1
\$\begingroup\$

I'm designing this board which will control current through a coil using an IGBT. The coil is 500 uH and is mounted around 3 cm above the PCB and will handle peaks of 400 A. Because of the close proximity to the board and the large magnetic field strength at peak current I'm worried this will affect the gate signal for the IGBT.

enter image description here

enter image description here

As above the gate signal runs from the connector through R2 to the gate of Q1. The top plane is GND. I'm restricted by the connector position and board dimensions. I realise the signal trace is pretty long and so it has more inductance than what would be ideal I'm assuming. So are there any other methods I can use to reduce EMI from the coil during turn-on aside from reducing trace length?

\$\endgroup\$
8
  • \$\begingroup\$ I realise the signal trace is pretty long What are the lengths of each segment of the gate trace? \$\endgroup\$ Nov 15, 2023 at 8:36
  • \$\begingroup\$ One more thing: The coil ... will handle peaks of 400A but your IGBT can't. Check the SOA graphs. Regardless of the pulse width the peak current is limited to ~110 Amps. \$\endgroup\$ Nov 15, 2023 at 8:40
  • \$\begingroup\$ The top plane is GND this doesn't make sense when you only appear to have one puny track on the underside. \$\endgroup\$
    – Andy aka
    Nov 15, 2023 at 8:44
  • \$\begingroup\$ Sorry ignore the IGBT part number in the schematic it's not the actual one I'm using I just needed one that was in TO-247 package in Altium's library. I'm using IXXH80N65B4. Trace lengths following from the connector to resistor are; 4.7, 3.7, 10.3, 10.8, 3.4 giving 32.9mm total. \$\endgroup\$ Nov 15, 2023 at 9:17
  • 1
    \$\begingroup\$ I also can see a few design issues here (I can't use the word flaw as you are space- and placement-limited). 1) If the connector to the bottom-right (J2) indeed carries 400 VDC then the traces seem to be too close for that level of voltage difference. Same for COIL to the top-right. See IPC standard(s) for details. 2) If possible, try to route the high voltage (or high current) return trace (IGBT's emitter) separately to J2 because the small-signal ground uses the same plane. Just to prevent some potential issues. \$\endgroup\$ Nov 15, 2023 at 9:19

2 Answers 2

1
\$\begingroup\$

From comments:

what determines the frequency of the propergating wave from the coil since it's only a pulse? Is it the rise time of the IGBT gate?

A coil over a board gives us an EMI equivalent circuit of a loosely-coupled transformer, where the coupling factor depends on the relative distance and orientation, and the inductances are the coil itself and the total stray inductance of the trace, IGBT pins, connector and wiring.

Thus, the important part is not the current, but the voltage, and volts/turn. Voltage is induced ~instantaneously, coincident with change in collector voltage. A little feedback to the gate circuit won't matter (presumably, you're driving VGE(on) high enough and VGE(off) low enough, relative to VGE(th), that a volt here or there makes no difference), but a lot could cause oscillation, or damage outright.

The frequency content, or transient response, will have various time constants due to the PCB ground plane (the self-inductance of the trace increases as frequency decreases, because magnetic field is able to penetrate the surrounding ground plane over time), and any other surrounding metal, and these will have impedance terms for which the coil current will matter. The bulk of the interference route will be the instantaneous transformer action though.

Don't ignore the emitter inductance and PCB plane / return path, either. TO-247s don't exactly give good Kelvin connections so as to separate these paths; the emitter pin will always be common to both, and this coupling depends on IC as well as dIC/dt (the rate of change). (Having the gate and collector paths on opposite sides of the device, as you do here, is probably about as good as you can do on PCB.)

As for coupling in general, the simplest solution is the non-solution: don't worry about the board, slap a trick metal plate inbetween them instead.

Copper is an effective shield for AC, and steel (or with mu metal if you need really low levels) for DC.

Steel is good at AC as well, as a shield, but depending on what you're doing with the coil, it might not be the best option. For example, it will get quite hot if the repeat rate / duty cycle is more than a little.


Putting active circuitry directly behind a pulse coil doesn't sound very smart; not to say there might not be reasons to do so, but I have a sneaking feeling that there is more work that could be done here, that goes beyond a mere PCB. You may wish to ask another question about your project, providing ample details of its purpose, the mechanical layout as-is, and what constraints drive the layout and component values.

\$\endgroup\$
0
\$\begingroup\$

To keep the noise out keep it short and put a ground plane under it, (or between it and the noise source),

Here ground would be your IGBT emitter.

If practical rotate the IGBT 180 degrees and swap the "sig" connector terminals too,

double check those spacings, your 400V terminals (and conductors) look awful close to each other.

\$\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.