DDC114: How to route analog lines from a photo diode on a PCB

Hi Boaz,

On page 27 of the datasheet it talks about how to lay down analog signal paths. It recommends placing analog ground around the paths. Also making them as short and direct as possible. 

Hi Matt,

So if I understand correctly, it is better to route the analog lines on an outer layer, and surround it with ground (on that layer), rather than routing it between two layers of ground?

Thanks,

Boaz

Hi,

To add to Matt's reply... There are different factors at play here:

1. One is shielding against interference (including the control and data signals of the DDC). From that perspective, inputs between ground planes is the best, but simply having a ground plane under the signals may be good enough. That, of course, depends on the level of interference in the system. You know, if it is running besides a motor, you may want to embed the inputs between ground planes.
2. The other is that the noise of the DDC increases with input parasitic capacitance. That can be explained from a circuit analysis of the input amplifier. Some of our DDCs show a table of noise vs input capacitance. So, from that perspective, if there was no risk of external interference one would remove all shielding. Placing the inputs between two planes looks like worse case. At the same time, the added capacitance may be small, specially when compared to the PD capacitance. And the increased noise may also be relatively small (it may take a lot of capacitance to make this effect visible). My general advice would be to keep the separation between the planes and the ground big (use a thicker board).
3. The last one, which is quite important too in precision systems, is the one mentioned on the DS extract above. The input  is virtual ground. Any other trace around the inputs with a DC component will create a current flow into the input (straight Ohm's law: VDC/R, where R is the isolation between the two traces). As the DDC can measure really small currents, it would also measure that and create an offset on the measurement. For this, the best solution is, besides keeping inputs away from any non ground signals, to use what is called a guard, which is a ground line between inputs and any DC (or AC) sources, to sink any leakage to ground. Effectively the inputs do not see any DC around them...

Overall, it really depends on how sensitive is your application and other factors, like easy of debugging (if you bury the trace...), cost (number of layers on the board), etc. But as you ask, the best I would guess is the sandwich with two planes spaced with a good gap (to minimize parasitic capacitance) and use guards on that input layer to stop the flow of any leakage from the DC planes or signals on that layer. Our EVMs may give you some ideas too, and if I recall right, we typically do not embed all traces in the planes.

Regards,

Edu

PS.: The input impedance of the device is very small (not "high" as the DS says, it's a typo)

Hi Eduardo,

Thank you for the detailed answer.

One more parameter for these kind of circuits is the PCB material.

As I understand, there are some special materials that are used for HV applications, with very low leakage currents, but some require special PCB processes, or can handle only two layers.

Is it worth going to special PCB materials, or usually the standard ones with good surface cleaning will do the job?

Best,

Boaz

Hi Boaz,

I think that is going to depend on your application. Sure, some systems measuring very small currents will go to that extend, but many don't. You can compute the amount of leakage based on your board layout, material, and DC traces and compare it against your spec and to other sources of leakage (like the ibias of the DDC). In the end, you may be more worried about changes of that leakage, as you may be able to calibrate out the rest... Our EVMs use standard organic materials (FR4...)

Regards,

Edu