Characteristic impedance of combination of CPWG and stripline on inner layers

Hi everyone,

I have been searching for quite a while about the following subject, but can´t seem to find a decent answer on this. Imagine a 4-layer PCB (Top layer, Mid1 layer, Mid2 layer, Bottom layer). Mid1 layer and Bottom layer are GND panes with here and there vias to pass signals from the top layer to the Mid2 layer and back. RF signals on the top layer are done using CPWG. RF signals on the Mid2 layer are done with stripline or - and now comes the tricky part - striplines surrounded by GND planes as well. My question louds: What is the characteristic impedance of these kind of RF lines? Note that these kind of RF lines are no ordinary striplines, but rather striplines + surrounded by GND Planes at both sides, so similar to a CPWG, with GND plane also above the RF line. I have add two images to clarify.

Thanks and best regards
Simon

The embedded CPWG (second picture) is covered by some calculation tools, e.g. Polar Si6000 and Si8000. Specific inductance and capacitance can be also calculated with 2D solvers like Quickfield Student.

Via fences are generally required to avoid unwanted wave modes, hence the point involved with figure 1 versus 2 isn't if you have vias but how close they are. The figure 1 vias are still in the coplanar ground "slipstream" and won't change impedance much. PCB thickness variations probably matters more.

If you want exact modelling of a specific PCB geometry, a general 3D solver or planar specific solver like ADS Momentum would be necessary.

FvM said:

Via fences are generally required to avoid unwanted wave modes

Click to expand...

Yes exactly. By leaving out those vias, your various "ground" metals are unconnected and can be start to have unwanted potential here and there ... causing all sorts of resonance and strange behaviour. Then it's no longer "all ground" but instead all different conductors that are only connected somewhere far away. Don't do that!

You don't need to create a via fence, but make sure all grounds are connected at distances closer than lambda/10 wavelength (wavelength in PCB medium, not air)