Implementation of a coplanar waveguide in the design of a Butterworth filter
Can those soft curves on the upper ground plane that KiCad adds automatically around the pads of the capacitors affect the behavior of the waveguide?


Above 10 GHz, they might.

In Altium I can add a "keep out" to prevent these features from being produced. You should be able to do something similar in KiCad.


  Have I added too many viases around the signal line? And are there enought viases all over the rest of the board? I am a bit lost about viases


You can't really have too many vias. If you are not trying to save fractions of pennies, I wouldn't worry about too many vias.

The issue I would worry about (for a 10 GHz design, not for 100 MHz) is that where you tee your line to connect to the shunting LC components, you break the coplanar geometry. Without more analysis I couldn't say what frequency that will start to affect your performance, but at some point it will.


  Thank you for the comments and answer, I have edited my design to this new PCB:


Ideally, don't make stubs to connect the L and C. Just put their pads right on the main signal trace. Allow the ground to fill in under the part so you maintain your 0.49 mm from the trace to ground.

Spread out C1, C3, and C5 if you have to to make things fit.

Doesn't particularly matter if you have L on one side of the trace and C on the other (assuming you can fit two pads on the trace without changing the trace width), or both on the same side of the trace.