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.

The most tedious thing for me while routing PCBs are the powers. I have made several PCBs of these kind and it seems that I have not learned much from the process. The power connections are always a mess.

Here is the description: The circuit need multiple powers including \$\pm5\,\mathrm{V},\pm12\,\mathrm{V}, +3.3\,\mathrm{V}\$. The circuit is to measure weak current at \$10\,\mathrm{pA}\$ level. Therefore, the PCB layout is supposed to be very important. And the ICs are placed in different places which may need different voltages. A four layer PCB is used with signal/ground/\$+15\,\mathrm{V}\$/signal. I can give \$+15\$ and GND for ICs directly through vias. However, for \$\pm5\,\mathrm{V}, -12\,\mathrm{V}\$ and \$3.3\,\mathrm{V}\$, the power lines keep messing with each other. Sometimes I have to use several vias in one power line. Further, if a STAR structure is to be used, the condition will be much more complex.

Could I ask for some tips on design of the power lines? And how to improve my PCB skills?

supplement: Many experienced engineers talked about analog ground and digital ground. Here comes a perfect tutorial for me: http://pdfserv.maximintegrated.com/en/an/TUT5450.pdf

And about decoupling techniques for analog IC, here is a very good one: http://www.analog.com/static/imported-files/tutorials/MT-101.pdf

share|improve this question

2 Answers 2

up vote 6 down vote accepted

Generally you don't need separate planes for power. If you have a good solid ground everywhere (you do want a plane for that in many cases), then the only issue for power is that the voltage drops due to the power current and DC resistance in the traces are acceptable. Don't worry about high frequency AC impedance in delivering power that much. Instead, bypass the power locally to the local ground at each place it is used.

In fact, especially for sensitive analog circuits, I often add a little deliberate impedance to a power feed so that a local capacitor has something to work against to filter out the high frequencies. If you put a 0805 chip inductor, for example, in series with the power connection of each IC, then follow that with a 20 uF ceramic cap to ground, you will have clean power everywhere. This is for chips and individual circuit sections that draw up to a few 10s of mA.

I just checked, and the jellybean 0805 chip inductor I commonly use for this is 950 nH and 600 mΩ. Just about any reasonable copper power trace will have less inductance and resistance than that. With this extra impedance in series with the power, a little more due to the power trace doesn't matter. With this strategy, allocating a plane to a particular power net it just a waste of routing space, and doesn't produce as good a result anyway.

As I have said many times before here, another important thing to do for low noise is to keep local high frequency currents off the main ground plane. The ground connections of a noisy subcircuit are all tied together with a local net, then that net connects to the main ground plane at a single point. The same thing works in reverse to keep noise from getting into a circuit. A sensitive analog circuit should also have its grounds connected locally, then that net tied to the main ground plane at one point.

share|improve this answer
Thanks for you reply! I agree with your sharing on grounds, if you are interested in more systematic expression, here is a perfect tutorial from maxim: pdfserv.maximintegrated.com/en/an/TUT5450.pdf And thanks for your advice on decoupling. You mentioned inductance, do you mean ferrite bead? Here comes a perfect tutorial on decoupling from Analog Device: analog.com/static/imported-files/tutorials/MT-101.pdf –  richieqianle May 25 at 13:07

I count at least 7 supply voltages. Frankly, if you don't want the sort of routing you seem to have, you need a 6-layer board. One tip for your present design - when you run power from one layer to another, if it's more than a few tens of mA, use multiple vias. There isn't all that much copper in the hole plating. You don't want a literal star configuration, but you do want a split ground plane (one part for analog, one for digital, tied together preferably at one point or small area), or perhaps a single ground plane with the analog section relatively isolated by a couple of cuts in the copper. Keep all the digital traces, including power supply voltages, physically out of the analog area - digital signals will happily couple capacitively into your analog ground plane if they run over the plane. Likewise, digital signals (including transients on the digital ground) will couple into your analog power traces, so decouple your analog power traces at the point they physically enter your analog area. Bring analog power returns on separate traces from the power connector to the analog ground.

When dealing with very sensitive analog stuff, like 10 pA signals, think of current flow as being (physically) like water - it travels from source to return, mostly directly, but it spreads out a little, too.

See, for instance, The best stack-up possible with a four-layer PCB?

share|improve this answer
Thanks, I will check the choice of 6-layer PCB. I'm afraid the price of it. However, I am not fully convinced on the separation of ground part. Here is a tutorial from Maxim:pdfserv.maximintegrated.com/en/an/TUT5450.pdf –  richieqianle May 25 at 13:01
In the tutorial, pay attention to Fig. 17 –  WhatRoughBeast May 25 at 16:39

Your Answer


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.