I have been designing RF PCBs for a year for an RF front-end system.

One of my PCBs has very strict constraints about its size measurements. So, I should design it very densely.

The problem with this PCB is that there is a microstrip line so close to a GND mounting via as can be seen from the figure.

enter image description here

Also, I should use the copper zone due to GNDs of capacitors, inductors, ICs etc. So I cannot delete the GND copper zone around there.

I used Rogers4350B with the thickness of 30MIL. So, microstrip line's width was calculated as 1.65mm. This line comes from a coupler topology, so I cannot change the line from microstrip to coplanar line.

My question is: How far the copper zone can get closer to microstrip line without deteriorating the microstrip line topology?

Is there a rule of thumb about these kinds of problems?


1 Answer 1


Where the proximity to a ground conductor only happens for a short length of track, a small fraction of a wavelength, you can regard it as an extra lumped capacitance to ground.

Depending on the quality you need from the track, you can ignore it, or you can thin the track down at that point to make it a little inductive, which turns the shunt C into a lowpass filter. There are two ways to determine how much to thin the track. (1) Go full FEMM on it and (2) shave a bit off with a scapel, and measure, and repeat. You might find you haven't the resolution to measure the difference it makes, in which case you can ignore it.

This technique is the same as what you are already attempting to do, incorrectly, with the corner going into the component. When a microstrip turns a corner, the bend has an excess capacitance to ground, which is compensated by cutting a mitre across the bend. You have not cut enough off, so your track will already be a little low impedance anyway due to the bend. See this answer and this tutorial for more about mitred bends.

An alternative way to look at is this. The line is coplanar plus ground at that point, whether you don't want to change to coplanar or not. When you look up the dimensions, you'll notice that for the same substrate thickness, the centre conductor for CPW+ground is narrower than for pure microstrip. Narrow it down at that point to the correct CPW+G dimensions, and a little more as the line geometry is changing. (Back in nineteen hundred and frozen to death, an extension of the centre high impedance conductor when you connected two transmission lines of different sizes was called a Krauss Step, a little extra inductance to tune out the extra capacitance caused by the discontinuity, but can I find any reference to that now? Nope. Any help with a link from ancient RF engineers welcomed.)

As a side note, I'll wager that the discontinuity you get transitioning into and through PLD is larger than you get from the encroachment of the ground screwhole.

  • \$\begingroup\$ What is a Krauss step? @Neil_UK \$\endgroup\$ Commented Feb 17, 2020 at 10:44
  • \$\begingroup\$ @AldrichTaylor I presume you've googled for it. So have I, and not found it yet. It's an extra bit of high impedance line used to tune out the extra capacitance you get when changing between two lines of the same impedance but different dimensions or configurations. It was so much used when I started microwave work, I thought it would be easier to find. It's probably in Zverev, but I don't have a copy to hand. I was hoping somebody would pick it up and link to it. I might not have spelt it correctly. \$\endgroup\$
    – Neil_UK
    Commented Feb 17, 2020 at 11:41
  • \$\begingroup\$ Is the Krauss step related to Kuroda's Identities? \$\endgroup\$
    – Mast
    Commented Feb 17, 2020 at 18:56
  • \$\begingroup\$ @Mast No, thanks for looking though. \$\endgroup\$
    – Neil_UK
    Commented Feb 17, 2020 at 21:23

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.