0
\$\begingroup\$

This is my first high power PCB. I have been doing some reading and going through few reference designs. really looking for some guidance from the community. Please do correct me and if possible point me at the right direction.

Lot of people has suggested for 70um or 2ounce copper. I personally want to avoid it if possible and use any existing PCB Stackup from JLC PCB 4 layer stackup with standard FR-4.

Also my stack up plan is to keep [1.SIG TOP| 2. GND | 3. POWER | 4. SIG BOT].n

The layout keeping the digital and analog grounds on the same ground plane with decent separation.

The board has to drive a 3 phase BLDC motor.

  1. I was planning on keeping control board (TMC 4671) and the gate driver with power MOSFET on a separate board connected using a board to board connector. Should I do it on single board?
  2. Usually design guides recommend lots of vias while routing in between planes. for the power MOSFET. What is lot and how can I calculate it?
  3. I am using vias with 0.45mm diameter and 1.6mm height. I am not sure what should be the height should I assume board thickness from top layer to bottom here?
  4. Should I use thermal relief vias for the MOSFET? If yes how can i use and also where to decide to put thermal relief vias?
  5. Planning for a 2mm trace with standard FR4 dielectric and minimum conductor space of 0.6-0.8mm. Is the conductor spacing and trace enough since 100A (assuming less than 5A continuous)?
\$\endgroup\$
1
  • \$\begingroup\$ 1. I would not. 2. Depends, are you using SMD or THT? What solder process are you using? 3. 1.6 mm is very common. 4. Depends on your production and service process. Is your solder process ok with no thermal relieves and you don’t plan to do any service with a regular soldering iron then you don’t need any reliefs. 5. Depends. How long is that 200 A pulse? \$\endgroup\$
    – winny
    May 12, 2021 at 16:41

1 Answer 1

5
\$\begingroup\$

You are using a standard 35µm 4-layer stackup, which is fine. Signal/power/power/signal is also quite common. Digital and analog plane on the same layer is fine even without lot of separation.

Now, for the questions: the control board is often separate (plugged in vertical in many design) to better isolate the controller from the switching noise. Also with heavier copper you need greater clearance so you couldn't solder a fine pitch controller: already at 70µm copper clearance become 0.2mm so a 0.5mm pitch component starts to be problematic. If you can fit your controller/drivers on the main board it's simply cheaper (one board less to make)

Lots of vias: you are talking about thermal vias: they spread the heat between planes. For a price they also can fill them with thermal compound. The 'lots' is really an empirical issue. I use 2-2.5mm spacing for example with 0.3mm vias. There is some literature on the effectiveness of thermal vias but it's trial and error most of the time. If you are rich there is thermal simulation software, never used it however.

1.6mm is the typical thickness of the board. Yes, usually vias go from top to bottom unless you are doing high density interconnects with blinds and embedded vias. Very expensive, don't even think about them. The value could be useful for estimating via inductance but I don't think it's needed in this application. I simply never heard talking about via height…

Thermal relief for MOSFETs depends on your assembly process. It's a compromise: without relief you have better dissipation but it can be problematic to solder them properly. Most of the time is better to relief the pads. Also remember to reduce the paste area from the big pads to avoid outgassing issues: the datasheet should give indication for that (often for thermal vias too).

As for the trace width/clearance: you didn't specify the single most important parameter for spacing, the working voltage. There are tables with clearance and creepage to be used. If it's a very low voltage motor it seems fine. As for the trace width you have to decide how much the board can heat up: it depends on the enviroment and other things. For 5A 2mm is usually enough, you can find the calculators on the net. The bigger the better anyway. For the 100A surge it's more difficult, it depends on the surge 'shape' (you literally have to integrate the energy to find out)

\$\endgroup\$
4
  • \$\begingroup\$ good answer, I agree with essentially everything said here. I'm a bit confused about your comment at the end about surge current though. What does the integral of energy correspond to physically? Did you mean integrate power to calculate energy, which could in turn allow you to roughly estimate the temperature rise in the copper? \$\endgroup\$
    – Ocanath
    May 12, 2021 at 17:10
  • 1
    \$\begingroup\$ Exactly that. It's the same I2s calculation used for fuses (in fact, a copper trace is a fuse you don't want to blow). Either that or find some empirical table or just put all the copper it fits and hope for the best. Unless you are doing high reliability and then you need to demonstrate with calculation and/or tests. If you have access to it, IPC-2152 Standard for Determining Current Carrying Capacity in Printed Board Design is the definitive guide (not free) \$\endgroup\$ May 13, 2021 at 5:52
  • \$\begingroup\$ hi sorry for the late reply, thanks for replying all my question i was desperately looking for some feedback i will make sure to keep note of these pointer, also the working voltage around 48V i used an online calculator to calculate the trace width and clearance. just a noob question how can i account for the 100A surge. \$\endgroup\$
    – ti-do
    May 15, 2021 at 16:41
  • \$\begingroup\$ for 48V your values are fine. The 100A surge need to be evaluated case by case, depending on the shape of the current waveform \$\endgroup\$ May 17, 2021 at 8:46

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.