Danling Ground copper areas on PCB

[madhu.wesly01]

Hi,

Can someone share the best practices to avoid dangling ground on PCB, and mitigating tips in-case of unavoidable cases.

Is using polygon cutout good practice for eradicating the dangling ground copper areas? In this method will there be any impact in performance for signals or components if there is no GND copper around(near) them?   

TIA.

[T3sl4co1l]

1. For the most part, don't bother pouring outside or signal layers on a multilayer board.  Can be helpful in demanding cases, but isn't worth the trouble for the most part.

2. In 2-layer designs, pour the same net (GND) both sides, and stitch with vias.  This connects peninsulas, crossings and islands, and provides a ground nearly as good (in terms of impedance and average distance from trace to ground) as a multilayer board.

3. Any islands remaining, should simply be too small to bother pouring or connecting (set a minimum island area threshold).

Tim

[DaJMasta]

Does your CAD tool have an option to do this automatically?  In the software I've been using (CircuitMaker, basically Altium Designer with a less useful UI) you just check a box when you define your polygon pour and the system won't generate any part of the plane that would be floating.


For high speed signals using controlled impedance models, the distance to a ground is important but this is probably not your application.  For using ground as 'shielding', if it's not there it doesn't provide the benefit, but it's otherwise no difference.  Via stitching in key points can usually connect stray bits of the pour, but leaving it out in an area you can't connect isn't likely to have a big effect - things are probably dense enough that there's not going to be much stray signal penetration there anyways.

[Miti]

3. Any islands remaining, should simply be too small to bother pouring or connecting (set a minimum island area threshold).

In Eagle there's a check box in the polygon properties named "Orphans" that can leave or eliminate the unconnected islands.
I use a healthy amount of stitching vias between top and bottom with reasonably big drill size to minimize the via resistance.

[madhu.wesly01]

Hi,

@Miti, in my case there are no unconnected islands. All the (GND)copper pour(even islands if any) connected to Ground some how on my 4 layer PCB.

@DaJMasta, I use KiCAD, I am not sure if it has that check box.

Please have a look at the image attached.

[EEEnthusiast]

you can set a larger clearance area for the ground pour so that it does not creep into smaller spaces.
May be a 1mm spacing