How do I Prevent a filled zones from connecting between SMD pads?

[Billy_B]

Is there a good way to keep plane fill zones from connecting between pads of an SMD component?
The GND pads on the left is the behavior I want, the GND pads on the right is the behavior I don’t want.

I have used the following in the past:

1. Adding keepout areas between Zones - tedious for boards with lots of components.
2. Drawing the fill zone so it surrounds each pin - also tedious for multiple components.
   
3. Adding a small pad that will not connect to Fill-Zones - this is tedious and I could see future updates to KiCad Breaking the Zone fill connections because the fill-zone keeps the copper outside the pad clearance of pads that are set to not connect to fill-zones
   
   
   

[paulvdh]

You can set “Pad connections” to “None” in the zone properties:

But then you’re responsible yourself for how to connect pads to zones.

[ronsimpson]

@Billy_B

keep plane fill zones from connecting between pads

Why? I would just let it do the job.
I think you can make a keep out zone from left to right down the connector. Do not cover the top of the connector. One zone, not one for each pin. I have not tried it. I think you have to check “zone fill” box.

[Piotr]

@Billy_B

to keep plane fill zones from connecting between pads of an SMD component?

According to my experience there is nothing wrong in connecting between such pads until there is enough room between them for solder mask (it looks you have enough room).
If there is not enough room and opening in solder have to be common for all pads then such connections tend to make tin to make bridges between consecutive pins. That is also technically accepted but looks ugly.

@paulvdh

You can set “Pad connections” to “None” in the zone properties:

I would change Pad connection to None for selected footprints or only selected pads allowing the rest to be connected ‘as usual’.

[Billy_B]

@Piotr

According to my experience there is nothing wrong in connecting between such pads until there is enough room between them for solder mask (it looks you have enough room).
If there is not enough room and opening in solder have to be common for all pads then such connections tend to make tin to make bridges between consecutive pins. That is also technically accepted but looks ugly.

I am designing the boards so a board house can assemble and inspect the PCB’s.I like to keep connected pins connected outside the footprint so the technician doesn’t have to reference documentation to see that two pins are supposed to be connected.

[Piotr]

@Billy_B

so the technician doesn’t have to reference documentation to see that two pins are supposed to be connected.

Are you sure they work that way and it is important for them?
I am not telling that you wre wrong. I just don’t know, but I never had any problem in connecting adjacent pads directly until I got 0.4mm raster and such pads looked as being shorted. But it passed through automatic optical test (our contract manufacturer uses for all assembled PCBs) without any problem as tester knew (I suppose from gerbers) that those pads are connected. That only looked ugly for human so I changed it.

It looks that KiCad also has nothing against connecting such pads directly.

[Naib]

If you really do not want such connections, one option could be to use the KEEPOUT area tool and draw a box around such parts in question and set the rule to keep copper zones (while permitting traces)

Such keepouts are really useful and have been expanded to cover DRC rules in v5.99