Maker Pro
Maker Pro

Removing ground planes under small capacitors

J

Joel Kolstad

Jan 1, 1970
0
Does anyone around here bother to have the ground plane underneath, say, an
0402 capacitor removed? I ran through some numbers, and it looks like you can
easily end up with something in the ballpark of many tens to the low hundreds
of femtofarads by not doing so -- if your "circuit" capacitors are only in the
couple pF range anyway, this seems like it could be significant. I'm
operating the hundreds of MHz ballpark, so I'm not too worried about
"non-lumpedness" yet by doing this.

I've seen data sheets such as that of the Analog Devices AD8045 1GHz GBW
op-amp suggest removing the ground planes from underneath the input and output
pins to avoid creating a pole that might noticeably reduce the device's GBW...

Thanks,
---Joel Kolstad
 
C

Chris Carlen

Jan 1, 1970
0
Joel said:
Does anyone around here bother to have the ground plane underneath, say, an
0402 capacitor removed? I ran through some numbers, and it looks like you can
easily end up with something in the ballpark of many tens to the low hundreds
of femtofarads by not doing so -- if your "circuit" capacitors are only in the
couple pF range anyway, this seems like it could be significant. I'm
operating the hundreds of MHz ballpark, so I'm not too worried about
"non-lumpedness" yet by doing this.

I've seen data sheets such as that of the Analog Devices AD8045 1GHz GBW
op-amp suggest removing the ground planes from underneath the input and output
pins to avoid creating a pole that might noticeably reduce the device's GBW...

Thanks,
---Joel Kolstad


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.


--
Good day!

________________________________________
Christopher R. Carlen
Principal Laser&Electronics Technologist
Sandia National Laboratories CA USA
[email protected]
NOTE, delete texts: "RemoveThis" and
"BOGUS" from email address to reply.
 
K

Ken Smith

Jan 1, 1970
0
Does anyone around here bother to have the ground plane underneath, say, an
0402 capacitor removed? I ran through some numbers, and it looks like you can
easily end up with something in the ballpark of many tens to the low hundreds
of femtofarads by not doing so -- if your "circuit" capacitors are only in the
couple pF range anyway, this seems like it could be significant. I'm
operating the hundreds of MHz ballpark, so I'm not too worried about
"non-lumpedness" yet by doing this.

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.
I've seen data sheets such as that of the Analog Devices AD8045 1GHz GBW
op-amp suggest removing the ground planes from underneath the input and output
pins to avoid creating a pole that might noticeably reduce the device's GBW...

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.
 
J

Joerg

Jan 1, 1970
0
Hello Joel,

Does anyone around here bother to have the ground plane underneath, say, an
0402 capacitor removed? I ran through some numbers, and it looks like you can
easily end up with something in the ballpark of many tens to the low hundreds
of femtofarads by not doing so -- if your "circuit" capacitors are only in the
couple pF range anyway, this seems like it could be significant. I'm
operating the hundreds of MHz ballpark, so I'm not too worried about
"non-lumpedness" yet by doing this.

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.

I've seen data sheets such as that of the Analog Devices AD8045 1GHz GBW
op-amp suggest removing the ground planes from underneath the input and output
pins to avoid creating a pole that might noticeably reduce the device's GBW...

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.
 
J

John Larkin

Jan 1, 1970
0
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.

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
 
J

Joel Kolstad

Jan 1, 1970
0
Hi Joerg,

Thanks for your feedback...

Joerg said:
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.

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.
Also not on controlled impedance traces where the cap serves as a DC block
(such as in T/R switches).

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
 
J

Joerg

Jan 1, 1970
0
Hello Joel,

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.

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.
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. :) )

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.
 
Top