Layout basics for analog & digital

[mayor]

Short story: I am working on a design which uses a microcontroller with ADC inputs and lots of digital, of course. The ADCs are fed by op amps that are driven by DACs.

I plan on using a 4 layer boards. I am not too sure where to place the DACs, and what to do with the microcontroller, with regards to a ground plane. Basic pointers appreciated.

[mrkev]

Well, you can either make one big ground plane, or better is to have two separated ground planes, one for digital and other for analog. Connected together only at one point, usually somewhere under the microcontroler. The placement is hart to tell without schematic.. Just put digital together and analog together 

[DanielS]

The way mixed boards usually play out is you split your board (and ground/power) in two with all the analog stuff on one side of that split and all the digital stuff on the other. The ADCs and DACs often straddle the planes with the digital IO/control/power/ground on the digital side and the analog inputs/outputs/power/ground on the analog planes.

[ludzinc]

(Flame suit on)

Split ground planes are a bad idea.

You want to minimise inductance loops, and to do this you ideally want your signal trace to lie directly next to or above a ground return.

If you have a digital control signal that crosses a split plane, you create a big loop, and it's easy to do this inadvertently with split planes.

See the over simplified attached picture for an example.

That said and done, it's still a good idea to segregate your analogue and digital stuff where possible (separate regulators for analog circuits vs digital is a good idea too).

[TriodeTiger]

You might want to save this guy your computer: http://www.analog.com/library/analogdialogue/archives/43-09/EDch%2012%20pc%20issues.pdf

Other than trial and error and review, I thought I'd look up what PCB books / whitepapers and appnotes I could find on the subject - and that was the best one I came up with in a few moments.

[DanielS]

If you have a digital control signal that crosses a split plane, you create a big loop, and it's easy to do this inadvertently with split planes.

Control signals usually do not need to cross over the split plane since most ADCs and DACs designed for use with split planes (you should use one of these if you care enough about noise to bother with a split plane) are designed to straddle the split so all their digital IO and power pins can be on the digital side, and all their analog IO and power on the analog side like this...

[Dago]

Often times split ground planes are not needed. Just use one big ground plane and physically separate the board (meaning the "modules" on the board, ie. power supply, amplifier etc.) so that the return currents do not overlap, this achieves the pretty much the same thing as a split ground plane.

Designing a board with proper split ground planes is much more difficult. You really need to think about the return currents.

[jahonen]

Splits may also create unintended resonances at some random frequencies and the result might be actually worse than without a split. So if there happens to be an aggressor signal at that frequency, it might make things worse. Having a single solid plane with proper placement of functional blocks is usually the solution with least amount of surpriseness.

Since this kind of discussion is usually just a list of everybody's opinion, I'll post measurement which I made some time ago.

Test board had an oscillator which drives a CDCV304 clock driver, which drives some 50 ohm transmission lines terminated at the ends. I made two exactly similar boards, but other one had all copper removed between via fencing:



These measurements are measured from that SMA connector connected to a Rohde & Schwarz FSV 7 spectrum analyzer. Here is a measurement from a board using continuous ground:



And here is a measurement from a board using split ground:



As you can see, there is some gain for creating the split but then, at ~580 MHz the situation becomes significantly worse due to a resonance. High power stuff might be a valid reason to do split grounds but for signal stuff, I think it is definitely not a magic bullet which solves all the grounding problems.

Regards,
Janne

[David Hess]

In precision analog designs, it may be necessary to maintain a ground plain island to keep digital return currents from corrupting the analog ground.  Cuts may be made in the ground plain to route return currents around an analog island. 

Maintaining a single point analog to digital ground connection gets tricky when you have more than one converter or interface between the separate domains.  Extreme cases may require galvanic isolation and include features to minimize capacitive and inductive coupling between the two domains.

Underused tricks include the use of baluns to subtract common mode high frequency noise and signaling with currents instead of voltages.

[DanielS]

Often times split ground planes are not needed. Just use one big ground plane and physically separate the board (meaning the "modules" on the board, ie. power supply, amplifier etc.) so that the return currents do not overlap, this achieves the pretty much the same thing as a split ground plane.

Putting your sensitive stuff on separate PCBs is just a very expensive way of splitting a ground plane and you still need to use many of the same extra precautions as a split ground plane to make it work right... and you may end up still needing a split plane on that card anyway to separate board-to-board interface noise from the sensitive analog stuff - you still have all the noise on the main board's ground plane coming in through your plug-in board's ground pin(s) regardless of return currents.

The only thing using a separate card really does is prevent you from accidentally routing unrelated signals through the split plane area. Yes, it does also reduce the footprint on the PCB but the logical thing to do with analog stuff is put it near a board edge/corner, out of the way from unrelated chips so there won't be any unrelated return currents needing to go through the area.

[tggzzz]

Short story: I am working on a design which uses a microcontroller with ADC inputs and lots of digital, of course. The ADCs are fed by op amps that are driven by DACs.

