I’m trying to do an RF design. I’ve got a dipole antenna with an SMA connector. I was wondering if I should separate the RF Ground from the analog and digital ground.
I know it is good to separate digital and analog ground planes and connect them with a small trace. Is this the same approach that should be taken for the RF ground?
These days having separate or split ground planes is generally frowned on - you are normally better off segregating analog and digital sections of the board, and watching your ground return current paths.
However, sometimes separate / split analog-digital-RF ground planes are recomended - eg the datasheet for the AT86RF231 from Atmel, where they recommend this on page 13:
http://www.atmel.com/dyn/resources/prod … oc8111.pdf
“The ground plane of the application board should be separated into four independent fragments, the analog, the digital, the antenna and the XTAL ground plane. The exposed paddle shall act as the reference point of the individual grounds.”
If you do split the ground plane you must be VERY carefull not to have ANY traces crossing the ground plane over the split. All traces between different sections MUST pass over the section of the groundplane where the different sections meet.
Have a look at how this is implemented on page 2 and 5 of the following design note, and notice how no traces cross any of the splits in the ground plane:
www.atmel.com/dyn/resources/prod_documents/doc8092.pdf
Actually, this isn’t strictly true - notice that the small “analog section” of the ground plane has it’s power supply crossing the split. However, they have used a small inductor that straddles the analog and digital sections, which serves to provide a filtered analog supply, as well as limit the rise and fall time (and hence generated interference) associated with any ground return signals corresponding to that power supply connection.
Thanks for the great reply, that’s very helpful. What about power planes. Is it good to use a power plane if you have multiple layers to work with.
I had seen some recommendations to alternate signal / ground / power layers in design with 4+ layers. However, I’ve also seen some comments that power planes are not necessary as long as you have a ground plane and they might actually cause problems.
I guess the nice thing is that you can drop a via right next to a power pad.
In general, having a power plane is a good idea if you can afford to go to a 4+ layer PCB. At RF frequencies it appears like a ground plane, and it can really help control EMC. It’s a good idea to have a ground or power plane separating signal layers in a PCB to control crosstalk.
For very high speed digital circuits, some board places can make the PCB with a very thin dialectric layer between GND and power planes, which provides “distributed capacitance” that improves the performance over just having bypass capacitors.
You would just have to be careful if you’re trying to split the ground plane as described above, since the same rules would apply.
So in cases where only 2 layers are used is the best approach to use a ground plane on the bottom and fat power lines snaking through the design? Or should there be power islands/planes on the top side?
Normally when I only use 2 layers, the top layer is very full of signal traces, but I try as hard as I can to minimise any tracks on the bottom layer. I don’t always succeed, so I normally pour ground on the remaining free space on the top layer and put a bunch of vias to bond top and bottom planes together to minimise the ground impedance. And yes, It’s good to make the power traces as wide and short as you can.
If you manage to have a pretty decent groundplane on the bottom layer (without many breaks in it), you may like to pour the top plane as power, so you can minimise the impedance of this too.
According to MichaelN, summarizing:
Electrical separation = Mechanical separation in 99% of the cases.
Mechanical separation != Electrical separation. That’s why to split planes is frowned on, and if you “break” some return current, this solution becomes a fatal disaster.
When you’re designing a board, always try to think electrically imaging the return current path. The more you separate all the return currents, the better ground planes are split.
noether, I’m not quite sure I understand you.
Split ground planes can be made to work well, but if you aren’t careful they can cause big problems.
In most situations, CAREFUL SEGREGATION of the PCB into analog and digital “zones” and a single, unbroken groundplane will give good results. If you need very low noise, go for a split ground pane, but be very careful about ground return paths.
MichaelN:
noether, I’m not quite sure I understand you.Split ground planes can be made to work well, but if you aren’t careful they can cause big problems.
In most situations, CAREFUL SEGREGATION of the PCB into analog and digital “zones” and a single, unbroken groundplane will give good results. If you need very low noise, go for a split ground pane, but be very careful about ground return paths.
100% agree xD, that’s what i tried to explain.
If you split a ground plane (mechanically), you have to be very careful about ground return paths.