I am routing differential pairs in Altium 20 and using controlled impedance profiles. I am using microstrips on external layers only.

Impedance Profile Type List

For instance, I want a 100 Ω controlled impedance pair, and have used "differential" before which seemed to work fine. Because the traces are together on the same layer (plane) I'm not sure how "coplanar" differs. Information on Altium's page about this is not really clearing it up for me.

What's the difference between "differential" and "differential-coplanar?"

With "differential", selecting the top layer provides this properties panel:

Differential Properties

Using "differential-coplanar", selecting the top layer provides this properties panel:

Differential-Coplanar Properties

I've always manually created a DRC rule to keep the ground pour on the same plane away from the differential trace by some amount. It appears that the coplanar option specifies a clearance (S) which aims to do the same thing. (Although the value provided is smaller than expected.)

  • \$\begingroup\$ In my mind, co-planar is just a specific type of a differential pair on a PWB, one where the two traces are in the same plane. From my experience, this is the most common geometry used for diff pairs. \$\endgroup\$
    – SteveSh
    Jun 29, 2021 at 19:26
  • \$\begingroup\$ @SteveSh I've only ever seen them in the same plane, so perhaps I should use coplanar. But that still leaves the other option as unclear or unknown to me. \$\endgroup\$
    – JYelton
    Jun 29, 2021 at 20:48
  • \$\begingroup\$ Do they mean "coplanar waveguide" as opposed to microstrip or stripline? Can you try and see what it does? \$\endgroup\$
    – Matt
    Jun 29, 2021 at 21:09
  • \$\begingroup\$ @Matt I've added images showing the properties of either choice, along with comments. \$\endgroup\$
    – JYelton
    Jun 29, 2021 at 21:45

1 Answer 1


The coplanar option designs a grounded coplanar waveguide structure. In this design there is a coplanar ground plane a controlled distance away from the trace that is close enough that it significantly affects the impedance of the trace. See how in your microstrip example the traces are 192 um wide while in the coplanar design they are 117 um wide. This difference is to compensate for the extra capacitance to the nearby coplanar ground. For this reason it is different than just setting a design rule to keep the ground pour away. If you let the ground get this close to the traces you would mess up your controlled impedance. See how the gap between the traces is the same as the gap to the coplanar ground. This should be much closer than your normal ground pour design rule would allow.


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.