ground plane connections

J

Jamie Morken

Guest
Hi all,

When using a high frequency (1MHz to 3MHz) stepdown buck switcher on a
board to generate the 5Volt rail, what is the best way to connect the
switchers ground plane to the rest of the 5Volt ground plane? Is a
single point connection good to use to reduce noise, or is it better
just to make one big ground plane under the switcher circuitry and the
5V circuitry?

cheers,
Jamie Morken
 
"Jamie Morken" <jmorken@shaw.ca> wrote in message
news:psNnd.195871$9b.79390@edtnps84...
Hi all,

When using a high frequency (1MHz to 3MHz) stepdown buck switcher on a
board to generate the 5Volt rail, what is the best way to connect the
switchers ground plane to the rest of the 5Volt ground plane? Is a single
point connection good to use to reduce noise, or is it better just to make
one big ground plane under the switcher circuitry and the 5V circuitry?
Click to expand...
The switcher chip manufacturers usually have recommended PCB layouts.

Leon
--
Leon Heller, G1HSM
http://www.geocities.com/leon_heller
http://www.kasamba.com/viewExpert.asp?conMemID=105725&Catid=1111&banID=2100
 
On Sat, 20 Nov 2004 20:05:41 GMT, Jamie Morken <jmorken@shaw.ca>
wrote:

Hi all,

When using a high frequency (1MHz to 3MHz) stepdown buck switcher on a
board to generate the 5Volt rail, what is the best way to connect the
switchers ground plane to the rest of the 5Volt ground plane? Is a
single point connection good to use to reduce noise, or is it better
just to make one big ground plane under the switcher circuitry and the
5V circuitry?

cheers,
Jamie Morken
Click to expand...
Just one common plane for the whole board is usually fine, unless
you're doing very low-level stuff. Keep the low side of the input cap,
the anode of the catch diode, and the low side of the output cap very
close to minimize broadcasting the circulating switching current about
the plane.

Some people like to cut a c-shaped relief in the ground plane and tuck
all the switcher parts on the resulting peninsula to keep circulating
currents out of the rest of the plane, but that's not normally needed.

What else is on the board?

John
 
In article <psNnd.195871$9b.79390@edtnps84>,
Jamie Morken <jmorken@shaw.ca> wrote:
Hi all,

When using a high frequency (1MHz to 3MHz) stepdown buck switcher on a
board to generate the 5Volt rail, what is the best way to connect the
switchers ground plane to the rest of the 5Volt ground plane? Is a
single point connection good to use to reduce noise, or is it better
just to make one big ground plane under the switcher circuitry and the
5V circuitry?
Click to expand...
It depends a great deal on what the rest of the board has on it and what
it hooks to. In digital logic cases it is almost always ok to just hook
the switcher stuff straight to the boards ground plane.

If the circuit has analkog stuff or something else that can be disturbed,
you want to make sure that the AC currents all stay local to the switcher
section. This is usually done by careful parts placement adn perhaps
using a layer of the PCB as an extra ground layer.


/
------+----/ 0---+----))))))------- To load
! !
--- ---
--- ^
! !
+---------- Local plane or careful placement
!
--------+-------------------- PCB ground plane


In extreme cases where you have very small signals near the switcher, it
is best to layout as though you will be adding a shield. It costs almost
nothing extra in the board design and if it turns out you need the shield,
you have a place to put it. I have resorted to having the switcher on its
own plane above the PCB's ground plane and running all the lines in and
out through inductances. It sort of like this:


........ Shield ............
. .
. ------------ .
Vin -+-[L1]-+---! Switcher !----+--[L2]-+---- Vount
! . ! ! Circuit ! ! . !
--- . --- ------------ --- . ---
--- . --- ! --- . ---
C1 ! . ! C2 ! C3 ! . ! C4
! . ---+-----+--------- . !
! . ---+ . !
! ....!.[L3].................. !
! ! !
---+----------+-----------------------+--- GND

L1, L2 and L3 are all on the order of 1uH and are lossy.

