3
\$\begingroup\$

I have 7 x A3941 DC motor drivers and they have to coexist on a board with an STM32 MCU and onboard 5V and 3.3V supplies. Since there are a lot of ‘noisy’ components here, will the following ground plane layout be valid for noise immunity/suppression?

The quiet ground is essentially a plane for a few components as per the recommendation in the A3941 datasheet.

enter image description here

EDIT: The current placement layout is as follows,

enter image description here

EDIT-2: Came across this wonderful video a day ago on splitting ground planes and if you should do so. A real eye opener for me.

Improve this question
\$\endgroup\$
3
  • 4
    \$\begingroup\$ If you choose to have those islands only run traces over those bridges, never across the gap. You could also just do without the islands but maintain component partitioning since return currents flow in the ground plane under the traces if they can (smallest loop area) and the goal is to prevent return currents from something noisy flowing under something quiet. \$\endgroup\$ – DKNguyen Apr 22 at 3:28
  • \$\begingroup\$ @DKNguyen yes this will be an unbroken plane however traces on other layers also shouldn’t cross the islands other than the bridge area? There are quite a few traces since they all connect to the MCU. \$\endgroup\$ – electrophile Apr 22 at 3:33
  • 2
    \$\begingroup\$ More accurately, no trace should ever cross a gap in that trace's ground/reference plane. Doing so prevents the return current from flowing in the plane beneath the trace and that's when it branches out in big loop to try and find its way back home. \$\endgroup\$ – DKNguyen Apr 22 at 3:36
14
\$\begingroup\$

Generally gapping the ground plane is universally bad for EMI. Here is why:

  1. If you fail to contain the generated energy at its source due to bad layout, it will spread throughout the board regardless of GND split or not. Use good layout, cabling and io-filtering. Minimize all loops.

  2. the GND split will amplify radiated emission and pickup (slot antenna).

  3. instead of gapping the plane, place your components in functional groups that are far from each other to isolate them mutually from common impedance noise. Within the group, cluster components as tight as possible to minimize loops. For a motor drive, all the components surrounding the driver circuit are one group though. But things like MCU and oscillators should be a bit off

  4. there are countless more subtle rules to follow (but gapping GND is not one of them). In your case I think having connectors on one side of the board will help with cable radiation.

If you have something really bad that does not need a ground plane (like a motor), then don't gap the GND plane around it but pull the GND plane back and connect it with traces. That way at least you won't get slot antennas

Improve this answer
\$\endgroup\$
4
  • 1
    \$\begingroup\$ Try to have the power input close to the motor drivers so you aren’t pulling the high currents across the pcb \$\endgroup\$ – Kartman Apr 22 at 5:00
  • 1
    \$\begingroup\$ Thanks. This answer is helpful. The A3941 data sheet suggests that some components have a separate ground called the quiet ground. How do you accommodate this? \$\endgroup\$ – electrophile Apr 22 at 5:24
  • 3
    \$\begingroup\$ @electrophile I would say it is wrong advice. Many EMI experts agree that datasheet advice on layout is often terrible. Motor drivers are well known subjects. Layout is critical but GND gapping is not a useful solution if EMC is important. \$\endgroup\$ – tobalt Apr 22 at 6:06
  • 2
    \$\begingroup\$ I found the part about the sensitive components in the datasheet. A better way to do it for those components is: use GND traces for those sensitive components and run these on another layer (not in the GND plane layer) \$\endgroup\$ – tobalt Apr 22 at 6:08
4
\$\begingroup\$

will the following ground plane layout be valid for noise immunity/suppression?

No.

The quiet ground is essentially a plane for a few components as per the recommendation in the A3941 data sheet.

List the currents in your design, in descending di/dt order. On top of the list you'll probably find the input and output currents of your motor driver. Then, keep these currents out of the parts of the ground plane where sensitive circuits are. So... this is all about placement.

