What's the purpose of a grid or lattice-shaped ground plane?

[Taylor]

For example:

http://www.sixproducts.com/wordpress/wp-content/uploads/weak-groundplane.jpeg

http://lh4.ggpht.com/_BGvgroHHiOU/SmqMWQIkRBI/AAAAAAAADXc/YV2hS7zMJro/s800/ground-island-via-pwb.jpg

I have previously read about this - some things said that the idea was to use less plating material, or that it helps the soldermask adhere to the surface. However, lately I've seen some home-etched boards which use this kind of ground plane, so this can't only be an issue of fabrication. It must have something to do with impedance or something. Or to minimize ground loops?

Anyone know why this is done?

[edvard]

Maybe because a filled ground plane would act like a parasitic capacitance to ground? :shrug:

[amptramp]

It may be to alleviate stress from the differential coefficient of expansion of epoxy-glass and copper.  Back when I was working on avionics equipment, I used a local board manufacturing facility (Graphico Precision) that did all types of boards including multilayer.  A standard test for delamination was to submerge the boards in 425 degree F peanut oil.  If it survived that, it was good enough for a flow soldering operation.

[R.G.]

It is for thermal reasons as AT mentions, and for etching convenience.

Gridding makes the mechanical strength of the ground plane smaller, so the pull it absorbs on thermal changes can be more easily accommodated by the thin sections instead of a solid sheet. It's easier to stretch many thin wires than one solid sheet. This makes the board bow much less on changes in temperature. The difference in thermal coefficient makes for bowing of the board and in extreme cases at high temperature, delamination as the heat softens the epoxy and the push or pull loosens the copper.

It's also good practice in etching. It would be ideal when etching a double sided board if both sides had about the same % coverage of copper over the area. This lets the etching process proceed evenly and doesn't require you to etch one side too much to get rid of all the copper on the "slow" side. This used to be a big deal a few decades ago, but modern spray etchers have made it almost moot. Equal % copper on both sides is also good practice where boards will get hot, as the different forces on top/bottom will stay balanced and the board will stay flatter.

A gridded ground plane is a theoretically poorer ground plane, as it reduces the average conductivity of the ground plane by filling it full of non-conductive holes. But this is generally not an issue for audio.

[Earthscum]

May be a silly question, but would using the unused copper on top to make a ground plane help reduce bleedthrough from LFO's (my problem as of late), or in high impedance circuits such as analog CMOS applications?

I've done this on a couple boards in the past, only etching out .1" holes where leads can go through without contact, and soldered grounds on top and bottom (still running ground traces), but I really don't know if it made a difference because I didn't do a normal board to compare it with. <shrug> (early boards, and I didn't want to waste the etchant at the time. Noob thinking I guess.)

[R.G.]

May be a silly question, but would using the unused copper on top to make a ground plane help reduce bleedthrough from LFO's (my problem as of late), or in high impedance circuits such as analog CMOS applications?

I've done this on a couple boards in the past, only etching out .1" holes where leads can go through without contact, and soldered grounds on top and bottom (still running ground traces), but I really don't know if it made a difference because I didn't do a normal board to compare it with. <shrug> (early boards, and I didn't want to waste the etchant at the time. Noob thinking I guess.)

Not silly, but perhaps not simply answerable. It depends on where the topside copper is connected, where it's interrupted, what the source and termination impedance of the signals are, their highest frequency components, the width of the traces across/around it, and what other signals are nearby.

Adding ground plane because you can seems like one of those good ideas, but it can bite you. First, it raises the parasitic capacitance of the traces near/over it. That may not make a difference unless you are using high impedance inputs like we do with CMOS, JFET or MOSFETs. It generally helps reduce crosstalk of traces - unless there is a heavy ground current that happens to run under the trace you're trying to keep quiet. At DC, ground planes don't help you much. All that matters is raw resistance. At power line frequencies and low audio, ground planes don't help much, especially when you want to control exactly where ground currents flow so you can avoid ground noise. There may be a voltage drop in your grounds, but it won't contain other contaminating signals if you do star grounding. Generally this is true up through audio. Ground planes can help where you need shielding, but the shielding a plane can do is limited. As you get into RF, ground inductance is a much bigger issue than ground resistance, and field effects make the ground currents "want" to run right under the conductors which carry the signals for which the ground currents provide balance. The circuit makes its own point to point grounding out of the plane, dynamically as signal currents flow.

It's not necessarily a bad idea, but it's not an unqualified good idea either. The devil is in the details.