Ground looping w.r.t PCB routing

[PCB design]

When does Ground looping problems arise w.r.t PCB routing. How can this be avoided?

 

[marce]

Could you explain more your concerns regarding ground looping as with most of todays multilayer boards with copper pours and via stiching boards tend to have numerous ground loops!

 

[PCB design]

Hey,

Commonly we would route the GND for various components placed in a PCB forming a single loop.
Theoritically, GND looping problems may be avoided if such grounds are routed in tree structure in power electronics related designs.
My question was how would tree structure routing be implemented in routing a pcb with limited space.

Pls advise!

---------- Post added at 08:07 ---------- Previous post was at 08:01 ----------

Any other solution or better ways to avoid such problems!

 

[andre_luis]

Any other solution or better ways to avoid such problems!

That is called split plane and seems be the better choice if there no are space avaliable to separate geometrically with thin connections.

 

[marce]

Contigous ground planes are best. Splitting ground planes tends to cause more problems than not splitting.
These days, it is rare to hear the term ground loops in regards to a single PCB design, generaly these are caused when sub-systems are interconnected.
What kind of design are you doing.

 

[andre_luis]

hi marce

In fact, I noticed a video codec IC manufaturer refering to spliting planes as an unnecessary procedure.
However, I didn´t noticed that recomendation at Power applications.

+++

 

[marce]

It is better not to split planes, especially ground, you can cause more porblems than it fixes. I have been promoting a single ground plane for years, with even now much oposition, but the weight of support is for unsplit planes. Henry Ott, Keith Armstrong, Ti, National, etc etc. This does require careful layout especially in how you comparmentise your design, ie analog in one area, high speed digital in another, and where the signals are routed.
The best one I have seen was a sensitive DAC with DSP for measuring, the engineer insisted the planes were split and connected through a little zero ohm link. It didn't work and whatever he tried would not make it work untill he joined the grounds together. The small star point meant that any noise had to traverse this high impendance link, causing more noise and a significant difference in voltage levels between the analogue and digital grounds, in this case the equivilent of 4 bits out of 12 for the DAC, so the data was never right. When it came to EMC testing the design just gave up, crashing at the lowest levels of induced noise.
As I said even today myths regarding ground planes (some consider them magical!!!!!) still abound, the strangest often coming from the audio community. There is nothing magical about them, its basic physics.

**broken link removed**
Grounding of Mixes Signal Systems
http://www.ieee.org.uk/docs/emc1206a.pdf
Printed Circuit Design & Fab Magazine Online
http://focus.ti.com/lit/ml/slyp167/slyp167.pdf

---------- Post added at 08:31 ---------- Previous post was at 08:13 ----------

Regarding power applications, I've done numerous ones where you sometimes have to control where currents travel, this can be done with very careful placement and strategic splits in the ground plane, to controll the high current loops. I've done this on motor control boards and high power switch mode supplies and chargers. With realy high power designs I still prefer the control logic galvonicly isolated from the power section (on a seperate board is best as generaly control is multi layer small features, power is double sided large features and heavy copper) with Adums ADUM1300 | Triple-Channel Digital Isolator | Digital Isolators | Interface | Analog Devices or similar devices. This gives the best layout and makes life less problematic layout.
The problem is with PCB Design's problem is its very hard to give a decisive answer without looking at the circuit and layout.