The impedance of L1 forces the AC current to flow in C2. You can't use a
large inductance here because larger inductors have too much stray
capacitance. You must maintain a high impedance at high frequencies. L1
also reduces the conducted EMI on the input power.

L2 serves very much the same purpose as L1. From an EMI point of view it
usually matters less than L1. From a circuit performance, it often
matters more.

L3 is a bit of an oddity. If the shield is used, the drops caused
by ground currents will tend to drive it with an AC waveform. The
losses of L3 prevents the shield from tuning up at some frequency.
--
--
kensmith@rahul.net forging knowledge
 
Hi Jamie,

One big old common ground plane is what I found to work best for most of
my designs. And also for those that I had to redesign. This included one
design where the switcher provided 5V at up to a whopping 100 amps.

However, it helps to still adhere to Ken's advice of keeping currents as
local as you can. That means not placing the inductor too far away from
the FET. The same goes for the path to decoupling caps, Schottkys and so
on. In other words anything where high currents are abruptly changing
their path. With regard to noise issues decoupling caps have to be seen
as the 'real' power supply in switchers since that is where almost all
the short term energy gets drawn from or is dumped into.

Regards, Joerg

http://www.analogconsultants.com
 
"Jamie Morken" <jmorken@shaw.ca> wrote in message
news:psNnd.195871$9b.79390@edtnps84...
Hi all,

When using a high frequency (1MHz to 3MHz) stepdown buck switcher on a
board to generate the 5Volt rail, what is the best way to connect the
switchers ground plane to the rest of the 5Volt ground plane? Is a
single point connection good to use to reduce noise, or is it better
just to make one big ground plane under the switcher circuitry and the
5V circuitry?

cheers,
Jamie Morken
Click to expand...
The decision for splitting the ground depends largely on the peak currents.
For most of the low powered switchers a large common ground plane is preferred,
as long as the switcher is grouped for the shortest spacing so as to localize
the currents and minimize the IR drops. For really high currents, say over 10
amperes, you must consider the current path on the board and decide whether to
group and split the ground plane to limit influence from the high peak
currents.

Remember a single point connection has a finite resistance which must be
minimized to avoid heating the board.
 
Hi Clarence,

Remember a single point connection has a finite resistance which must be
minimized to avoid heating the board.
Click to expand...
Also, don't send lots of amps through one lone via until it gloweth in
the dark ;-)

Regards, Joerg

http://www.analogconsultants.com
 
Joerg wrote:

Hi Clarence,

Remember a single point connection has a finite resistance which must be
minimized to avoid heating the board.



Also, don't send lots of amps through one lone via until it gloweth in
the dark ;-)

Regards, Joerg

http://www.analogconsultants.com
Click to expand...
Damn, here I was thinking Copper is a room-temperature superconductor. doh.

You can work out the current-carrying capacity of vias by assuming the
via wall thickness is 1/2 that of the pcb copper cladding.

Cheers
Terry
 
"Joerg" <notthisjoergsch@removethispacbell.net> wrote in message
news:q4tod.48593$QJ3.28799@newssvr21.news.prodigy.com...
Hi Clarence,

Remember a single point connection has a finite resistance
which must be minimized to avoid heating the board.

Also, don't send lots of amps through one lone via until it gloweth > in the
dark ;-)
Regards, Joerg
Click to expand...
Oh yes! Or char the board!
For surface mounts in even a relatively low powered buck regulator I often use
six vias for the caps, and at least the same for the diode. The vias for this
purpose are larger ones, not .01 In Dial, if space is available I want them
more like .03 dia to get more plating.

However the "single" point may be one entire side of the circuit area with only
a narrow isolation on three sides. This arrangement will still avoids the
currents in the supply being in the ground circuit of other portions of the
circuit.
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top