PCB Gridding vs multipoint/star point.

[electronicsfreak]

Hello everyone.

Please forgive me if this seems rudimentary, but I really do want to know. What exactly is gridding when it comes to distributing a ground connection across a printed circuit board? I've found a few articles on it, but in all honesty, I'm reading it as though doing such a thing will create multiple ground loops within such a circuit, something I've learned in the past that is a terrible thing to do.

I've made simple proto/perf-boards before simply distributing power/ground in a star/daisy-chain format, but given the opportunity to make a 2-layer PCB I'd love to try to reduce whatever noise I've got in this project. Any thoughts?

Thanks fellas!

 

[ronsimpson]

I don't do "gridding" I use solid copper.

It is done because if a large PCB has mostly copper on one end and mostly no copper on the other end it will warp. (one side/other side) With gridding you can have a ground that is 75% or 50% copper and more match the other part of the board.

The holes in the grid should be small and not a problem if you stay below 10ghz.

 

[Mike odom]

Using a grid on a ground AND power supply on a pcb does not cause ground loops, it decreases them. When you're trying to use a shield, you tie one end to ground. Tying two points to ground allows outside signals to flow from one of the points to the other, causing a ground loop and introducing a noise current into the circuit you're trying to protect. This is done because any flow of current causes a magnetic field, which when passing through the wires/circuitry produces a noise current into that circuit.

As for ground/power supply runs on a pcb board, you want the current in path to follow the current out path as closely as possible, to reduce the 'loop size' and thus reduce interference the loop emits or picks up. A solid plane is best, as current can go anywhere it wants, and will follow the supply current. If you can't use a solid plane, then a grid is best. Of course, the mulitpoint star is the best of all, that way you don't have currents from circuit A flowing in circuit B, and vice versa, but this is not always possible, especially in a digital circuit with high density pin counts. When I lay out a pcb board, I route power and ground first. I lay in a grid (both power and ground), verticals on top and horizontals on bottom. Every column, every row. Then when routing I take away only the traces I need to to squeeze signal runs in. Whenever I think about how I'm going to place the parts, I always have ground and power feeds in mind.

Grids are only better than solid planes as mentioned above, if you have a large plane on the bottom and almost no copper on top above it, the board will warp. A way around this is to copper fill a ground plane on top, or even floating copper (not tied to power or ground), and only etch off enough copper to supply a space between runs.

Multilayer is excellent because you get a whole plane for both power and ground.

Also, it is bad practice to run power on one end of the board and ground on the other. They should come in at the same end of the connector and be routed as close together as possible.

When routing high power circuits and low power/sensitive circuits on the same ground, put the high power stuff closet to the power supply, and the low power stuff out on the end of the run. The low power stuff will not interfere as much with the high power stuff and the high power will distort the low power runs. The distortion is called 'ground bounce' and it due to ohm's law (the basic law of current flow). Copper traces have resistance, and current flowing through them will drop a voltage across a length of copper. The bigger the traces, the lower the resistance. This is why decoupling capacitors are placed next to ICs, so they can supply the high frequency hi current draws when the circuits switch, and hold the voltage steady, and then refill from the bus.

 

[throbscottle]

Now you mention it... Does floating copper have any meaningful effect on small signals and high Z circuits? Can it act as a kind of "floating shield"? I've always wondered, and since milling with a dremel type tool is my only means of making pcb's now it could be an issue.

 

[Mike odom]

no, floating copper won't stop the E field, so it doesn't act as a shield. It has to be grounded (or tied to the power bus) at one point only to act as a Faraday Shield (on a pcb it's called a guard ring). Tying it to two or more points connects it into the ground (or power) bus. Currents will then flow through it. This could be good or bad. If you tie it into the ground bus, and there are nearby power runs, it will neutralize the effect those power runs have on your local circuits. If there are no power runs, it will affect the circuits. Intel has an extremely good app note on this, I'll see if I can dig it out. My best investment when I first got into engineering (in 1982) was a book called "Grounding and Shielding Techniques in Instrumentation". Still available today... what I learned by reading that just once 30 years ago I have put to good use and solved many (many) system problems that other engineers thought were head scratchers... they just weren't seeing the problem from the right perspective.

 

[throbscottle]

One of those things that when someone explains it is obvious, but it's really good to be told Would certainly appreciate a look at that app note - though I'll have a hunt for it on their site anyway.

Thanks

 

[3v0]

This should be moved to
Circuit Simulation & PCB Design

 

[throbscottle]

It wouldn't be app note 589 Design for EMI, would it, Mike?

 

[cachehiker]

Intel has an extremely good app note on this, I'll see if I can dig it out. My best investment when I first got into engineering (in 1982) was a book called "Grounding and Shielding Techniques in Instrumentation".

Hoping and waiting for the first.

Will be investigating the second.