Continue to Site

Welcome to

Welcome to our site! is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Ground/ Earth Loops - HUM case

Not open for further replies.


Advanced Member level 1
Jul 13, 2001
Reaction score
Trophy points
Activity points
Ground/ Earth Loops

Hi all,

In audio circuits, ground loops cause HUM (instability).
When autorouting in Layou*t Plu*s, is the routing loop- free?
Does the status of the design in terms of loops change after copper pour?

Views welcome.


A would NOT autoroute any sensitive analog parts of any circuit board. You see, it is not the "ground loops" as such which is the problem, but sharing a wrong ground return. A sensitive low level circuitry should not share a ground path with for example power supply or output amplifier. No autorouter is smart enough to consider the correct return paths and ground impedances. It is better to do the job manually.

Autrouters can often do a good job on a multi-layer digital board, but on analog circuitry? In my opinion, not very likely.

Return paths

Thanks ted. your replies to my questions have been very useful.
What should be the terminating point for a particular section ground return path? Should it be the filter capacitor?


Ground/ Earth Loops

What in case of a stereo amplifier with bridge o/p on each channel and

operating from the same supply (consider split supply). In this case

the load is not ground referenced and the supply lines act as return

lines. Do we route seperate paths for +ve, -ve and GND lines in this


Is there an e-book on this topic? Preferably with examples and



Unfortunately I do not know any e-book about the subject. I try to summarize my experiences with this kind of designs, without actually being any guru in this particular topics -- but I have made several basically similar constructions in different contexts. Some well working, others needing rework.

I would follow these principles: You may keep the power output stage, inclusive its bypass capacitors, in one ground system/feed system. The two channels are likely not disturbing each others, because they have relatively high level inputs. The power output stage is fed directly from the power supply.

When the load is not ground referenced, the return currents travel through power rails. In any case thus the bypass/filter caps are very important. Be aware the ESR values of those cpacitors, too! The Effective Series Resistance of electrolytics is often the most important factor for the ripple and noise distribution. It is easy to calculate the minimum capacitance, and then be surprised that the result is not even close by matching the theory.

The driver driving that output stage has intermediate signal levels and moderate return currents. Do not let the ouput return currents run through this stage, and a separate filtering might be necessary--I am not sure about your particular design. Input of this is connected to the most sensitive input part, and ground to it should be connected from here in single point, parallel with the signal(s).

The input amplifier should have at least a RC filtered power supply feed, or even it's own regulator chips. And of course, here the "single-point-grounding" FOR THE INPUT AMPLIFER itself should be then carefully connected to the rest, to avoid the "ground loops" and also unwanted feedback from the output stage.

Try to imagine where the big currents flow in the output, and keep those paths short, low-impedance and separate. Similar way, the sensitive parts should be an "islands" of their own, with no ripple or output currents flowing through them.

Good luck!

Return Lines

Hi ted,

Thanks againg for your detailed reply. The issue on return lines is now quite clear and hopefully my next pcb's should give me optimum results. By the way, most of the times the uncrowned Guru's get things across quickly than a 1000 page book.
The term 'islands' made me visualise what you wanted to say.
I also found this in the Capture* help(F1):

To isolate a power net to a schematic page
Place a power symbol and attach it to an off-page connector.

When Capture resolves netname conflicts, the name of the off-page connector takes precedence over the name of the power object, and the off-page connector's scope is limited to the schematic folder. All pins on the same page that are connected by name or by wire to the power symbol are connected to the isolated power net.

For example, say you want to isolate your analog and digital grounds and then connect them at one point when you make a printed circuit board. You place your analog circuitry on a separate schematic folder. On each page in the analog schematic folder, you place a ground symbol with the name GND. This implicitly connects all the pins named GND to ground. Then you connect that power symbol to an off-page connector named AGND. To connect AGND to the digital ground (GND), you can create a part whose footprint is a strip of copper with two pads, GND and AGND.

Can I have your e-mail id? I will keep you pposted on the results.



Ground Return Lines

Hi again ted,

As mentioned in the earlier post, I am pleased to tell you that I re- did my PCB, this time with consideration for return

lines, along the guidelines you provided.
All the problems have been eliminated and the results are 100% sucessful. I have a lot to thank you for the help and hints.

The best part was that you came forward to share your expertise with us. If there is any thing that I can do, let me know.

Thanks again ted!
and thanks elektroda!!


Not open for further replies.

Part and Inventory Search

Welcome to