0
\$\begingroup\$

I have been reading up on grounding and what is AGND and DGND i.e / analogue ground and digital ground respectively. Suppose , I have an ADC chip and a MCU in a PCB. Now, previously I would have a ground plane beneath them and split them into Analogue ground and digital ground. I have now realised that splitting the ground planes will be detrimental to my return path at higher frequencies of the signal.

So, the best way is to have a single ground plane or have 2 different ground plane which is connected by a ferrite bead. Then during layout remove this bead to have a thin connection between the 2 grounds.

But, this approach has an issue according to me, which might be wrong. Will this thin line not act as a sort of high impedance that blocks currents thereby making the 2 grounds at 2 different potentials ?

\$\endgroup\$
1
\$\begingroup\$

Don't split your grounds. Drop the word split altogether. Instead, use partition. Partition your grounds.

As the previous answers have stated, the purpose of this is to keep noisy digital currents away from the analog. So you partition your board, and keep all digital traces in one area, and keep analog in another.

The use of ferrite beads on PCB to seperate grounds is a hack. Dan Beeker (Freescale) and Rick Hartley have both both expressed that ferrites are for people who do not know what they are doing. Be aware of where your currents are, and you wouldn't need to use any ferrites at all.

So keep a single plane, but partition your board such that analog signals are kept away from digital. It helps alot if the IC has pinouts which make this easy.

There some good information from Henry Ott http://www.hottconsultants.com/techtips/split-gnd-plane.html

If you look at the following image enter image description here

You can see that the board has been partitioned. To minimize any potential leakage, or stray feilds, there are cuts in the ground plane. This creates bridges that go from analog to digital grounds. This is ok so long as the routing ensures that no trace passes over such gaps.

\$\endgroup\$
  • \$\begingroup\$ So, in a nut shell. The ground should be considered as one big plane. Now, when u say partition it means allocating or placing my circuits in such a way that they do not interfere with each other. Ofcourse, some creeping is inevitable. But on the whole its ok. Now, what exactly do you mean by the word partition ? Is it not synonymous with split? \$\endgroup\$ – Board-Man Nov 24 '15 at 5:17
  • \$\begingroup\$ Could you kindly post the free scale link please? \$\endgroup\$ – Board-Man Nov 24 '15 at 5:20
  • 1
    \$\begingroup\$ @VUK partition means allocating specific areas of the board. When I read split, I think a complete separation, which is not recommended. As for the link, both Dan and Rick verbally communicated it. Dan said it during DWF seminar, and Rick said it at PCB West 2015 \$\endgroup\$ – efox29 Nov 24 '15 at 5:27
  • \$\begingroup\$ Thank you very much indeed. Now, the image you posted has split section. These are not exactly split,rather fenced section. Calling them split would be a misnomer,right? \$\endgroup\$ – Board-Man Nov 24 '15 at 5:29
  • \$\begingroup\$ @VUK I suppose that could just be my interpretation. I can't definitly say that split means a continuous break. I try and avoid using terms that can be interpreted in many ways. "Split" is one of those words for me. \$\endgroup\$ – efox29 Nov 24 '15 at 5:31
2
\$\begingroup\$

There is no law about that. If you had ten ADCs, under which would you connect the grounds? The reason to separate the ground planes is that you want to keep digital currents out of analog signals' way. So see how you can do the same with a single plane. After all, current doesn't just flow anywhere, it needs a mesh.

\$\endgroup\$
  • \$\begingroup\$ Then that would mean the split plane analogy is also fine as long as I dont route those signals referenced to it, right? \$\endgroup\$ – Board-Man Nov 24 '15 at 5:01
  • \$\begingroup\$ Yes. But you are concerned about ground bouncing, right? Although i don't think a thin tracr is that bad, but who knows? By the way, you must also make sure that there is no path for current from your analog side also outside the board, or no separation would help. \$\endgroup\$ – Gregory Kornblum Nov 24 '15 at 5:05
  • \$\begingroup\$ Yes, ground bounce is my issue. \$\endgroup\$ – Board-Man Nov 24 '15 at 5:06
  • \$\begingroup\$ So even having a single gnd and connecting both the AGND and DGND is fine. Then to prevent any digital currents from creeping into my AGND, I can put a small fencing. But, is fencing an apt methodology ? As fencing would mean removing copper in certain locations and hence/forth will give rise to split ground planes. \$\endgroup\$ – Board-Man Nov 24 '15 at 5:09
1
\$\begingroup\$

The point of having separate grounds is to have the ground currents for each section confined to that section. Most importantly, to keep high-speed digital transients out of sensitive analog circuits. If you have done this successfully, the two grounds can be connected by a relatively high-impedance connection. Since the current between the two sections will be very low, the voltage across the connection will also be low, per Ohm's Law. Then the two sections will be at nearly the same voltage.

If you're not trying for extreme performance, it's often possible to simply place the digital circuits on one side of the board and analog on the other. If the power connector is properly placed (more or less between the two sections) this will often be adequate. Current is like water, and physically tends to take the shortest path.

\$\endgroup\$
  • \$\begingroup\$ And shortest path could be the path of least resistance or inductance. This is dependant on the application,right?\ \$\endgroup\$ – Board-Man Nov 24 '15 at 5:11
  • \$\begingroup\$ Not so much application, but layout, and the point is that if the affected circuits are in close proximity to the ground power return, you won't get ground currents over on the other side of the board. \$\endgroup\$ – WhatRoughBeast Nov 24 '15 at 21:49
0
\$\begingroup\$

The whole AGND/DGND thing on ADC chips is a bit weird as it actually refers to the ON CHIP division and is done because the bond wire inductance is sufficient to cause crosstalk in modern converters if they are not separated.

Personally, I favour a single ground plane, no splits unless proven to be needed (they seldom are) with careful layout and especially component placement, for certain you must never pass a fast signal net across a split in a plane, that is just asking for trouble.

High frequency current is seldom an issue as the return current at high frequency will flow so as to minimise loop area (And thus stored energy in the magnetic field), this usually means that it will flow in the plane right underneath the relevant signal track (For this reason fast digital should be kept away from the analogue stuff). This is a good reason to fit low value source termination resistors on any digital that has to approach the analogue bits, it helps with ground bounce apart from anything else (ADC output pins should always be source terminated (and ideally locally buffered)).

Now there is something to be said for being careful about where you take things down to the plane in the analogue section, in particular with single ended stages, it pays to consider where the current loop is (Hint, it involves the driving opamps decoupling caps), and return the reference of the next stage to that point.

73 Dan.

\$\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.