Those of you new to power design probably haven't learned yet how crucial PCB layout is in our field. The power stage gets laid out the old-fashioned way, manually, and the reasons are discussed in the articles below.

If the experienced engineers want to add some more rules, feel free to share them here.
Or, if you have some classic real world experiences to share, that would be good too.

I have 9 basic rules I use for layout, and you can find these in article [43] and [44] in our design center. http://www.ridleyengineering.com/design-center.html [43-44] Power Supply Development Diary Parts X and XI

If you have a layout engineer not familiar with power (or even if he is) these rules can be useful to share with them.

Dear Sir,

I want to add few more comments here from my experience and understanding,

1) using a powerful CAD tools like DX-Designer expedition tool , we can define different voltage level of nets in the constrains editor which automatically take care of creepage and clearance.
2) To reduce switching noise sense resistor’s Ground should be connected to DC’s ground directly.
3)High-voltage traces related to the drain of MOSFET and RCD snubber should be kept far way from control circuits to prevent unnecessary interference.
4) If a heat sink is used for the MOSFET, connect this heat sink to ground.
4)The area enclosed by the transformer aux winding, Diode and Capaciotor, should also be kept short path.
5) Need to place all decoupling capacitor and resistor near to the controller for good decoupling and to reduce the switching noise.
6)ESD energy is delivered from secondary to primary though the transformer stray capacitor, so the controller circuit should not be placed on the discharge path.
7) Finally an appropriate isolation strategy must be defined and rigidly applied throughout the design. Creepage and Clearance spacings must separate all hazardous voltages from user accessible points. There should be a very clear channel between primary and secondary circuits.

Pls correct me If I am wrong anywhere....

I have 4 rules when routing a SMPS PCB:

-Consider the path that current flows and minimize the loop area in high di/dt circuits.
-Be mindful of high dv/dt nodes and current injection into high z circuits and ground.
-Be aware of component and board parasitics.
-Remember that "ground" is a relative term impacted by current flow.

Thanks for the rules.
Now I have something to ask.
Let me explain the scenery first. I am working on a digital control power supply. Almost everything looks OK. The power grounds and signal grounds are isolated with galvanic isolation, Except one voltage measurement which was done through a diff. attenuator of 600k resistance on each +ve and -ve rail to the input of diff. amp. The power ground and
The resistance between the power circuit (pgnd) and control circuit (gnd) measures to be of min. 300k ohm.

Q1. Is that OK??


Now, let me take your opinion too regarding the control section grounds.
All the power and analog signal layouts apart, I would like to have some comments on isolating the grounds in digitally controlled power supplies (viz., AGND for ADCs/ref., digital GND for VDD of MCU, op-amp gnd and digital input/ouput circuit grounds).

Q2. Of the grounds mentioned above what are the grounds to be tied together, what are to be kept isolated?
Q3. If they are to be isolated, then which kind of ferrite bead / resistor to be used?
Q4. Which grounds of above need a plane and which may not need?

Thank you.

A good topic.

Perhaps simple questions, but complicated answers. Grounding of power supply controls is a BIG issue, whether they be digital or analog.

First, it is good that your power supply and ground are completely galvanically isolated. That minimizes failure propagation, you really don't want to lose you controller when a FET blows up. I would say that the diff amp connection should be OK, but would have to see schematics to be more certain.

Even if you are galvanically isolated, there are still problems that can occur with the grounds. If you have a high voltage power stage, and current transformers in a noisy part of the circuit, capacitance can disturb the signals and lead to failures on some bridges.

On the low voltage part, ground planes will provide shielding, but don't run them near noisy power parts or they will act as a nice antenna. In other words, don't just run ground planes everywhere.

Like on the power circuit rules in the article, you must provide defined paths for gate drive currents, don't let them just run where they like through ground planes. The can run several amperes of current.

I'll defer to others on ferrite bead issues for grounds. I have never used them personally. I just prefer to have a single point connection of different ground planes. Adding in some inductance can cause as much trouble as it solves.

Also I think it will be circuit specific as to which you connect or separate. Planes are use to both provide low impedance, and to shield. Keep that in mind when you decide whether or not to use a plane.

Those are excellent points. Huge ground planes are great for small signal circuits but can be detrimental in power. Keep a power ground plane only under the power section and signal ground plane only under the signal circuit.

Many ignore the gate drive path and sometimes have a good distance between devices. The connections should be as short as possibe, just like the power switching loop. Lots of noise can be generated by the fast gate drive pulses. For power switching devices I came up with placing a copper plane of same footprint directly underneath the device and connecting it back to the B+ at the transformer node. Essentially capacitively coupling the noise in a small loop.

The connecting point of power and signal grounds is critical as well. Most controller specs give direction as to optimum placement.

Another critical section of layout is the EMI filter. The 2 sides should be physically matched/impedance balanced. Earth ground placement is extremely important. The entire filter should be placed so the earth ground/chassis connection is as short as possible.