I plan on using a 4 layer boards. I am not too sure where to place the DACs, and what to do with the microcontroller, with regards to a ground plane. Basic pointers appreciated.

You should start by reading all the literature produced by the manufacturer of your chosen MCU. That will provide specific recommendations and, hopefully, an indication of the performance that can be expected.

Old aphorism: "there are lies, damned lies, statistics, and adc/dac specifications".

[Bassman59]

Split ground planes are a bad idea.

Yup.

[Neilm]

Have a look at www.compliance-club.com. Look for the layout articles by Keith Armstrong. I found them well written and very useful - you can learn a lot from them.

Also - beware I have seen datasheets for ADCs specifying split analogue and digital planes. Almost every time I have investigated EMC failures with split plains, stitching them together fixed the problem.

[mrkev]

Splits may also create unintended resonances at some random frequencies and the result might be actually worse than without a split. So if there happens to be an aggressor signal at that frequency, it might make things worse. Having a single solid plane with proper placement of functional blocks is usually the solution with least amount of surpriseness.
.
.
.
As you can see, there is some gain for creating the split but then, at ~580 MHz the situation becomes significantly worse due to a resonance. High power stuff might be a valid reason to do split grounds but for signal stuff, I think it is definitely not a magic bullet which solves all the grounding problems.

Regards,
Janne

Well, duh!
Everything gets tricky when you get higher than few hundereds MHz. But below 100MHz, there isn't much that can speak against split grounds...
Btw. nice measurment, it just made me smile a bit, when you called difference of less than 6dB, barelly above noise level and somewhere deep at -100dBm (about 70uV vs 200uV) significant difference . Plus, you can always count that resonation freq or measure it at prothotype level... Good to know anyway...

[tggzzz]

Also - beware I have seen datasheets for ADCs specifying split analogue and digital planes. Almost every time I have investigated EMC failures with split plains, stitching them together fixed the problem.

It can be informative to look at the PCB layouts for the manufacturer's ADC/DAC evaluation boards. If they incorrectly showed the ADC/DAC in a less than favourable light, they wouldn't even be released!

[T3sl4co1l]

Also - beware I have seen datasheets for ADCs specifying split analogue and digital planes. Almost every time I have investigated EMC failures with split plains, stitching them together fixed the problem.

It can be informative to look at the PCB layouts for the manufacturer's ADC/DAC evaluation boards. If they incorrectly showed the ADC/DAC in a less than favourable light, they wouldn't even be released!

I wouldn't be so sure of that.  Do they always run EMC on dev kits?  Who knows.  (If someone wants to bring a few into a chamber during spare hours, please do!)

I've personally seen nanosecond edges coming off an LT dev board that claims good performance, but doesn't happen to make any claims about EMC as well.  Guess what product ended up with spikes in the 100s of MHz...

Tim

[tggzzz]

Also - beware I have seen datasheets for ADCs specifying split analogue and digital planes. Almost every time I have investigated EMC failures with split plains, stitching them together fixed the problem.

It can be informative to look at the PCB layouts for the manufacturer's ADC/DAC evaluation boards. If they incorrectly showed the ADC/DAC in a less than favourable light, they wouldn't even be released!

I wouldn't be so sure of that.  Do they always run EMC on dev kits?  Who knows.  (If someone wants to bring a few into a chamber during spare hours, please do!)

I've personally seen nanosecond edges coming off an LT dev board that claims good performance, but doesn't happen to make any claims about EMC as well.  Guess what product ended up with spikes in the 100s of MHz...

Sure; everything is secondary to making the device look good.

It is completely reasonable for a the device eval board manufacture to take the attitude that their board cannot represent how the device will perform in your system (even ignoring their traditional use of specmanship!). It will always be necessary for you to exercise skill and judgement when designing a component into your system.

Nonetheless useful information can be gained by looking at the eval board. And it would be unwise to presume that it will contain all the information you need. No surprises there.

[Dago]

Often times split ground planes are not needed. Just use one big ground plane and physically separate the board (meaning the "modules" on the board, ie. power supply, amplifier etc.) so that the return currents do not overlap, this achieves the pretty much the same thing as a split ground plane.

Putting your sensitive stuff on separate PCBs is just a very expensive way of splitting a ground plane and you still need to use many of the same extra precautions as a split ground plane to make it work right... and you may end up still needing a split plane on that card anyway to separate board-to-board interface noise from the sensitive analog stuff - you still have all the noise on the main board's ground plane coming in through your plug-in board's ground pin(s) regardless of return currents.

The only thing using a separate card really does is prevent you from accidentally routing unrelated signals through the split plane area. Yes, it does also reduce the footprint on the PCB but the logical thing to do with analog stuff is put it near a board edge/corner, out of the way from unrelated chips so there won't be any unrelated return currents needing to go through the area.

Sorry, "modules" was most likely a bad word. "Functional block" used by jahonen is what I meant. Not actual separate boards.