# Coplanar waveguide with GND Vs. microstrip general rules

I have been fiddling around with GPS antenna trace impedance matching. I have only Saturn PCB SW to make some calculations.

I can't quite get it when microstrip starts to behave more like a coplanar waveguide. If I calculate trace as a microstrip then 0.15mm trace on top of GND plane with 0.1mm FR4 in between yealds about 50 ohms. However in practical situation there are almost always some coplanar copper plane quite close to the signal trace.

How long distance away could be considered enough to coplanar plane not to contribute to the trace impedance?

In Saturn PCB trace impedance is still changing in coplanar waveguide calculations even if I increace coplanar plane gap to trace to 1 meter. That does not make any sense in practical implementations. There will be always some conductive planes quite close proximity of the antenna trace in PCB designs and I assume that there might be some rule of thumb value when plane could be considered to be distant enough.

Second question is that is it always needed that coplanar plane (top) to be stiched with vias along the edges to the reference plane (L2)? Some presentations of the coplanar waveguides are without those vias and some of them are presented with those vias.

For most microstrip on FR4 figures I've seen, a w/h ratio of 2 gives about 50 ohms.

Once grounded traces/walls are 3 substrate thicknesses away from the track, their effect on the impedance becomes insignificant, for most purposes.

You might want to be slightly further away for precision work, but if you're on FR4, you're not doing precision work. Plug in the tolerances for FR4 Er into your line impedance calculators to get an idea of what changes in impedance are significant.

Co-planar doesn't have anywhere to be stitched to, perhaps you mean CPWG, Co-planar with ground? This is a convenient geometry to describe co-planar with a ground plane, microstrip with side walls, and as an intermediate structure between microstrip and co-planar.

If the ground return happens symmetrically on all top and bottom ground planes when a signal is launched into the line, then vias are not needed. However, that's rather theoretical, as complete symmetry is difficult to achieve, and after a little distance, even the best line may have modes travelling differentially between any of the 'grounds'. It's these modes that vias are intended to suppress. Depending on what you have connected to these lines (sensitivities, generation of harmonics etc), these extra modes may be insignificant, or spell disaster.

Of course, where CPWG is being used to convert microstrip to co-planar, or microstrip to a coaxial connector on the edge of the board, these vias are vital to carry the ground currents as they move from one plane to the other.

• Thanks. I thought that there would be some rule as you mentioned. As mentioned in the first post my antenna trace width from GPS module to antenna connector is 0.15mm on top of 0.1mm FR4 and solid GND below. This gives 51 ohms. Which I think is good enough. However if I change from microstrip to coplanar wave in Saturn PCB and enter my isolation distance of 0.5mm from coplanar plane to trace it will give impedance of 60 ohm. That made me question if my 0.5mm clearance from antenna trace would be enough. Commented Oct 18, 2023 at 7:39