Filling the unused space with ground plane in mixed signal pcb

Question

I'm designing a 4-layer pcb which consists of a GSM module, GPS module, a microcontroller (SAM4S) and a proper dc to dc buck converter.

The traces of the antennas are extremely short, fewer than 5mm long.

And the highest speed of signals is the SPI which I chose for external nor flash and/or a micro sdcard communication.

There are also few analog signals for monitoring very low frequencies (100 Hz in worst case).

I was thinking if it's a good idea to fill every unused space with ground plane stitching with vias (as if it's manufactured in cnc). I will not let any dead copper though.

Will this cause any problem in signal integrity?

Answer 1

Most of the datasheets I saw had a recommendation, how to use the ground planes around the RF IC.

• most of the chip/pcb antenna designs recommended no filling around the RF lines, similar to this one. Possible reasons: reduce parasitics, field-shaping, etc. Notice the stitching vias at the edge of the polygons. image source

• I saw some designs with external antennas, that used filling around the RF line. Here you have to take care of the characteristic impedance of your line. If your RF line is a microstrip on the surface layer, then your refence is usually one of the internal layers. Thus you have to take care, that the filling on the outer layer is coupled much less to your signal, than the internal layers. The recommendations I've read mention a clearance around 3-4x the distance to the reference plane. image source

So my recommendation is:

• check your datasheet recommendation or app. notes of the supplier
• if there is nothing regarding this, I would leave the area around the antenna empty (no components, no copper, nothing at all), but I would separate the non-rf part with a filling + stitching vias, in order to make wave propagation inside the pcb impossible + reduce EM emission of the DC/DC

PS: regarding digital signals - it is not the SPI frequency that matters regarding signal integrity, but the rise and fall times of those signals. Rule of thumb: if your track is longer than 1/10-th of the way the signal travels during the rise/fall time, you might get reflection issues.

Answer 2

Don't do that, unless you know exactly what for. Creating unexpected capacitance is always a bad idea, as all kinds of AC stuff (mainly from switching devices, but not only) will travel the most unexpected ways.

Actually what you should do is to channel ac stuff exactly the way you want.