Avoid zone fill with single net point

[SukkoPera]

Is there a way to avoid a zone fill to extend on a section of the board where there is only a single pad belonging to that net?

I would like to avoid things like the following:

[pedro]

Yes, a keepout zone where yo don’t want the filled zone.

Or redraw the zone and avoid covering the unwanted area.

[SukkoPera]

Of course, but the zone is actually the ground fill for the whole board and doing that manually would be cumbersome. I guess I have no choice :).

[eelik]

You can stitch the back and front copper zones together.

Here are a couple of potential places. With using some small effort you can push some tracks and vias and optimize the areas and connections.

[paulvdh]

I sometimes lay a track on areas like that.
Then I lay that track from one GND pad to another GND pad (or a via) through the GND zone. The goal is to let this track get shoved around a bit by the interactive router, but not let it break the connetion between one piece of a GND plane to another section of the GND plane.
In the example that eelik posted, you could draw a track from (Pin 6 GND) to via locations 2 & 3. This pushes aside the ~RDY~ net and lets the copper flow into that section.

I also advise you to make a checklist for final things to check & cleanup before you generate Gerbers. One of the items on the checklist should be to verify the quality of the GND zones.

[Robert_Loos]

You may edit the properties of that particular pad:

but I think it will be reverted if you update the footprint from library.
Why do you want to avoid it at all? I don’t think it has negative effects except if you have to save weight.

[paulvdh]

In a more general sense:
It does not make much sense to have bits and pieces of GND plan on different layers. It is much better to have a single big and continuous GND plane on one layer, and no GND plane on any other layer at all. It is not the amount of copper area in the GND plane that counts, it is the continuity through that plane, and every layer change breaks that.

Therefore: Choose one layer for your GND plane, and remove your GND fill from the other layer altogether. Then move as many as possible tracks away from the GND plane layer, and make the remaining track pieces as short as possible. Some small holes in the GND plane are not a big deal (unless you go to real high frequencies). As a guideline, try to keep holes in the GND plane below 5mm.

This is just a simple guideline. For a real analyses you need to consider the return path of each and every signal track and how the current flows through the GND plane. That is not easy to do (There is specialized software for that, called a “field solver”).

Also:
Read and study some articles about EMI and PCB layout. There is lots of info on the 'web.

[Robert_Loos]

Paul, I completely agree with you and Eelik. But just to answer the original question: with regard to crosstalk, it is better to have a piece of ground between two signals than only a gap.

[paulvdh]

I’m not entirely sure here, but as I understand it, a (widish) gap is better then a “finger” sticking out of a GND plane. A piece of copper, even if it is connected to a GND plane some place further acts as an antenna just picks up the noise and sends it further.

A wider gap reduces capacitance and EM field pickup.

The original question is about removing small zone fills which only have one pad, and removing the zone altogether is very likely the best way to do it. (Combined with increasing the GND zone area & continuity on the other side of the PCB.