Can I not write to GitHub, is that the issue?
I’ve followed some forum instructions and can’t seem to find anything on this issue.
Do you have an actual reason to use this KIGITHUB library? It’s recommended to install with an installer or dowload and make the library a local one. I suspect that if you have to ask here, you don’t know how this KIGITHUB works and why. KIGITHUB is a legacy from old times. They once thought downloading the library automatically from github is a good idea, but later came to other conclusion and KIGITHUB isn’t used anymore (in 5.0) by default.
So the solution here is?
I don’t care how or why the lib works I just want it to work.
It’s nice that KiCad is free and all but it’d be nice if major sections of the program operated better.
Do not modify system libraries. Make your own personal libs as you will loose your changes on update otherwise.
Here some info on how to do this: Creating a new footprint library
In addition: The kicad team does no longer suggest the use of the github plugin. For this reason kicad 5 no longer uses it for its library. If you run v5 then please read this: I had KiCad 4 installed previosly. Now i updated to v5. Now i have some problems with the library setup
For info about installing footprint libs take a look at this: How can i install a specific version of the footprint library?
A more detailed answer to a similar question can be foun here: High level thinking
I can only emphasize what Rene (and others) say.
All “professional” layouters use the included libraries as templates and create their own standard libraries from that. In “my” company it is simply not allowed to use any footprint that is NOT company specific.
Even for my crude home PCBs I modify the carefully designed KiCad footprints into a more generous style 
The advantage is that the KiCad libraries can expand and evolve freely without influencing existing designs…
Seems that I stumbled my way through the process and have an understanding now how the system works.
However I still think it’s a bit tedious and there are things that I can’t seem to accomplish.
One such example is having multiple pads for the same signal on a part.
In other words I don’t see all the pads on the same net in the layout.
I did figure out how to create my own library and I did so per project, it’d be nice if you could import the global library that is created into a project.
Just an observation.
Takk Takk!
Highlight net. Second icon ont the right toolbar.
Something similar to what you want: File->Archive Footprints->Create a new library and archive footprints
Thank you I’ll take a look.
Here is the issue with the pads.
I currently have to go in and change each to the net that their associated with.
All of these pads belong to the same part on the same signal line.
With the image, I hope that it’s easier to see what I mean when I say I’m wondering where or how you can associate all the pads in the footprint layout.
Tussen Takk.
What, specifically are you trying to accomplish here? Am I correct that you want to use via stitching to connect a bottom pad of an IC to copper on both sides of the board for thermal and/or current capacity reasons? Do you have a datasheet that we might look at so we can help understand what you want/need?
A general comment. You can have multiple pads in KiCad footprints that all have the same pin number. If they are overlapping enough then they will be considered connected to each other. So if (as I suspect you are trying to do, but I could be wrong) you want to connect a SMT pad under an IC to both sides of the board, you can have in the footprint a collection of pads all the same pin number. A large SMT pad covering the entire area, then several small drill (via sized) THT pads (pad shape doesn’t matter) within that larger SMT pad. I’d be careful soldering that sort of arrangement (unless you can communicate with your board house that those holes are to be filled vias) as all the vias would absorb solder paste like a sponge.
Aren’t you using a schematic?
There is no need to set the net name of a pad in the footprint editor. The pads in the layout take the net name from the schematic/netlist.
Here is the part: https://katalog.we-online.de/em/datasheet/7461099.pdf
The issue here is that all of those pads belong to the same net and are not being placed as such.
Interesting part.
Yeah, make all of the pins pin number 1. Put two SMT pads (copper only, no solder mask or solder paste), one on the top and one on the bottom, both also as pin 1 to connect them all so you don’t have to run traces between all the pins. On the schematic just use a single pin symbol as pin 1, and connect that pin to your desired net.
Try this footprint (you may want to rename it…): dummy.kicad_mod (2.8 KB)
Note, I haven’t tested this on a PCB yet.
In FP editor:
In 3D viewer Top:
in 3D viewer Bottom:
Oh, I just realized that my sample footprint name might be taken as insulting. That wasn’t the intention. I used the word “dummy” with the following meaning: a prototype or mock-up, not as a reflection of anyone’s character, save my own.
1 Like
I knew what you meant by dummy, no worries. Thanks for the part. I’ll open it and see how you did that.
Very interesting artifacts. Almost looks like Navajo Art.
I’m wondering if it is the thermal relief algorithms interfering with each other from the through holes. Might want to try by changing the connection to copper zones in the “local Clearance and Settings” tab of the pad properties in the footprint editor. I’m thinking changing the setting from the default “From parent footprint” to either “Solid” or “None”. Because of the number of pads and the fact that at each point there are 3 pads overlapping, it might be faster to select and change one of the THT holes and save. Then open the footprint file in a text editor and copy the attribute setting from the one THT pad to all the other THT pads using clipboard cut and paste. Then reload the footprint into the board file.
Ah yes, that did indeed fix it. Navajo indeed.
Now just to physically test the press fit.
Great. Glad to help. Just out of curiosity, what fill setting did you use, and would you provide a screen shot of it in use? Thanx.
You may want to make several footprints all with slightly different drill hole sizes. Have a very small board made with one each of the sized footprints and use that to test fit to make sure you specify the right drill diameter for your full project (and any future projects that use this part).
1 Like
This assumes that the drill has the same tolerance in your next order.
It might make sense to contact the manufacturer about that and talk to them regarding tolerances. (you might need to specify tighter tolerances for these holes depending on the part that will be pressed into the pcb.)