vias between parallel planes and traces?

[Michael Noone]

Hi - I am finishing up work on a 2 layer board. The bottom copper is a
ground plane (though it is interrupted in many places by mostly short
traces). The top copper also has in one place a ground plane that is used
to protect a particuarly sensitive module. My primary question is this: How
should I connect these two ground planes? I figure I should just
periodically place VIAs between them. But how many vias and how often? A
via/cm^2? 10 vias/cm^2? I should note that almost the entire board is
surface mount, so there are few pins going between the planes connecting
them. Or - instead of distributing them evenly - should I be 'tacking' the
corners of the top (smaller) ground plane with vias? Or should I be making
a sort of line of vias around the border of the top ground plane?


On a very related note: I have two DC/DC modules on the board. Connected to
each are two fairly large surface mount capacitors (1 Panasonic G package
and 1 1210 package). These capacitors are connected between ground and the
output of the DC/DC modules. There is a ground plane beneath them (the one
on the bottom copper). What I am unsure of is this: should I connect a
trace between their grounded sides and the ground pins of the dc/dc
switchers? Or, should I put vias on them going straight to ground. Or,
should I connect a trace between them and the ground pin on the dc/dc
switcher and also put vias on that trace connecting it to ground? Right now
I'm favoring the third of those - but I'm unsure. If I do it that way, same
question as above, how many vias should I be putting on the traces? They're
fairly hefty - 2mm in width. Or - should I connect them in some other way?

Thanks,

-Mike

 

[John Popelish]

Hi - I am finishing up work on a 2 layer board. The bottom copper is a
ground plane (though it is interrupted in many places by mostly short
traces). The top copper also has in one place a ground plane that is used
to protect a particuarly sensitive module. My primary question is this: How
should I connect these two ground planes? I figure I should just
periodically place VIAs between them. But how many vias and how often? A
via/cm^2? 10 vias/cm^2? I should note that almost the entire board is
surface mount, so there are few pins going between the planes connecting
them. Or - instead of distributing them evenly - should I be 'tacking' the
corners of the top (smaller) ground plane with vias? Or should I be making
a sort of line of vias around the border of the top ground plane?


On a very related note: I have two DC/DC modules on the board. Connected to
each are two fairly large surface mount capacitors (1 Panasonic G package
and 1 1210 package). These capacitors are connected between ground and the
output of the DC/DC modules. There is a ground plane beneath them (the one
on the bottom copper). What I am unsure of is this: should I connect a
trace between their grounded sides and the ground pins of the dc/dc
switchers? Or, should I put vias on them going straight to ground. Or,
should I connect a trace between them and the ground pin on the dc/dc
switcher and also put vias on that trace connecting it to ground? Right now
I'm favoring the third of those - but I'm unsure. If I do it that way, same
question as above, how many vias should I be putting on the traces? They're
fairly hefty - 2mm in width. Or - should I connect them in some other way?

Before I try to answer your ground plane questions, I would like you
to describe why you have a ground layer. What (and be as specific as
possible) is it supposed to do for your circuit? Does it do different
things for different parts of the circuit? You may find that you are
answering your own questions.

 

[Michael Noone]

Before I try to answer your ground plane questions, I would like you
to describe why you have a ground layer. What (and be as specific as
possible) is it supposed to do for your circuit? Does it do different
things for different parts of the circuit? You may find that you are
answering your own questions.

OK well the top ground plane is for a very specific purpose: it is directly
below a compass module that is very sensitive to interference and whatnot.
Unfortunately I had to run some signal lines directly beneath it so I moved
them to the bottom layer and then put the ground plane above them on the
top layer to shield the module from the signal lines (they're SPI lines
that will be running at about 5Mhz as I recall). The datasheet for the
compass module very specifically stated not to run any traces directly
beneath the module, so this was the best I could do.

The other ground plane is there, to me, for three main reasons:

-simplify layout by making a ground signal always readily available
-give lots of copper to ground signal to decrease resistance
-provide a sort of shield to the circuit board. (this is something I've
always been told)


So with all that said I'm still not entirely sure about how to answer my
questions... Any suggestions?

Thanks,

-Mike

 

[John Popelish]

OK well the top ground plane is for a very specific purpose: it is directly
below a compass module that is very sensitive to interference and whatnot.
Unfortunately I had to run some signal lines directly beneath it so I moved
them to the bottom layer and then put the ground plane above them on the
top layer to shield the module from the signal lines (they're SPI lines
that will be running at about 5Mhz as I recall). The datasheet for the
compass module very specifically stated not to run any traces directly
beneath the module, so this was the best I could do.

Excellent information. I suspect a compass module is not only
sensitive to electric fields but also to magnetic fields. This means
that you want as little current passing through that section (you can
section the ground plane and tie the pieces together at points of your
choosing that guide currents) of the ground plane as possible, so that
section should be isolated from supply current fed through the ground
plane. And any traces that pass under it, if they carry any
significant current, should be in the form of transmission lines with
the return current passing along side, going the other way, to cancel
the external magnetic field from that current. In this case, such
cancellation should be used for all large currents in the general
vicinity of the compass.

The other ground plane is there, to me, for three main reasons:

-simplify layout by making a ground signal always readily available
-give lots of copper to ground signal to decrease resistance
-provide a sort of shield to the circuit board. (this is something I've
always been told)

Well, the shield can be useful to keep outside electric fields away
from your traces and components, or from communicating between them,
but also to keep the electric fields of your traces and components
from getting out into the surroundings.

The ground plane can also be a voltage reference for either logic or
analog circuits, or both. It is especially important to keep supply
current out of the parts that are analog references.

