I'm attempting to calculate the necessary trace width of a PCB transmission line in order to have a characteristic impedance of 50ohm. However, different online calculators are giving me slightly different results.

My PCB substrate is FR408 from OSHPark. So, the dielectric at my 5-6GHz frequency range is 3.66, the trace height is 1.4mil and the dielectric thickness to the first intermediate layer (this is a 4-layer board) is 6.7mil.

This Mantaro calculator tells me that I need a trace width of 11.98mil. Chemandy on the other hand tells me 14.72mil. 3mil seems like a substantial enough difference. Is one of these calculators more accurate than the other, or should I use a different equation altogether?


Looking at the equations, Chemandy provides an explicit calculation for the effective dielectric (due to the fact that one side of the microstrip is adjacent to air, as explained here), whereas Mantaro does not. If I use the effective dielectric provided by Chemandy with the Mantaro calc, the difference between the results roughly halves, but does not disappear. This might explain part of the discrepancy, but is not a full explanation (and still does not specify the right equation to use).

The reason provided in the edit is incorrect. I found the exact equation Mantaro uses in High Speed Digital Design by Johnson, where he explicitly states it takes into account the effective dielectric.

  • \$\begingroup\$ Are you planning on a microstrip-design, or a coplanar waveguide? \$\endgroup\$
    – Araho
    Jan 15, 2019 at 18:31
  • \$\begingroup\$ A microstrip design. \$\endgroup\$
    – MattHusz
    Jan 15, 2019 at 18:32
  • 5
    \$\begingroup\$ FWIW, Saturn gives 48.7 ohms with 14.7 mil trace width and 54 ohms with 12 mil width. You might get a somewhat more definitive result if you can get access to Polar or Ansys HFSS. But given the uncertainty about the actual Dk, possible etching variation, possible thickness variation, etc., probably anywhere between 12 and 15 mils trace width will give you as good results as you can hope for with a shop that doesn't directly support controlled impedance.. \$\endgroup\$
    – The Photon
    Jan 15, 2019 at 19:40
  • 1
    \$\begingroup\$ (If OSH Park does support controlled impedance, then just let them adjust the width as required) \$\endgroup\$
    – The Photon
    Jan 15, 2019 at 19:40
  • \$\begingroup\$ Since it sounds like you found an answer, could you post it as an answer and mark this question as answered? Thanks. \$\endgroup\$
    – TimWescott
    Jan 29, 2019 at 21:52

1 Answer 1


It looks like two simulators you used bracket the value given by FEM simulation of the stackup described in the OSHPark documentation.

Impedance vs Width

Here is a simulation of the characteristic impedance of your microstrip structure swept over trace width.

You should remember, as some of the comments on your question point out, that there will be some variation in the geometric parameters of your board during fabrication including changes in line width and prepreg thickness.

  • \$\begingroup\$ This is really useful, thanks for posting this. It still doesn't quite explain the discrepency between the various sources, but maybe the answer to that is this is really a task for a simulator and not approximate equations. \$\endgroup\$
    – MattHusz
    Jul 25, 2019 at 4:27

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.