Adam Seychell
Guest
Mon Feb 08, 2010 2:26 am
I'm designing a 120A 4 phase step down power supply, and require a 6
layer 2OZ PCB to meet current carrying capacity requirements. There will
be a mix of sensitive analogue and digital in my purpose built
multiphase controller consisting a mixture of op-amps, discrete
transistors, high speed comparators, ADC, DAC, programmable logic & a
microcontroller.
Is it feasible to separate analogue and digital components so they are
placed directly on opposites sides of the PCB, and use separate
non-isolated ground planes ?
I am speculating that return currents from digital lines should only
flow in the adjacent ground plane layer, and not interfere with
subsequent ground and signal layers. For a 6 layer stack I am considering:
[analogue components]
--------------------------
L1 analogue signal
L2 ground
L3 power (analogue)
L4 power (digital)
L5 ground
L6 digital signal
------------------------
[Digital components]
L2 and L5 will be connected only in limited locations.
Adam Seychell
John Larkin
Guest
Mon Feb 08, 2010 2:39 am
On Mon, 08 Feb 2010 11:26:35 +1100, Adam Seychell
<bogus_user_at_bogus_server.com> wrote:
Quote:
I'm designing a 120A 4 phase step down power supply, and require a 6
layer 2OZ PCB to meet current carrying capacity requirements. There will
be a mix of sensitive analogue and digital in my purpose built
multiphase controller consisting a mixture of op-amps, discrete
transistors, high speed comparators, ADC, DAC, programmable logic & a
microcontroller.
Is it feasible to separate analogue and digital components so they are
placed directly on opposites sides of the PCB, and use separate
non-isolated ground planes ?
I am speculating that return currents from digital lines should only
flow in the adjacent ground plane layer, and not interfere with
subsequent ground and signal layers. For a 6 layer stack I am considering:
[analogue components]
--------------------------
L1 analogue signal
L2 ground
L3 power (analogue)
L4 power (digital)
L5 ground
L6 digital signal
------------------------
[Digital components]
L2 and L5 will be connected only in limited locations.
Adam Seychell
That sort of thing can be very hard to work on. If you have the space,
it's better to keep everything on the same side, with the power and
signal stuff separated horizontally.
The two ground plane thing is OK, but they could use the same ground
plane if you keep big circulating currents out of the low-level stuff.
One way is to almost split the ground plane into two halves with a
fairly wide gap connected by a few relatively skinny traces.
How are you going to get the 120 amps off the board?
Johm
Adam Seychell
Guest
Mon Feb 08, 2010 4:26 am
On 8/02/2010 11:39, John Larkin wrote:
Quote:
On Mon, 08 Feb 2010 11:26:35 +1100, Adam Seychell
bogus_user_at_bogus_server.com> wrote:
I'm designing a 120A 4 phase step down power supply, and require a 6
layer 2OZ PCB to meet current carrying capacity requirements. There will
be a mix of sensitive analogue and digital in my purpose built
multiphase controller consisting a mixture of op-amps, discrete
transistors, high speed comparators, ADC, DAC, programmable logic& a
microcontroller.
Is it feasible to separate analogue and digital components so they are
placed directly on opposites sides of the PCB, and use separate
non-isolated ground planes ?
I am speculating that return currents from digital lines should only
flow in the adjacent ground plane layer, and not interfere with
subsequent ground and signal layers. For a 6 layer stack I am considering:
[analogue components]
--------------------------
L1 analogue signal
L2 ground
L3 power (analogue)
L4 power (digital)
L5 ground
L6 digital signal
------------------------
[Digital components]
L2 and L5 will be connected only in limited locations.
Adam Seychell
That sort of thing can be very hard to work on. If you have the space,
it's better to keep everything on the same side, with the power and
signal stuff separated horizontally.
The two ground plane thing is OK, but they could use the same ground
plane if you keep big circulating currents out of the low-level stuff.
One way is to almost split the ground plane into two halves with a
fairly wide gap connected by a few relatively skinny traces.
How are you going to get the 120 amps off the board?
Johm
With bus bars for Vin, GND and Vout. After much head scratching, I
decided on hand soldering 2 x 12mm copper bus bars in close vicinity to
the power components. A single hole at end of each bus bar will provide
termination to 25mm^2 cable lugs and the like.
