Removing ground planes under small capacitors

I just did something like that with an OPA355 photodiode amp. I put cutouts under the RC feedback path, and the photodiode and it's pin which connects to the opamp.

I've done it on larger circuits but not 0402s.

When making a crystal oscillator, it often makes sense to move the ground to the bottom of the PCB. PCB material doesn't make very good capacitors. They drift more than NPO/COG.

When making very high impedance circuits, the capacitance to the ground plane can be too low of an impedance to allow in the circuit.

You really want to reduce the capacitance at the input pins. The feedback resistor and this capacitance create a pole that can cause peeking or oscillation. To prevent this oscillation, the op-amp's compensation must reduce the bandwidth.

The output pin of an op-amp has a lowish open loop impedance so the capacitances here have less effect.

Hello Joel,

For high-Q resonant circuits and for high impedance nodes such as the collector or drain of an RF transistor I do. For decoupling or RC filters I don't. Also not on controlled impedance traces where the cap serves as a DC block (such as in T/R switches). However, the actual size of the cap doesn't really matter in those decisions.

Same if you didn't void the plane under the parts in the collector/drain path of an RF stage. On stuff in your frequency range you can see a noticeable drop in bandwidth if you don't.

I measured some FR4 at +950 ppm/K. I wonder what the prop delay tc is like... I guess I should measure that some day, too.

John

Hi Joerg,

Thanks for your feedback...

This is a standard LC filter (50 ohms) with various LC series and parallel resonators; I'm tempted to try a layout both with and without the ground plane judiciously removed and see what happens.

Agreed -- I've noticed that if all you're after is a DC block, you can typically get away with some awful 100nF cermaic cap that costs under a penny and the various parasitics will often do nothing but help make the path look like more of an RF short. (Seeing the effect of SRF on an S21 plot usually takes some effort, and it helps a lot if you've cheated and measured the SRF previously so that you know where to look. :-) )

---Joel

Hello Joel,

You could keep the area underneath the ground plane void of traces and use one layout. Then take one board and mill away the plane. Or, if you are really daring, chip it away with a Rotozip or Dremel grinder (but be careful...). Another option is to use thermal relief type connections at, say, two sides where there is nothing on the other side you could hit. Then grind these away with a little diamond disc.

Normally yes but that often doesn't work in T/R switches. There you have to trade off between switch transients (often called ringdown) and mismatch at the low end of the RF band.