Should chassis ground be attached to digital ground?

Question

I'm working on a PCB that has shielded RJ45 (ethernet), RS232, and USB connectors, and is powered by a 12V AC/DC brick power adapter (I do the 5V and 3.3V step down on board). The entire design is enclosed in a metal chassis.

The shields of the I/O connectors are connected to a CHASSIS_GND plane on the periphery of the PCB and also make contact with the front panel of the metal chassis. The CHASSIS_GND is isolated from digital GND by a moat (void).

Here's the question: Should the CHASSIS_GND be tied to the digital GND plane in any way? I've read countless app notes and layout guides, but it seems that everybody has differing (and sometimes seemingly contradictory) advice about how these two planes should be coupled together.

So far I've seen:

• Tie them together at a single point with a 0 Ohm resistor near the power supply
• Tie them together with a single 0.01uF/2kV capacitor at near the power supply
• Tie them together with a 1M resistor and a 0.1uF capacitor in parallel
• Short them together with a 0 Ohm resistor and a 0.1uF capacitor in parallel
• Tie them together with multiple 0.01uF capacitors in parallel near the I/O
• Short them together directly via the mounting holes on the PCB
• Tie them together with capacitors between digital GND and the mounting holes
• Tie them together via multiple low inductance connections near the I/O connectors
• Leave them totally isolated (not connected together anywhere)

I found this article by Henry Ott (http://www.hottconsultants.com/questions/chassis_to_circuit_ground_connection.html) which states:

First I will tell you what you should not do, that is to make a single point connection between the circuit ground and the chassis ground at the power supply...circuit ground should be connected to the chassis with a low inductance connection in the I/O area of the board

Anybody able to explain practically what a "low inductance connection" looks like on a board like this?

It seems that there are many EMI and ESD reasons for shorting or decoupling these planes to/from each other, and they are sometimes at odds with each other. Does anybody have a good source of understanding how to tie these planes together?

Answer 1

This is a very complex issue, since it deals with EMI/RFI, ESD, and safety stuff. As you've noticed, there are many ways do handle chassis and digital grounds-- everybody has an opinion and everybody thinks that the other people are wrong. Just so you know, they are all wrong and I'm right. Honest! :)

I've done it several ways, but the way that seems to work best for me is the same way that PC motherboards do it. Every mounting hole on the PCB connects signal gnd (a.k.a. digital ground) directly to the metal chassis through a screw and metal stand-off.

For connectors with a shield, that shield is connected to the metal chassis through as short of a connection as possible. Ideally the connector shield would be touching the chassis, otherwise there would be a mounting screw on the PCB as close to the connector as possible. The idea here is that any noise or static discharge would stay on the shield/chassis and never make it inside the box or onto the PCB. Sometimes that's not possible, so if it does make it to the PCB you want to get it off of the PCB as quickly as possible.

Let me make this clear: For a PCB with connectors, signal GND is connected to the metal case using mounting holes. Chassis GND is connected to the metal case using mounting holes. Chassis GND and Signal GND are NOT connected together on the PCB, but instead use the metal case for that connection.

The metal chassis is then eventually connected to the GND pin on the 3-prong AC power connector, NOT the neutral pin. There are more safety issues when we're talking about 2-prong AC power connectors-- and you'll have to look those up as I'm not as well versed in those regulations/laws.

Tie them together at a single point with a 0 Ohm resistor near the power supply

Don't do that. Doing this would assure that any noise on the cable has to travel THROUGH your circuit to get to GND. This could disrupt your circuit. The reason for the 0-Ohm resistor is because this doesn't always work and having the resistor there gives you an easy way to remove the connection or replace the resistor with a cap.

Tie them together with a single 0.01uF/2kV capacitor at near the power supply

Don't do that. This is a variation of the 0-ohm resistor thing. Same idea, but the thought is that the cap will allow AC signals to pass but not DC. Seems silly to me, as you want DC (or at least 60 Hz) signals to pass so that the circuit breaker will pop if there was a bad failure.