The gate driver ICs are right up against the MOSFETs, allowing logic
level PWM signal to go off to the controller circuit some distance away.
The power and signal stuff are physically separated by 2", but are on
the same PCB. I was concerned about laying the digital components on the
opposite side to analogue components in the power supply controller section.
2G
Guest
Mon Feb 08, 2010 7:18 am
On Feb 7, 4:26 pm, Adam Seychell <bogus_user_at_bogus_server.com> wrote:
Quote:
I'm designing a 120A 4 phase step down power supply, and require a 6
layer 2OZ PCB to meet current carrying capacity requirements. There will
be a mix of sensitive analogue and digital in my purpose built
multiphase controller consisting a mixture of op-amps, discrete
transistors, high speed comparators, ADC, DAC, programmable logic & a
microcontroller.
Is it feasible to separate analogue and digital components so they are
placed directly on opposites sides of the PCB, and use separate
non-isolated ground planes ?
I am speculating that return currents from digital lines should only
flow in the adjacent ground plane layer, and not interfere with
subsequent ground and signal layers. For a 6 layer stack I am considering:
[analogue components]
--------------------------
L1 analogue signal
L2 ground
L3 power (analogue)
L4 power (digital)
L5 ground
L6 digital signal
------------------------
[Digital components]
L2 and L5 will be connected only in limited locations.
Adam Seychell
I think it is feasible. Just ensure that the stackup minimizes the L2-
L3 spacing and the L4-L5 spacing, while maximizing the L3-L4 spacing.
This will minimize the respective loop inductances.
Tom
John Walliker
Guest
Mon Feb 08, 2010 1:54 pm
On 8 Feb, 04:18, 2G <soar2mor...@yahoo.com> wrote:
Quote:
I think it is feasible. Just ensure that the stackup minimizes the L2-
L3 spacing and the L4-L5 spacing, while maximizing the L3-L4 spacing.
This will minimize the respective loop inductances.
And similarly, try to keep the busbars as close to each other as
possible and gently twist the external cables together to minimise
loop area.
John
Martin Riddle
Guest
Tue Feb 09, 2010 2:04 am
"John Walliker" <jrwalliker_at_gmail.com> wrote in message
news:c0ea3e9a-9b46-461e-af09-8111ad03e951_at_m31g2000yqd.googlegroups.com...
Quote:
On 8 Feb, 04:18, 2G <soar2mor...@yahoo.com> wrote:
I think it is feasible. Just ensure that the stackup minimizes the
L2-
L3 spacing and the L4-L5 spacing, while maximizing the L3-L4 spacing.
This will minimize the respective loop inductances.
And similarly, try to keep the busbars as close to each other as
possible and gently twist the external cables together to minimise
loop area.
John
I think he needs to move his Analog Power layer(L3) to the Top (Or
Bottom). Inner layers for high power stuff results in higher copper
temps, he may wind up delaminating the board. Plus, mounting the Buss
bars may be easier.
Cheers
Jon Slaughter
Guest
Tue Feb 09, 2010 8:09 pm
Adam Seychell wrote:
Quote:
I'm designing a 120A 4 phase step down power supply, and require a 6
layer 2OZ PCB to meet current carrying capacity requirements. There
will be a mix of sensitive analogue and digital in my purpose built
multiphase controller consisting a mixture of op-amps, discrete
transistors, high speed comparators, ADC, DAC, programmable logic & a
microcontroller.
Is it feasible to separate analogue and digital components so they are
placed directly on opposites sides of the PCB, and use separate
non-isolated ground planes ?
I am speculating that return currents from digital lines should only
flow in the adjacent ground plane layer, and not interfere with
subsequent ground and signal layers. For a 6 layer stack I am
considering:
[analogue components]
--------------------------
L1 analogue signal
L2 ground
L3 power (analogue)
L4 power (digital)
L5 ground
L6 digital signal
------------------------
[Digital components]
L2 and L5 will be connected only in limited locations.
[analogue components]
--------------------------
L1 analogue signal
L2 ground (digital)
L3 power (analogue)
L4 ground
L5 ground
L6 power (digital)
L7 ground (digital)
L8 digital signal
------------------------
If you can get away with it.
