Grounding

If it was my board, I wouldn't put ant grounds on top unless I had a particular reason for doing so. I would stitch short jumpers across any slots in the bottom side plane caused by bottom side traces, to improve the continuity of the plane. I would use pairs of grounded traces (or surrounds) to shield particularly sensitive signals, or to contain the noise or control impedance for particularly powerful or fast signals. Otherwise ground pour islands are just antennas.

Reply to
John Popelish
Loading thread data ...

Hi All,

I know this subject has been beaten to death but I thought I would check people's latest thoughts anyway.

I have a PCB with 2 switch mode power supplies and a PIC with a few other bits and pieces. Most of the tracks are on the topside of the board and I have used the bottom layer for a ground plane but it still has a few tracks and components. I have connected all of the ground pads on the topside of the board to the ground plane on the bottom layer via via's. In the past I have simply poured the copper ground plane on both layers anywhere it fits with 25mil clearance but lately I have been thinking this might not be the best way as it doesn't necessarily leave much control over where the ground current will flow. This time have split the bottom ground plane up into power and digital grounds with them connecting at one point.

Now I am a bit confused as to what I should do with the top ground plane. If I pour copper over the top without regard, I will end up with some multi point grounding, where the ground pads are connected to the bottom plane at more than one point. Would it be wise to not use a top ground plane at all to prevent this and carefully control the ground currents to minimize noise?

Regards,

AJ

Reply to
AJ

Where the bottom side ground plane has a trace plowed through but you wish the plane continued is the place to think about. In that area, you use traces, pours and vias to cover over the trace that was plowed in, as much as you can.

This means that you are likely to end up pouring as many plane sections on top as you did on the bottom.

Reply to
MooseFET

If the board did contain any particular sensitive signals, controlled impedances or particularly fast signals, I would be hesitant to use a two layer board to begin with. Increasing to at least a four layer board would provide you with a solid power and ground plane that will act as a reference for your high speed signals and allow you to generate controlled impedances, which are a function of the geometry.

On simpler designs that are predominantly low speed and low frequency, I commonly use a copper pour for a ground plane and sometimes use a top pour for the power. With judicious and proper use of decoupling capacitors and sufficiently wide traces, the power connections can be more arbitrary, but a low impedance ground is still a must.

Reply to
Noway2

Thanks for the input guys, I have tried to implement your idea's.

Best regards,

Adrian Hamilton

Reply to
AJ

Going to 4 or more layers is often a superior approach, and it may not be as costly as you suppose. However, if you're stuck with 2 layers: Provided that you can adequately 'stitch' the layers together with vias, incomplete copper pours on different layers can improve grounding. However, this may require more vias than are economical, since board cost is partly determined by the number of holes. The key layout rules to observe:

1) Do not allow high speed signal lines to cross 'slots and moats', since their associated return currents will be forced to go around the slot or moat, creating a loop that represents an impedance discontinuity, parastic inductance, and EMI radiator. 2) Take particular care to stitch any 'flags', which are elongated copper pour regions. Any dv/dt on flags will radiate, i.e., EMI currents will flow through parasitic capacitance to the flag region. 3) Pitch of stitching vias should be on the order of 1% of a wavelength of the highest harmonic frequency originating in the circuit or present in the ambient. For the mixed 100MHz DSP and 20-bit codec boards I've designed, this usually meant vias every 5 mm or so. Note that this is a density of 4 vias per sq cm, which is as many as 400 extra vias on a 10cm x 10cm board. Paul Mathews
Reply to
Paul Mathews

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.