Hello!
I have the following problem with USB-C connector. I would like to connect the VBUS pins to the proper plane. You can notice that pin B4 is properly connected, but B9 is not. However, the plane comes extremely close to B9, and judging by the width of B4’s thermal connection, the remaining space is more than enough to also connect B9.
Just in case, I have widen the are using the D command to move the traces. But although this time there is at least 5 times the space needed to pull a trace to B9, it’s still not connected. The thermals seem to be set at 45 degrees, so that might be a part of the problem.
This 3rd image shows that If I leave some space beyond 45 degrees, then it gets connected. Is there a way to force attachment, move the thermal attachments, or that sort of trick? I solved it by adding a wire to B4, but there is probably a better solution.
One thing that I see is your zone clearance is larger than your net clearances. (That’s why there is a gap between the edge of the zones and the clearances around the pads.) If you lower your zone clearance down to your net clearance, does that help the spokes get formed? Note that the quadrant 3 spoke isn’t being formed to the top VBUS pin (B4). Also try thinning the spokes. There might be a clearance violation preventing the formation of the spoke. Either the zone clearance, spoke width, or combination of both.
Hello!
Oops, yes indeed I forgot the 3rd image. Anyway, by lowering the trace labeled “NRX”, it gives room for one spoke to be drawn.
Ok, I will try with thinner spokes. They are 0.2mm right now, but anyway for a length that small, I suppose it’s not a problem to make it thinner, even if USB-C is supposed to allow a few amps current.
Around the Zone clearance, there also has to be a minimum copper width before KiCad draws the thermal spokes. In your case this minimum width is not met and therefore the spokes can not be drawn. Your “NRX” track is just too close.
Your options are:
Set the Zone connections of some individual pads to “Solid”.
Draw some copper tracks, for example from B4 to B9. This will push the NRX track away enough to make room. It also prevents B9 to become disconnected if NRX is later shoved for some other reason.
If you want to just draw a pad connection from a pad to a zone (so the track has an open end), then you should also lock these track segments in place, or else they will get deleted by the utility: Pcbnew / Tools / Cleanup Tracks & Vias (This was moved from: Pcbnew / Edit / Cleanup Tracks & Vias in KiCad V5.1.x)
