8
\$\begingroup\$

I have designed a PCB for a charge amplifier to handle a piezoelectric sensor. The first prototype is working properly.

However, coming down to the specific working frequency range, since the feedback loop is effectively a high-pass filter, with a cutoff frequency of 0.1 Hz, and there is a constraint on the capacitor's magnitude, with it being inversely proportional to the gain, I need to use very large resistance(s), in the range of 3-10 GΩ, so I came to this question regarding the PCB design.

I have ordered SMD resistors, 5, 1, 0.5, and 0.1 GΩ, all with the dimension of 0805 (inches), and the material of the board of the PCB is FR4, the data sheet of which can be found here. It's going to be just the plain board with no coating or anything else after etching the copper.

I assume there might be some complications when it comes to such high resistances, stuff that I should be aware of, some design tips, and I just want to make sure there are no fatal flaws in my selection of components, or some properties that render them unusable for my application, like for instance the resistivity of the FR4 material, and the shortness of the 5 GΩ resistor. I have researched about aspects that seemed relevant to me, but I am still not sure I thought of everything.

So, if you see anything fishy or if you care to shed a light on anything related to this design, it would be very much appreciated.

By the way, is there any drawback to installing a number of resistors in series in the feedback loop instead of one gigantic one, maybe noise issues?

\$\endgroup\$
3
  • 3
    \$\begingroup\$ I remember looking into some work on a mass spectrometer a few years back where an op amp circuit was turning a femtoamp sized current into a voltage and the resistors had to be stood off from the PCB with isolators because the FR4 would affect the circuit. I know this is rather vague, but it does suggest you might need to be concerned about the PCB with this kind of circuit. \$\endgroup\$
    – DiBosco
    Oct 10, 2017 at 13:49
  • 1
    \$\begingroup\$ I don't really understand your circuit requirement, but are you familiar with this T-network feedback design Thevenin Equivalent circuit for T feedback network of inverting ideal op amp - it may give an extra degree of freedom to achieve the required loop gain with lower value resistors. (Also discussed in the Complex Feedback Networks of this TI application note www.ti.com/lit/an/slaa068b/slaa068b.pdf ) \$\endgroup\$ Oct 10, 2017 at 19:19
  • \$\begingroup\$ Thank you for confirming my suspicions DiBosco, this is exactly why I have called for this discussion, I will look into this possibility, the use of isolators, I haven't come across something like that before, if you like to point me in a certain direction, I'd appreciated very much! I came across this T-network, but I stayed clear from it, because in page thirty of this application report by TI: eeweb.com/design-articles/…, they do not recommend the approach for its effects on high noise and offset gains! Thank you for the suggestion! \$\endgroup\$
    – Albukhari
    Oct 11, 2017 at 10:53

2 Answers 2

12
\$\begingroup\$

I used to do condenser microphone stuff professionally, which was very much this kind of thing (10G ohms with maybe a 30pF source).

Cleanliness is VITAL, a bit of skin oil in the wrong place and you will get weird popcorn noise, very annoying (An ultrasonic cleaner can be your friend here).

I would absolutely advocate solder resist to keep the potential for surface contamination down, but really the way to go is to use a teflon standoff for the high impedance node, and think carefully about the possibility of using a discrete jfet for the input buffer.

Consider guard tracks and also consider cutting a slot in the board under the resistor, extending the guard tracks to a pour on a layer under the resistor is also not a bad plan.

The problem with multiple resistors is they expose more places for contamination, and also give more capacitance to internal layers, neither of which is good.

\$\endgroup\$
1
  • 1
    \$\begingroup\$ I will apply what I can from those tips and practices, Thank you! \$\endgroup\$
    – Albukhari
    Oct 11, 2017 at 18:45
2
\$\begingroup\$

As @dan-mills pointed out cleanliness is vital if going beyond a few GΩ. Never touch anything with bare fingers.

The hint to place a slot below SMD resistors is also very good - it not only increases surface resistance of the board, it also helps a great deal to get flux residues out of the way due to offering the flux the inner wall of the slot as a residence. This prevents flux residues from bridging the SMD resistor on their bottom side with a thin film of flux (which remains after reflow soldering as well as hand soldering). A bit of air humidity combined with this flux layer can introduce fantastic drifts and memory effects. I would suggest not to go below 0805, maybe even go up to 1206 dimension for the resistor. This not only increases creeping distance but also allows getting a better TC for high value resistors.

If there is notable voltage across a high ohmic resistor take also a look at the voltage coefficient. The rated resistance is often given for 10 or 50 V and can differ notably at far smaller voltages. I had a case where the resistance increased fourfold for voltages between 0...1 V, while it was stable and correct between 20....1000 V. Sometimes you must ask for such details. The reason is that the small sized high ohmic resistors use mixtures of partly semiconducting material and are often designed for higher voltage application so they have not been checked for very low voltage operation. This might be anecdotal evidence but happened to me in practice.

Also take a look at the data sheets of the FR4 base material. They offer typical values for surface and volume resistance (which lay either only 10 times or up to 10000 times above the IPC required values). You will want to look for a product with the highest typical value you can find. Don't let different units for those resitances trick you :) When going to 25 GΩ and beyond you may need to test each batch of PCBs and sometimes have to trash and reproduce. I'm doing this on some products since some years, we measure the resistance between important traces to be from 100 GΩ to 200 TΩ - as you can see with only 100 GΩ isolation between traces and a 25 GΩ resistor things start to get weird.

We also learned that water based cleaning processes (which is the standard procedure at many assembly houses) often renders previously good boards unusable. The reason seems to be that the water used (together with detergents), despite being tri-dest and having extremely low conductance below 1 µS/cm, too many ions are introduced to the base material which you cant get rid of by tempering. Any bit of air humidity (or changes of it) can vary the surface and volume resistance by noticeable amounts.

Also, depending on trace density of your board, proposed guard rings can be more a problem than a solution. You would prefer slots, stand offs, air wiring and such.

Lately I also noticed that some stop mask materials can have lower surface resistance than a well chosen FR4 base material. If so, it might be a good idea to reduce the solder stop to only cover areas absolutely required for reflow soldering to work. This can come into play from and above 25 GΩ resistance.

Hermetically sealed packages (TO-5, TO-8 and other metal cases with glazed pins) are recommended here. Temper everything for 8 h before sealing.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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