Ground plane question

8BIT · Post by **8BIT** » Sat Jan 15, 2011 2:32 pm

I am working a 2-layer board with mixed analog and digital. There are several SMT IC's and I have created a ground plane on the top of the PCB that surrounds all of the components and ties all of the ground connections together.

I have several through-hole parts (resistors and capacitors mostly) and some traces on the bottom of the board also. The majority of the traces are on the top layer.

My question concerns created a second ground plane on the bottom of the board.

Should I add this second plane?

If so, should I tie it to the top plane at all the through-hole pads and Vias or possible just one common connection?

I'm not sure that having two seperate ground planes is a good idea.

My primary goal is to reduce circuit noise.

thanks!

Daryl

Arlet · Post by **Arlet** » Sat Jan 15, 2011 3:49 pm

On 2-layer boards I always have 2 ground planes, connected by plenty of vias, especially around areas where the ground planes are intersected by other traces.
The idea is to create an uninterrupted ground plane as much as possible, for current to flow back along the shortest route.

GARTHWILSON · Post by **GARTHWILSON** » Sat Jan 15, 2011 8:57 pm

What is the analog? Data converters & amplifiers, or switching power supply?

Either way, they should have their own ground plane, and you join any two ground planes only in one place, and have power-supply bypass capacitors (.01uF) right there at that spot. Bring all the I/O through as close as possible to where the ground planes are joined. Don't make traces go across the chainsaw line, ie, the cut that separates the ground plane areas. Putting a trace across that chainsaw line, away from where the planes are joined, makes an antenna. It will indeed transmit and receive, even though it's right against ground planes, because its return-current path is not immediately beneath it, so there's a loop, possibly with other components or traces inside the loop area. This is indeed how some cell-phone and Bluetooth etc. antennas are made. I should probably scan and email you some articles on it.

In digital work, you want, as much as possible, to have the return current for any given trace to run immediately under it, no farther away than the thickness of the board itself. (Note that that won't usually be the shortest return path, but it will be similar to a twisted pair of wires.) Obviously you can't do this where the signal enters and exits the IC unless every other pin were either power or ground; but the unavoidable loop should be as small as possible.

With SMT, it works best to have the non-component side as the ground plane. If you only have two copper layers, you might have to put short traces in the ground plane as jumpers since you're short on layers; but if you have to do it, make those jumpers absolutely as short as you can.

If you have an audio-only circuit (as opposed to mixed signal), with its higher impedances and low frequencies, the enemy is electric-field coupling, not magnetic, so a break in a ground plane there is not such a big deal. In digital however, with very high dv/dt and di/dt rates, as tempting as it may be to fill all the blank areas with ground fills, those don't really help any. They're not the right approach.

Switching power supplies are yet another animal. The dv/dt may not be as high as the digital stuff, but the di/dt is astronomical. The AC loops there must be kept absolutely as small as possible. Also, if noise getting into analog lines elsewhere in the boards could be a problem, double-filter the power supply's input and output with ferrite beads. Wound inductors alone are not enough, because they have capacitance between the windings and they have a resonant frequency beyond which they are capacitive, and they don't present a high impedance at all for the highest harmonics.

I have done only a little in board lay-out with A/D and D/A converters and with Bluetooth (2.4GHz), but a lot with switching supplies and digital on the same boards with audio for our products, and have been quite successful. A switching regulator we have used a lot is the MAX732 which uses a constant frequency and PWM, and, out of necessity, I've gotten the noise down to a fraction of how much is specified. Especially when the load drops down to a low current, the board layout becomes extra critical to keeping the controller behaving well such that the pulse widths aren't varying all over the place between cycles, or even skipping pulses, both of which causes low-frequency noise that wreaks havoc in audio circuits.

ElEctric_EyE · Post by **ElEctric_EyE** » Sun Jan 16, 2011 12:11 am

That is excellent info Garth!

I also read about joining an analog ground plane to another ground plane at one point only. I'll keep my eye out for the app note. It may have been Maxim, TI, or Analog Devices as I believe I was looking for info on ADC's and happened to read it...

8BIT · Post by **8BIT** » Sun Jan 16, 2011 2:44 am

The application is a composite video overlay circuit with an AVR controlling the overlay. The IC's are mixed analog and digital and are all SMT on the top layer. Most of the bottom is the Vcc power with a few digital signal traces that would not fit on top.

For the top ground plane, I have ensured there are no islands (unconnected to the ground source). I had originally figured on the one plane but was not sure if having the bottom side include a ground plane was good or bad. It sounds as if I should keep the top plane and remove the bottom one.

Thanks for the feedback.

Daryl

ElEctric_EyE · Post by **ElEctric_EyE** » Tue Jan 18, 2011 1:05 pm

Daryl,
Here's the info. It's on a data sheet for a National Semiconductor ADC I was looking at. I thought it was an app note. Anyway, lots of good stuff in there on Pg.17 "5.0 Layout and Grounding".

http://cache.national.com/ds/DC/ADC08L060.pdf

GARTHWILSON · Post by **GARTHWILSON** » Tue Jan 18, 2011 4:40 pm

Quote:

For the top ground plane, I have ensured there are no islands (unconnected to the ground source).

Note however that penninsulas are pretty worthless too in digital work.

8BIT · Post by **8BIT** » Tue Jan 18, 2011 5:01 pm

EE, thanks for the link. Garth, I think most of the space is penninsula free.

Daryl

kc5tja · Post by **kc5tja** » Tue Jan 18, 2011 6:46 pm

I'm not able to find "peninsula" on the web, at least in the context of PCB design or layout. I think I have an idea of what a peninsula is, but can you please illustrate or provide a link?

GARTHWILSON · Post by **GARTHWILSON** » Tue Jan 18, 2011 8:13 pm

I didn't mean that it's a legitimate PCB-design term, but rather, I used the word after he mentioned "islands." My point is that filling in an empty space with copper and having it connected to ground only by a trace somewhere (or a via) isn't going to help.