I was wondering, whether someone could enlighten me a bit. In short, I have a custom pad in my footprint, and it won’t connect to the net. Here is an example: pin 1 is indicated to be part of the GND net, and on the first footprint, it is not connected to the copper pour. The second footprint was created the same way, with the sole exception that I don’t have a custom segment on pin 1. There the connection to the copper pour is OK. If I swap the two pins, i.e., I assign GND to pin 2, then pin 2 will be connected to GND, therefore, I assume that the general settings of the footprint are correct.
Could someone comment on this issue, or point out what I am doing wrong?
Version: 5.0.0-fee4fd1~66~ubuntu18.04.1, release build
libcurl/7.58.0 OpenSSL/1.1.0g zlib/1.2.11 libidn2/2.0.4 libpsl/0.19.1 (+libidn2/2.0.4) nghttp2/1.30.0 librtmp/2.3
Platform: Linux 4.15.0-33-generic x86_64, 64 bit, Little endian, wxGTK
wxWidgets: 3.0.4 (wchar_t,wx containers,compatible with 2.8) GTK+ 2.24
OpenCASCADE Community Edition: 6.9.1
Compiler: GCC 7.3.0 with C++ ABI 1011
What are the zone connect settings of the pad that does not connect?
Could you upload the footprint?
Rene, is this what you meant?
Sure, see attachment.
test1.kicad_mod (397 Bytes)
test2.kicad_mod (544 Bytes)
I think I didn’t read your question carefully enough. Here is the correct answer:
Now, if I set the pad connection to solid, then the connection will be established. However, there are only two options, solid or none (none was set by default). Is there a way to connect the pad with thermal reliefs?
The pad is probably a custom shape, they have only those two options. Change it to a normal rectangle or round shape.
EDIT: I didn’t look carefully enough - it certainly is a custom shape.
The pad that I need is much more complicated. I shaved it off, because I wanted to present the problem in the simplest case. So, no, rectangle or other standard shapes are not an option.
I think the underlying problem is that it’s difficult to create an algorithm which would create thermal reliefs for any arbitrary shape so that they would satisfy all users and needs. It’s simple and easy for round or rectangle pads.
This is a good point. Thanks for the comments!
The footprint is alright, as you probably knew.
The solution seems to be making the spokes by hand with traces from the pad to the zone.
And paly with the pad clearance.
This is an interesting solution. The snag is, I opted for custom pads, because the shape I need is not trivial, and if I assemble the shape out of standard components, then I will have to connect the parts by wire, even if they all share the same pin number. (I think this is a known problem/feature in kicad.) I wanted to save this extra step, but with the present situation, we are back to square one. Well, what the heck, could be worse!
Another solution might be to put small additional round or square pads in the footprint on top of your custom shape where you want the spokes to attach with the same pin number as your custom pin. Then hopefully the copper pour will automatically run spoke thermals to your desired positions.
I haven’t tried so this might not work, just brainstorming here.
I remember seeing a similar effect on a square mounting pad that I designed that had THT pads arranged along the edge of the large mounting hole pad. I had the smaller ones coincident with the edge of the big one and all of the individual pads got thermal spokes to the ground fill. Until, of course, I realized that I could make them all solid connections to the copper pour as part of the pad properties…
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.