And, of course, the plane is a path for supply current, if that
doesn't conflict with the above use. Noisy and high current supply
grounds may be better run as traces, to keep the I*R drop caused by
these currents out of a clean ground plane.

So with all that said I'm still not entirely sure about how to answer my
questions... Any suggestions?

Just to think about all the possible uses of the ground plane and how
one use may be in conflict with another. Every pour should have
specific purpose(s) in mind, not done just because you can.

 

[Jason Dugas]

Hi - I am finishing up work on a 2 layer board. The bottom copper is a
ground plane (though it is interrupted in many places by mostly short
traces). The top copper also has in one place a ground plane that is used
to protect a particuarly sensitive module. My primary question is this:
How
should I connect these two ground planes? I figure I should just
periodically place VIAs between them. But how many vias and how often? A
via/cm^2? 10 vias/cm^2? I should note that almost the entire board is
surface mount, so there are few pins going between the planes connecting
them. Or - instead of distributing them evenly - should I be 'tacking' the
corners of the top (smaller) ground plane with vias? Or should I be making
a sort of line of vias around the border of the top ground plane?


On a very related note: I have two DC/DC modules on the board. Connected
to
each are two fairly large surface mount capacitors (1 Panasonic G package
and 1 1210 package). These capacitors are connected between ground and the
output of the DC/DC modules. There is a ground plane beneath them (the one
on the bottom copper). What I am unsure of is this: should I connect a
trace between their grounded sides and the ground pins of the dc/dc
switchers? Or, should I put vias on them going straight to ground. Or,
should I connect a trace between them and the ground pin on the dc/dc
switcher and also put vias on that trace connecting it to ground? Right
now
I'm favoring the third of those - but I'm unsure. If I do it that way,
same
question as above, how many vias should I be putting on the traces?
They're
fairly hefty - 2mm in width. Or - should I connect them in some other way?

Thanks,

-Mike

Mike,

For your DC/DC converters, here is some basic information you should know
and some basic questions you should ask:

1.) What are the two surface mount capacitors being used for?

There are pretty much only two possibilities-- filtering or reservoir.
Filtering would be to make sure that any noise superimposed on the DC
output of your converter gets passed to ground and DOESN'T make it to the
load.

Reservoir would be for the purpose of ensuring that there is always
enough energy in reserve in order to maintain the proper voltage across the
load. If your load requires short bursts of current, then this capacitance
would act as a buffer between the output of the converter and the load. If
this capacitance *IS* in the circuit for the purpose of being a reservoir
then you would certainly want this capacitor connected directly across the
output terminals of the DC/DC converter (from + to -). Whether you have the
ground plane connected to the negative leg of the converter's output is
completely arbitrary-- the reservoir will perform the same function,
regardless.


2.) If this capacitor is for filtering, then what type of noise are you
trying to filter?
There are two possibilities here as well-- common mode & differential.
And this is where putting the cap from + to - or + to GND would make a
difference.

If you place a capacitor from + to - (as in the reservoir mentioned
earlier) you will effectively be sinking differential noise to ground.

Another technique is used when common-mode noise is problematic. In
this case you would want TWO capacitors-- one from the positive leg to GND
and one from the negative leg to GND. This will create a low-impedance path
for common-mode signals. (BTW, you'd want each of those caps' negative leg
tied to that ground plane you mentioned with a via).

Typically, common mode noise will not cause significant issues in many
designs and differential noise is tends to worry more people on average.

Hope this helps some.

Good luck with your project.

Jason

 

[Ken Smith]

Hi - I am finishing up work on a 2 layer board. The bottom copper is a
ground plane (though it is interrupted in many places by mostly short
traces). The top copper also has in one place a ground plane that is used
to protect a particuarly sensitive module. My primary question is this: How
should I connect these two ground planes? I figure I should just
periodically place VIAs between them. But how many vias and how often? A
via/cm^2? 10 vias/cm^2? I should note that almost the entire board is
surface mount, so there are few pins going between the planes connecting
them. Or - instead of distributing them evenly - should I be 'tacking' the
corners of the top (smaller) ground plane with vias? Or should I be making
a sort of line of vias around the border of the top ground plane?

Just for sheilding:

The main issue is one of frequency. At DC, one ground connection makes
the whole plane at the voltage give or take an IR drop or two. At audio
frequencies, you can usually just assume the DC values apply. At low
frequencies, the shield is acting electrostatically.

If are working with higher frequencies, the drop on the plane starts to
depend on the fraction of a wavelength you are from the via. The pair of
planes looks like a transmittion line. This line will have a low Z0
(impedance) and "c" (speed of light). Any RF currents, including those
from a switching converter, will generate signals in this line. You
should make the longest distance between vias less than 1/20th of a
wavelength.

Trust me on this: A nice pretty pattern of ground connections can end up
being completely useless at some very high frequency, which it will always
turn out to be a trouble maker. Don't make a nice pattern.

The ground of other circuits:

If you have a DC-DC convert or other part that sloshes large currents
around, you want to pay careful attention to the currents. You want to
reduce the area enclosed by the paths of the AC currents. Arrange the
parts so that the total loop is as small as practical. All lines that
enter or leave the DC-DC converter should have an impedance in series and
a capacitance to one ground point. Ideally you want the ground of the
DC-DC converter to hook to the plane at only the same point:

ASCII art:

-------
--+----\/\/-------! !
! ! !
! ---+---/\/\---! DC-DC !
! ! ! !
--- --- -------
--- --- ! ! !
\ ! ! ! !
\ ! ! ! !
-*-----------+--+--+-------- Local ground plane
!
-------+--------------------------- Global ground plane