Want to isolate a SMD pad from the surrounding copper zone although both are the same net.
When opening the tab “Connections” in the “Pad Properties” I can see a dialog field called “Pad Connection”. By selecting “None” I hoped to achieve this isolation but the contrary is the case:
the pad is completely connected to the copper zone, just like if I were selecting “Solid” instead.
Put the pad on a different Net . . . then connect the Nets with a Nettie if you need to . . .
Out of interest, how is the pad going to be connected to the Net if not by way of the zone ?
Thanks for your suggestion RaptorUK. Does it mean, that the “None” option described above has bug ?
Regarding your question: I want to connect the pad in question via a filter capacitor to the mentioned copper zone and not directly.
In my eyes that is 100% a different net . . . one net connects the pad to the Capacitor. Then the other pin on the capacitor is on the same net as the zone.
I don’t think there is a bug, none might be used for a pad that is not expected to be connected, for example a pad around a hole for a fastener. I think it’s purpose is to stop DRC complaining . . .
1 Like
Yes, that should work. But you have to depress the b key afterwards to re-calculate internal zone geometry. On a sidetrack, you may want to look into “netties” and how they work.
If you put the filter capacitor into the schematic, this should be solved automatically and the pad becomes its own net, like RaptorUK said.
Thanks a lot for the hints guys.
@paulvdh: Yes I know that I have to recalculate the zones by pressing b, but when selecting “None”, it behaves like selecting “Solid”, i.e. the pad is fully immersed into the zone (without thermal reliefs). I guess this is a bug. Some other CAD systems also provide the possibility to isolate a pad from the surrounding zones, although they belong to the same net. This makes sense in the case of decoupling capacitors for µC or for output capacitors of SMPS (in my case).
Just as a test I set the pad properties of an SMT pad in a GND zone to none and then refilled with b. The pad is now not connected as expected.
I don’t understand why you think:
One situation this can be useful is if you want a clearance for thermal spokes, but do not have the pad fully surrounded and the automatic spokes do not work properly. In that case you can draw a track manually to create “custom thermal spokes”.
Really ? It doesn’t work in my version (KiCAD 9.0.0, latest version). Same behaviour as “Solid”.
Just tested with kicad v9, the feature (set “pad connection == none”) in principle works. So either you are doing something different or there is a bug for some cases.
To get forward:
- please read the following FAQ article to promote yourself to the next forum user level
- as a promoted “basic user” you are allowed to attach the project (or at least a example showing the not-working “none” setting)
- then we can examine the project and either find a false setting or confirm the bug
sidenote: please write the version information already in the first opening post. This is necessary for the readers to reproduce your issue. And writing it right on the start saves time and askcall back questions for all parties.
OK, found the problem: The “Clearance” of the copper zone was set to 0.
Consequently, “Pad Connection” settings of “None” and “Solid” gave the same result
Thank your for your effort.
2 Likes
What does DRC say about this implementation ?
In my design rules a clearance is specified but DRC doesn’t complain because the pad I wanted to isolate is in the same net as the surrounding copper zone. No clearance required.
It doesn’t complain about the filter capacitor having both pins connected to the same net ?
The pin I wanted to isolate is an inductor pin which itself is connected to a capacitor pin.
Th other capacitor pin is connected to GND.
1 Like
But you say that also this pin you want to isolate has the same net.
If both capacitor pins have the same net == capacitor is shorted at schematic. It is something unusual.
This all sounds very sketchy. Why not just simply draw a schematic that matches the actual circuit? This will probably give you some trouble with the Power pin not driven DRC error, but that can be fixed by using a PWR_FLAG symbol.
Yes, I know it’s difficult to explain my intention without knowing/seeing the
details. But the main (pin isolation) problem is solved. No DRC errors.
Using PWR_FLAG right from the beginning to remove DRC complaints.
Everything’s now as desired.
Thanks for helping me. The discussion indirectly lead me to the solution. 
2 Likes