind if things start to heat up.
 

ronsimpson

Joined Oct 7, 2019
115
and an allowable temperature rise of 25deg
It looks like you will have most of the board at 25C and where the current runs at 50C. That seem stressful.
I do not like having more than 10C temp rise because of current.

I use the copper as a heatsink. Heat from the MOSFETs is going into the PCB. And heat from the PCB is going into parts.

I have run the same trace in all four layers to get the resistance down.
I have run a hot trace on the outside so heat gets out better then running copper on a inner layer.
I use a inner layer ground plane to help spread out the hotspots.
Remove as little copper as possible. This helps spread out the hotspots.
Use area fills for high current traces.
I do not use thermal reliefs with high current.
 
Last edited:

Thread Starter

TechWise

Joined Aug 24, 2018
54
It looks like you will have most of the board at 25C and where the current runs at 50C. That seem stressful.
I do not like having more than 10C temp rise because of current.

I use the copper as a heatsink. Heat from the MOSFETs is going into the PCB. And heat from the PCB is going into parts.

I have run the same trace in all four layers to get the resistance down.
I have run a hot trace on the outside so heat gets out better then running copper on a inner layer.
I use a inner layer ground plane to help spread out the hotspots.
Remove as little copper as possible. This helps spread out the hotspots.
Use area fills for high current traces.
I do not use thermal reliefs with high current.
I was planning on putting slots in the board positioned under the gate drivers as an isolation barrier. I was hoping this would prevent too much heat from the power section from being conducted back into the control section.
 

kubeek

Joined Sep 20, 2005
5,599
I suggest you do the control section as a separate board, because you could have trouble with making thin traces - high oz pcb has higher requirements for spacing between traces. Also you needlessly waste space on expensive board, when you could have the control circuit on a smaller and cheaper second pcb.
 

kubeek

Joined Sep 20, 2005
5,599
Here you have an example how I did my power and control board for my welder project. I used thin copper but have unmasked traces and soldered copper wire ontop, since it is a one-off.
 

Attachments

DickCappels

Joined Aug 21, 2008
5,882
Excellent advice there from kubeek in post #7. In all seriousness, having a separate board for the control circuit can help protect your control circuit and you from mishaps, particularly if you can keep dangerous voltages off of the control board.
 

Thread Starter

TechWise

Joined Aug 24, 2018
54
I suggest you do the control section as a separate board, because you could have trouble with making thin traces - high oz pcb has higher requirements for spacing between traces. Also you needlessly waste space on expensive board, when you could have the control circuit on a smaller and cheaper second pcb.
Excellent advice there from kubeek in post #7. In all seriousness, having a separate board for the control circuit can help protect your control circuit and you from mishaps, particularly if you can keep dangerous voltages off of the control board.
I should have said I'll be using a Texas Instuments Control Card for the control so all of the control will be on a separate PCB that will just dock into the converter.
 
Top