Maker Pro
Maker Pro

power supply layer loops

J

Jamie Morken

Jan 1, 1970
0
Hi,

I am making a 4 layer PCB and have multiple supply rails (12V, 5V, 3.3V,
2.5V, 1.2V). I have put all of the supplies on the internal layer2 as
polygons, some of the polygons look like large "C" shapes, is it better
to close these polygons to make them loops, or is it better to leave
them open? I think the loops will have lower inductance than open
branches, but not sure if they are recommended over using branches.

Also are loops better than branches for common mode noise immunity?

cheers,
Jamie
 
M

MooseFET

Jan 1, 1970
0
Hi,

I am making a 4 layer PCB and have multiple supply rails (12V, 5V, 3.3V,
  2.5V, 1.2V).  I have put all of the supplies on the internal layer2as
polygons, some of the polygons look like large "C" shapes, is it better
to close these polygons to make them loops, or is it better to leave
them open?  I think the loops will have lower inductance than open
branches, but not sure if they are recommended over using branches.

Also are loops better than branches for common mode noise immunity?

It is often the resistance more than the inductance that matters.
There is a significant capacitive connection from all points on the
polygon to the ground layer plus any bypass capacitors you've added.
Large currents and any resistances can combine to create noisy supply
voltages.

A lot depends on the frequencies that matter to the circuits. For
most op-amps, the PSRR falls off with frequency. On many it is the
minus rail that matters. If this is the case in your application, you
can focus on the part that matters.
 
J

Jamie Morken

Jan 1, 1970
0
John said:
Assuming an adjacent ground plane and a scattering of bypass caps, it
generally makes no difference. Loops are arguably a bit better, but
not much different in most cases.


I don't understand that question.

The PCB I am making experiences high frequency common mode noise
transients through isolated ferrite transformers that power a SMPS, so I
am wondering about ways to increase the common mode load of the circuit
so that the common mode noise transients are attenuated more. I am
using common mode chokes on the transformers, before I added these I was
getting microcontroller/FPGA resets due to the mosfet switching
transients being coupled through the ferrite transformers. I am
wondering if supply loops or branches are more immune to these common
mode noise transients, and also any other techniques that can increase
the common mode load or common mode rejection of the PCB, beyond using a
ground plane, bypass caps etc.

cheers,
Jamie
 
M

MooseFET

Jan 1, 1970
0
The PCB I am making experiences high frequency common mode noise
transients through isolated ferrite transformers that power a SMPS, so I
am wondering about ways to increase the common mode load of the circuit
so that the common mode noise transients are attenuated more.  I am
using common mode chokes on the transformers, before I added these I was
getting microcontroller/FPGA resets due to the mosfet switching
transients being coupled through the ferrite transformers.  I am
wondering if supply loops or branches are more immune to these common
mode noise transients, and also any other techniques that can increase
the common mode load or common mode rejection of the PCB, beyond using a
ground plane, bypass caps etc.

If everything including the nearby sheet metal is rocketing up and
down with some common mode signal, things will work. It is when there
is a path for the high frequencies to pass through the circuit and and
find their way back to the supply that there is trouble.

If you make all of the entry and exit points of the circuit all
grouped at one location the currents won't tend to flow through the
PCB as much. If the supply is under your control, you are far better
off trying to prevent the stuff from getting sent to the circuit
board. Placing RF beads on the input side of the supply can help.
What you currently have is:

Cx
In----+---[noise maker]-----!!-------+----- Circuit
! !
--- ---
--- ---
! !
------+------------------------------+----- Earth ground

Cx is the transformer's capacitance

A better situation is:
Cx
In----+-[Bead]-+--[noise maker]-----!!-------+----- Circuit
! ! !
! --- !
! --- Supplies !
! ! Local ground !
+-[Bead]-+------------------- !
! !
--- ---
--- ---
! !
------+--------------------------------------+----- Earth ground

The beads appear in parallel as far as the noise getting to the
circuit is concerned. You don't want good quality inductors because
at some frequency they will resonate with Cx.
 
J

JosephKK

Jan 1, 1970
0
Hi,

I am making a 4 layer PCB and have multiple supply rails (12V, 5V, 3.3V,
2.5V, 1.2V). I have put all of the supplies on the internal layer2 as
polygons, some of the polygons look like large "C" shapes, is it better
to close these polygons to make them loops, or is it better to leave
them open? I think the loops will have lower inductance than open
branches, but not sure if they are recommended over using branches.

Also are loops better than branches for common mode noise immunity?

cheers,
Jamie

4 layer board, 5 supplies, power pours starting to look strange. I
would recheck the floor planning first. If no help was found there i
would to move one supply to another layer.
 
Top