Take the 2-minute tour ×
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free, no registration required.

I had a colleague design a board for pH sensor amplification based on schematic (fig 1)and spec in a paper. The paper recommends using the spec noted in figure 3. It uses a guard ring to reduce surface leakage. He used the ground plane as the guard ring (see figure 2). Was wondering if this seems like it would be correct/work

Schematic

Schematic (fig 1)

Guard ring implementation with ground ring

PCB design of guard ring (fig 2)

Guard ring specification

Documentation of guard ring (fig 3)

share|improve this question
    
This looks like a case of "Of course I put the guard ring in ... look there it is..." except it was just plain forgotten. I'm not going to suggest he (tends to guys who have this problem) didn't understand the concept of a guard ring so didn't research / ask about it.... –  Spoon Feb 21 at 11:20
add comment

2 Answers

up vote 3 down vote accepted

A guard ring is supposed to be at the same electrical potential as the input it is guarding. This reduces leakage from that node. In its simplest form it is just a same-potential ring around the sensitive node, but it can also be a driven ring and/or trace via a separate unity gain buffer.

The purpose is to not have any voltage difference (or at least to minimize it) from the protected net or node to anywhere else, and thus no path for leakage.

Using a ground plane as a guard ring is downright stupid and clearly shows that your PCB designer doesn't know what he is doing, as the ground plane is the exact thing you don't want near the sensitive node. When I am designing a PCB with guarded nodes, I often cut-out and pull back any planes under the sensitive node(s) and also pull back the solder mask too. You want nothing there but the guard ring.

Furthermore, you need to consider the trace to the guarded pin as well. Which, by the way, you have backwards on your screen-capture of the PCB ... The trace entering from the left on your diagram is from the sensor and is going to the Vin+ pin, not Vin- as you have indicated. The Vin- should wrap around Vin+. That long input trace coming from the left side should be guarded as well, or come up with a way that gets the input signal to the Vin+ pin without going across the board like that. At the very least, the ground plane around that trace should be pulled back considerably.

share|improve this answer
add comment

Your colleague hasn't followed the guideline. The guideline is correct as a theory. The ideas is that the connection from the ph probe can only "see" a unity gain version of itself. This means there can be no leakage currents to ground or any other net in the circuit. Ask your colleague why he didn't follow the guidelines.

share|improve this answer
add comment

Your Answer

 
discard

By posting your answer, you agree to the privacy policy and terms of service.

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