I don't see any connectors on your drawing, and that's important. Since there is a power supply section, I suppose the power entry connector is there. And I don't know where the connector for the motors is, so I put it on the edge of the board closest to the drivers.

enter image description here

Current will flow from the power entry connector, through the board, in the ground plane, probably a bit like I drew. So it is going to nuke the potential of "0V" everywhere. Also, if the motor connectors are on the other side of the board relative to the power entry connectors, and your ground plane has high impedance because it's full of cuts, then there will be a potential difference between GND on both connectors, which means the cable will radiate common mode noise, and it will fail EMI.

So, it's simple : put the motor drivers right next to the power entry connector, with some decoupling caps on the DC rail in between. Then the motor connectors as close as possible to the power entry connector. All on an uninterrupted ground plane, and on the same edge of the board.

Then the high current won't go through your whole board, it will stay in that zone and follow the path of least impedance.

Basically, keep the area of high di/dt loops small and compact. The smallest area is achieved when forward current is on a fat trace or pour on layer1, and return current is on the ground plane on layer 2 right below.

If you use a differential current sense amp, remember they have pretty good common mode rejection from the sense resistor to the differential input, but the output is referenced to whatever "GND" is where you connect the "GND" pin of the chip, so you can make the differential pair longer to place that chip away from the noise, or pickup the reference from a quiet spot.

And, since you should never route traces over ground splits, when you get rid of the ground plane cuts, you'll find your routing is a lot simpler and you have plenty of space left. Also if you shorten the high current paths, you'll have much less fat traces taking space. So you'll have room to push the switching converters in a corner away from the sensitive bits, and just isolate with a bit of distance. I suggest to put the switchers on the other side of the power entry connector from the drivers, so the switchers don't emit noise into the motor cables.

Improve this answer
\$\endgroup\$
6
  • 1
    \$\begingroup\$ Valuable post. The placement of connectors is critical for EMI. If there are a lot of return currents in the 0V plane (such as in this example). Cable antennas have to be considered. \$\endgroup\$ – tobalt Apr 23 at 4:41
  • \$\begingroup\$ This is really helpful. Thank you. I've also edited my Q to include the current parts layout. \$\endgroup\$ – electrophile Apr 25 at 7:32
  • \$\begingroup\$ New layout is much better. Note 4 layer is on sale at JLCPCB, the price is very cheap, and it's really convenient. Will your motor drivers need a heatsink? If yes, perhaps more convenient to put them in a line so you can use just one aluminium bar on top pressing on all SMD chips. If not, you could swap "VIN 12V" and "Motor 3 driver" to put the power entry in the middle of the group of drivers, so current goes directly from power supply to drivers through shortest path. And... continuous ground plane. \$\endgroup\$ – bobflux Apr 25 at 9:38
  • \$\begingroup\$ Yes 4 layers are really affordable these days.. however they can be very hard to solder because they sink heat incredibly fast. \$\endgroup\$ – tobalt Apr 25 at 13:46
  • \$\begingroup\$ That's great if you want to cool your chips though ;) If you have trouble, get KSGER soldering iron with BCM2/3 tips from aliexpress, it's cheap, and heating element is directly molded in ceramic inside the tip, so it heats in 3 seconds and does not fear big ground planes at all. \$\endgroup\$ – bobflux Apr 25 at 14:29
0
\$\begingroup\$

Is your issue crosstalk between your motor drivers and low frequency microvolt signals you are processing on-board? If so, a gap isolating your most sensitive circuitry might be a good idea. Follow DKNguyen's advice: never route a trace across a gap, and gap any power planes the same way.

However, as tobalt notes, it is best to "let ground abound" in most cases. The great thing about a ground plane is that it allows your return currents to take the easiest path, usually minimizing their effects. Concentrating currents at the bridges is often trouble.

But for low-power analog circuitry sensitive to small low-frequency voltages, the trouble is that the low-frequency return current for high-power circuitry sharing the board spreads out, and may cause problems. There, a gap may reduce crosstalk. This is different from the EMC issues that tobalt discusses. In any case, I would never put gaps around all the digital and power sections the way you have drawn.

Improve this answer
\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.