1
\$\begingroup\$

I am designing an SMD PCB to control two motors that consume 6 A each. I have too many components and I am using 4 layers, so I want separate the tracks. I have found out that the tracks with high current must be in a external layer. I have been thinking in use this organization layers:

  • Layer 1: Power.
  • Layer 2: GND.
  • Layer 3: Communication signals (signals that changes their value in very short time, thus are very sensible to noise, for example Serial communication of ESP32 or PWM).
  • Layer 4: Control signals (digital pins that change their value between Vcc and Gnd but keep their value steady by a long time,for example the control of a LED).

I want to use a ground plane but in an internal layer, because I found that the ground must be near of the rest of signals. About the communication and control signals tracks must be separated for avoid interference between them, but I am not sure about the minimum distance between the tracks.

enter image description here

About the heat dissipation, I know that the high power components must be separated of the other components but I am not sure if can I put components in the opposite side of a high power component.

enter image description here

For example the MOSFET connected to MT1_2 is in top plane, is a problem if I put a resistance or IC in the same ubication that the MOSFET but in botton plane?

\$\endgroup\$

2 Answers 2

1
\$\begingroup\$

If you would have signals that require impedance matching (USB, Ethernet, antennas...), the usual way to achieve a continuous impedance is to put the signals on outer layer and a continuous GND plane on the next layer to it with 0.1-0.25 mm separation between the layers.

Having a continuous ground path next to any signal will provide a low inductance path for the return current, thus improving EMI performance.

If you have components that dissipate a lot of heat, you want to separete them from components that are sensitive to heat (Electrolytic capacitors, sensors...). And make sure the total dissipated power does not heat the nearby components above their specified temperature range.

The components are usually taking use of the PCB for heat dissipation, if that is the case, then having "heaters" on both sides of the PCB would add up.

Excessive heat will also raise the temperature of the tracks, which causes voltage drop and possibly more heating, depending on the circuit.

High current tracks on outer layers can dissipate heat to air, so the same amount of copper can deliver more current. Return path for the current is likely the GND plane. GND plane might also serve as a heat sink. If you need to dissipate a lot of heat in the ground plane, you need to bring that to the outer planes too. You can conduct heat through the PCB by placing vias to provide a thermal path.

So in short, if the MOSFET, resistor etc power dissipating components dissipate their heat to the PCB, then having them on opposite sides of the board does not help as they try to dissipate the heat to same body.

\$\endgroup\$
3
  • \$\begingroup\$ Can I put a plane gnd in multiples layers? \$\endgroup\$ Dec 13, 2022 at 20:25
  • 1
    \$\begingroup\$ Yes. Often two sided routing is required for the critical signals so the layers should be SIGNAL-GND-GND-SIGNAL in 4-layer board. The GND layers need to be continuous near the high speed signals. \$\endgroup\$
    – Ralph
    Dec 13, 2022 at 20:52
  • 1
    \$\begingroup\$ If you've only got UART and PWM, it sounds like carrying power in outer layers and using the inner layers for signals would be completely fine. \$\endgroup\$
    – Ralph
    Dec 13, 2022 at 20:57
1
\$\begingroup\$

I have found out that the tracks with high current must be in a external layer

They don't have to be, you can route them on multiple layers, the more layers the better because they'll share current. The trick is not to have so much resistance that it heats up too much. Use a PCB trace calculator to find out what is acceptable. Keep in mind that you can also have higher copper weights, usually this will increase the cost of the PCB so talk to a PCB manufacture for their stack-ups.

Lets say you have a trace that is 100mil wide and 1000mil long with 1oz copper and a 6A current. This will have 3.1mΩ of resistance. This would create ~100mW of power dissipation and about a 20C temp rise. The same trace from 2oz copper will half the power dissipation or 50mW and about a 10C temp rise.

For example the MOSFET connected to MT1_2 is in top plane, is a problem if I put a resistance or IC in the same ubication that the MOSFET but in botton plane?

Yes, you will have less temperature dissipation if the traces are getting hot and with components close together. These are harder problems to figure out. In the power dissipation calculations of the mosfets, use the max trace temp (which might be close to 20C worst case if your trace is the same as the example above) for the ambient temperature of the mosfets and see if the temperature calculations are OK

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.