Why zone not connects to pad?

[Piotr]

I have seen some such questions before. There were logical explanations why.
This time I don’t know what is going on.

I have noticed over pad/via you see on top that there are small wave in zone suggesting that it wants to connect to thermal pad, but something tells it to keep away from that pad/via.
So I have moved pad/via in footprint (in library) that you see on bottom.
In window you see that for that via (selected one) the pad connection is set to be as in footprint.
The same setting is for all pads in footprint and footprint takes settings from zone.
At bottom you see that it has nothing to connect to thermal pad but something keeps it away from that GND via/pad.
Pad 5 shows that footprint doesn’t block connections.

Any idea what is the reason?
KiCad 5.1.10, Windows 7.

[Rene_Poschl]

it could be that the different pads have their respective thermal antipad (the exclusion zone) where the others want their spokes to be. It this is the case, then asking for solid fill would connect to the pad (you can do that just as a test). If this does also not result in a fill then something else is going on. If it results in a fill then maybe try to set the vias fill option to none and see what happens then (or solid).

[paulvdh]

Can you upload a small test project with that footprint?
I’ll have a look at it to see which setting may be the cause of it.

[Piotr]

@paulvdh

Can you upload a small test project

All test project files + footprint copied to project directory:
SON8.zip (7.0 KB)

[Piotr]

@Rene_Poschl

asking for solid fill would connect to the pad

You are right. Changing connection for those via-pads to solid make zone to connect to thermal pad as I expected.
I didn’t considered using solid for anything at top here as datasheet says that non soldermask defined pad is preferred for that element so I wanted only thermal connections to pad at top (and solid to pad at bottom).
Now I suppose that a reason of a problem is that KiCad someway decided that for those via pads it would be better to use thermal connection not in ‘+’ shape but in ‘x’ shape.

[paulvdh]

I deleted some unimportant (aperture) pads, and placed the “copper” pads next to each other to get a better idea of what is happening.

Here a screenshot in the footprint editor:

And here a screenshot from the PCB (after zone refill):

From this you can see that KiCad is trying to connect to the rectangular bottom pad, but it uses 45 degree rotated spokes for the THT pads, and these interfere with the thermal spoke to the rectangular SMT pad.

Which is the same as you already noticed:

@Piotr

is that KiCad someway decided that for those via pads it would be better to use thermal connection not in ‘+’ shape but in ‘x’ shape.

Some more about orientation of thermal spokes in:

Thermal spoke orientation

Hello there, I was curious to know how is the thermal spoke orientation determined for the zone connect and if there is a setting at the pad level (or elsewhere) to select between 45-degree angle and straight spokes. In my design I found that there is both orientation for the same zone for 2 different connectors/pads: 45 degree angle spokes [image] Straight spokes [image] I came curious as I want to control the orientation for a specific connector (from 45-degree to straight) but haven’t …

And Indeed, by clicking a pad, then editing and setting [General tab] / Orientation to 30 degrees for the bottom pad, the spokes for that pad are now rotated:

But overall it probably don’t matter much, as I assume you do not want thermal reliefs at all in that center pad.

[Piotr]

@paulvdh

But overall it probably don’t matter much, as I assume you do not want thermal reliefs at all in that center pad.

I want thermal reliefs because:

@Piotr

I didn’t considered using solid for anything at top here as datasheet says that non soldermask defined pad is preferred for that element so I wanted only thermal connections to pad at top (and solid to pad at bottom).

If I do solid connection then that pad would became soldermask defined, and they suggest to use non soldermask defined.
I normally use that IC in SO8 or VSSOP8 (without thermal pad) but as they disappeared from market and only one still possible to buy is VSON8 I am redesigning PCB to use that IC. I don’t expect lot of heating going out of that IC so that pad (+ vias) I treat as mainly to better keep IC at PCB then by 0.3x0.6mm pads.