I am building a sensorless ESC which uses low-side shunt resistors to detect current. Good practice dictates that traces of equal length and width be connected from the pads of the shunt resistor into the microcontroller, differential amplifier, etc., like in this picture. (my FET driver has a built-in diff amp). Current sense resistor traces

I did this in Altium, but since the negative terminal of the shunt resistor is connected to ground, when I added a polygon pour ground plane, Altium decided to connect the trace to the plane, like this. Current sense traces connected to ground plane (I highlighted the original trace in Altium to make it obvious.)

Is there a way to avoid altium connecting the polygon pour to the trace?

Ideally the trace itself would be separate from the ground plane, but the other three sides of the solder pad (where the trace isn't) would still be connected to the ground plane.

  • 1
    \$\begingroup\$ I like to use net ties for kelvin connections, so that the trace isn't seen as the same net. But I don't know Altium. \$\endgroup\$
    – Hearth
    Commented Jun 17, 2021 at 14:43
  • \$\begingroup\$ I used Altium some years ago. It seems to me that, for this kind of problem, i wired myself these type of lines. Then making wiring these lines definitive. So auto-router did no changed it anyway. I am now perhaps wrong. \$\endgroup\$
    – user288518
    Commented Jun 17, 2021 at 15:12
  • \$\begingroup\$ I did wire the line myself, that's the whole point. I'm trying to get the ground plane to realize this and not overwrite what I already did. \$\endgroup\$
    – user289193
    Commented Jun 17, 2021 at 15:18
  • \$\begingroup\$ Another approach: use a 4- or 6-pad footprint, and read up on how to design it to produce minimal error. Your layout certainly may be sufficient, but if you want a free improvement in performance (since a PCB with poor layout is no cheaper than one with good layout) - there's a paper/app note somewhere about it so if you trust it, you don't need to do much in the way of experimentation :) \$\endgroup\$ Commented Jun 18, 2021 at 18:32

2 Answers 2


You need to change the net connection rules of your ground pour. Select the ground plane -> Properties panel. Select some option other than 'Pour Over All Same Net Objects'.

You can also create a 'Polygon Pour Cutout' (Place->Polygon Pour Cutout) around that trace, as changing the above rule might cause things to not connect to the ground pour nicely throughout the rest of your board.


There are a few other ways to separate out connections.

One is a net tie

The other is a keepout trace

  • 1
    \$\begingroup\$ Net tie is the way to do it. Net ties were created for situations like this. \$\endgroup\$ Commented May 2, 2023 at 22:48
  • \$\begingroup\$ I usually use net ties, the only problem I have is sometimes they get in the way when you have traces packed together. \$\endgroup\$
    – Voltage Spike
    Commented May 3, 2023 at 4:17

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.