Tie them together with a 1M resistor and a 0.1uF capacitor in parallel

Don't do that. The problem with the previous "solution" is that the chassis is now floating, relative to GND, and could collect a charge enough to cause minor issues. The 1M ohm resistor is supposed to prevent that. Otherwise this is identical to the previous solution.

Short them together with a 0 Ohm resistor and a 0.1uF capacitor in parallel

Don't do that. If there is a 0 Ohm resistor, why bother with the cap? This is just a variation on the others, but with more things on the PCB to allow you to change things up until it works.

Tie them together with multiple 0.01uF capacitors in parallel near the I/O

Closer. Near the I/O is better than near the power connector, as noise wouldn't travel through the circuit. Multiple caps are used to reduce the impedance and to connect things where it counts. But this is not as good as what I do.

Short them together directly via the mounting holes on the PCB

As mentioned, I like this approach. Very low impedance, everywhere.

Tie them together with capacitors between digital GND and the mounting holes

Not as good as just shorting them together, since the impedance is higher and you're blocking DC.

Tie them together via multiple low inductance connections near the I/O connectors

Variations on the same thing. Might as well call the "multiple low inductance connections" things like "ground planes" and "mounting holes"

Leave them totally isolated (not connected together anywhere)

This is basically what is done when you don't have a metal chassis (like, an all plastic enclosure). This gets tricky and requires careful circuit design and PCB layout to do right, and still pass all EMI regulatory testing. It can be done, but as I said, it's tricky.

Answer 2

There is never a need to use a 0 \$\Omega\$ resistor. That's a common CYA from someone who wanted to two or more of 1) tie them together at a single point 2) wasn't sure, and wanted to be able to do that and 3) if tied together in the schematic, they got merged in the netlist into a single plane, defeating the goal of a single point 4) wanted to be able to swap in another device, e.g. a cap.

Also see this question on "EMI Proof" design.

Answer 3

I am totally in favor of the last suggestion of David Kessner. I mainly deal with analog design on micro volt level where it is very easy to destroy the design by tying different ground signals together. Simply leave them isolated and take very good care of PCB design and decoupling to avoid parasitic oscillations. Lots depend on used frequencies and signal levels. Only careful design and TESTING of prototype under noisy conditions will prove if the design is right. Passing of ESD and EMI tests is usually unrelated.

Answer 4

The chassis ground is for safety only. From what I understand it's best to keep the actual ground plane of the circuit isolated, meaning that the chassis and digital grounds only connect at/outside of the power supply. This is done for several reasons, but two of the big benefits:

1. Much less chance that any radio energy the chassis (or it's components) pick up leak into the digital circuitry
2. Significantly reduces the degree that the chassis will serve as an "unintentional radiator" - eg the oscillations and state changes in the digital circuitry are much less likely to be amplified/radiated by the chassis.

Answer 5

In my opinion, The reason that way works well on PC, is the fact that there is only one board and also close to the power supply. My own application is one DC power supply, but several PCBs in distant of each other. For my application, considering EMI and RFI, I think the best way is to tie power supply negative DC output to metal chassis/ earth ground right after the power supply at a single point. That means there should be no ground connection to chassis on all PCBs. The wire pairs from power supply should be twisted. If I had to connect at PCB side, then some DC return current would follow through metal chassis and this is a concern for noise pickup. When you have only one PCB, it still better to put this single point at power supply side, because on many power supplies the DC ground is tied to earth ground inside the power supply itself. That single point connection is a hard tie to the earth/chassis. Note that there are some applications that it is unavoidable to have multi-point connection of DC ground to chassis at the PCB side, then on that case, I would recommend to go for float DC logic grounding, which means your DC logic ground and earth ground are isolated. If you are able to make sure you could make a single ground strategy in practice, it would help you much better in term of noise pickup.

Answer 6

Connect the PCB signal ground directly to chassis ground through mounting holes the return current may not through the power cable since chassis ground may have lower impedance for return current. If it is the case will it affect the EMI of the cables? for example the part of the twist pair radiation cancellation based on same magnitude but reverse direction current.