Radiated Digital Ground Noise
High-Speed Digital Design Online Newsletter: Vol. 2 Issue 17
I am now reading your book "High Speed Digital Design". I am finding it very interesting, well written and informative. I have now finished Chapter 7 "Vias" but a colleague of mine asked about circuit board grounding to help pass FCC testing of radiated emissions. I let him read section 5.8.2 on Chassis Layers for printed circuit boards.
We both agreed that in our experience, tying the digital ground to the chassis at the point of egress from the chassis (say at an output RS-232 connector) will quiet radiated digital noise. We agreed that this technique would put the chassis at the same potential as the digital ground.
What we could not explain exactly is how tying the digital ground plane to chassis actually reduces (common mode) radiated emissions from circuits going to the outside world (say via the RS-232 cable)? Thank you for your help.
Thanks for your interest in High-Speed Digital Design.
First let me say that tying digital ground (DGND) to chassis can be extremely beneficial, if your power supply architecture permits such a connection to be made. Now let's consider the precise point (or points) at which such a DGND-CHASSIS connection should be made.
Let's say your product is composed of a solid metal box, with one cable leading out of the box. Inside the product there is a single digital circuit board (PCB), powered by an on-board battery. The cable is connected to the PCB at the point where the cable exits the box.
We will consider two scenarios. In both scenarios the digital board is grounded at one and only one location. First, look at case (A) where the digital circuit is grounded to the chassis near the point where the cable exits the box.
(A) ____________________ | | | | CABLE | _______________ | PCB | | ______________X | | | | |________________X_|
Now look at case (B) where the digital circuit is grounded to the chassis at a point OPPOSITE where the cable exits the box.
(B) ____________________ | | | | CABLE | _______________ | PCB | | | X_____________X | | | | |__X_______________|
To properly understand the difference bewteen these two examples you need to keep in mind that tiny voltages differences exist at opposite ends of the ground plane of the PCB. These voltages are caused by the digital signal currents moving across the PCB on the signal traces. Every signal current generates an equal and opposite path of return current flowing along the digital power and ground system. As these high- speed currents traverse the finite inductance of the power and ground planes, they produce tiny voltages. These noise voltages as measured from one end of your ground plane to the other are too small to create a noticeable signal integrity problem, but plenty large enough to cause major EMI difficulties.
In case (A), the digital ground is pinned to the chassis at the point of cable exit. The digital ground voltage at that point equals the chassis potential. As viewed from the exterior of the chassis, the voltage potential on the cable and the chassis are the same. The cable, therefore, does not radiate.
Case (B) is different. Now the digital ground is pinned to the chassis opposite the point of cable exit. The digital ground voltage at the cable exit point now equals the chassis potential (from the far side) plus any noise picked up across the ground plane of the circuit card.
As viewed from the exterior of the chassis, the voltage potential in case (B) between the cable and the chassis differ. We have constructed an efficient antenna system, with the chassis acting as a grounded object and the cable (the antenna) driven by a voltage source equal in magnitude to the ground noise generated by the digital PCB. Yuk.
Ideally, you should ground your digital logic, the chassis, any cable grounds, and the cable shield (if present) to a common point, using broad, wide objects to accomplish all connections.
Dr. Howard Johnson