I’ve not had any difficulty creating thermal reliefs in the past, however, I came across something that has stumped me. Below is a picture that shows a number of pads connected to ground, with traces.
and the plan is to have copper fill top and bottom, with top-side copper connected to ground. However, when I fill, pad 5 of J1 does not make a connection to ground (it stops short)
whereas the thermal reliefs associated with the other pads connected to ground seem fine.
I took a look at the “pad properties” for pad 5 and they seem fine (that is, the same as the pad properties that have worked just fine in the past on a different design, with a slot in the pad, as in this case)
.
It’s not critical for this particular design, in part because I already have a ground connection to pin 5 (exclusive of the pour), yet it irks me that I can’t fix and/or explain the behavior.
You have a cutout on the edge cuts layer. Kicad does see the edge cut drawings as a separate thing to which it applies the normal clearance. If you want elongated holes you either need to use the default kicad way (assign a oval “drill” instead of a round one) or make your drawings on some separate layer (example eco1) and merge that layer later with the edge cuts layer. (Which of the workflows works depends on your manufacturer. Or more precisely on their tools.)
Thank you, “Rene_Poschl” … sure enough, when I decreased the size of the slot (so as not to infringe on the required clearance that you mentioned) the thermal relief showed-up as expected, per below;
I cannot decrease the size of the slot (in reality) and I’m stuck with the pad geometry I have because I’m constrained by the size of the PCB, so I’m wondering if there’s a way to modify the minimum clearance? (so that the thermal relief shows-up … based on my original pad/slot geometry).
I use OshPark to make my boards and I’ve not experienced any issues producing the desired effect (i.e. plated-through slot) using the method indicated in the attached pics (above), just FYI.
Until OHS fix there interpriter for slots its likely going to be easiest to just draw in the thermal reliefs on the layers you want. I doubt you have many plated slots.
Equally unless I am mistaken your zone appears to not be set to GND for the net. Looking at how it has thermally joined to the unnamed net of a resistor
This issue is discussed, and there is a link to another thread about a script that can be used to combine the gerbers for the layer that you put the cutout with the edge.cuts before sending the gerbers out. (You wouldn’t be able to simply send OSHPark your .kicad_pcb file, but then they don’t offer support for v5 files yet…)
Oshpark now seems to support standard kicad oval drills: https://twitter.com/laen/status/1018516545549619207
So you do no longer need to use the workaround of drawing on the edge cuts layer. Simply assign an oval drill to the pad.
