vias between parallel planes and traces?

John Popelish wrote in news: snipped-for-privacy@adelphia.com:

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

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.

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.

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.

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.

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

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

--
--
kensmith@rahul.net   forging knowledge