Head of library here.
This might not be a good idea to be honest. There is a very low chance that you got it right at the first go. Whoever does this part for you will not know enough about the parts to properly fix them for themselves or answer our questions. (Meaning it will waste both the time of maintainers and the guy who is prepared to do this part of the work for you.)
There is not much to making footprints and symbols aside from Fab layer. Using a parametric cad to draw the footprints to nominal dimensions from datasheets then printing it out on paper to check the part fits.
Learning git well enough to make contributions to the library really should not be that much of a problem. I understand that it seems daunting at first. There are a lot of tutorials out there. Github gives well written beginners guides and if you want to go into more details then https://www.atlassian.com/git/tutorials is your friend.
Print out to paper really is not precise enough to find the sort of errors we check for. (Your footprint must agree to all significant digits given in the datasheet.)
The fact that you use CAD increases the chance of the footprint being made correctly. Assuming you convert it with a good tool to kicad (kicad stepup might be the best option here.)
A previous post of mine gives a lot more detail to what we expect: Adding footprints for everyone to use instead of just for me
How about the symbols? Those can vary and there are lots of symbols kicad doesen’t have.
I agree that adding well made assets is the way kicads library will grow. But be aware that our high standards will require you to put in more effort as compared to making assets for your own use. (After all we want any asset in the library to be as useful to others as they possibly can be.)
This process simply requires communication between the maintenance team and the contributor. Having somebody in the middle will make the task a lot harder for everyone involved. (It is not impossible and there are no rules against it. If you find somebody willing then it is ok. I just want to make it clear to everyone involved what is expected.)
You could just put the files in some location where anyone can download them. People could give some comments and we all would see if they are up to the standards. Then, if they are really high quality, someone could volunteer to help with git as you proposed.
Edit: at first you could put some screenshots here.
Maybe as a sidenote: I am not prepared to review anything on any other platform than the correct github repos. Meaning not getting a response from me here does not mean your asset fulfills our requirements.
Two reasons for this. First: the forum simply does not provide the tools i would need. There is no easy way to see what exactly changed between reviews. Second: I feel all maintainers must have equal say. Not all of them are active here resulting in some of them being excluded if we make decisions here.
Edit nearly forgot: Github is setup with our testscripts that take care of a huge junk of review work. Not having them is a no go to be honest. (Do you really prefer learning how to run test scripts on your own over learning git?)
More details about the review process: the scripts check for KLC compliance, we maintainers check if your asset complies with the datasheet and industry standards. (And do some additional KLC checks for things that the script simply can not check.)
Even though I commend your work and giving the links, I must say that you should do some more work when you share it. Dpaste.com doesn’t let me download the file with the original .kicad_mod name. (The naming convention is important in KLC.) I have no idea what onshape is and what to do with it. You should share the 3D files in their source form and/or in their final .wrl and .step forms which are used in KiCad. @Rene_Poschl can tell more about what is accepted as 3D contributions.
The best option could be to share a zip file with the footprint file and symbol library files and the 3D original source, .step and .wrl files.
Also you should give direct links to the datasheets and other relevant information against which these can be checked. Never assume people can “easily” search for the information.
And it’s still unclear what you have already done to assure KLC compliance.
The point is that you should do yourself as much work as possible to make other people’s work easier. Nobody is willing to do complicated or even simple work which you could do yourself even though they would be willing to help with validating or with git or something like that.
BTW, this is not a promise that I would necessarily help. I just mean that you enhance your chances of getting helped if you do as much groundwork as possible. Your work is appreciated anyways, but because we all are volunteers who get no compenstation, we don’t want to do unnecessary non-creative things like manually changing names of files or doing file format conversions which could have been done “upstream”.
Also remember what Rene said:
But it actually might be a good idea if you find someone who is willing to invest some time to get familiar with the parts and with KLC. Then there would be better chances of getting it right the first time before giving it to the actual library maintainers. But the man in the middle should take some responsibility of the quality instead of only using git for you.
Here is a zip file with much of what I have I made the symbols and some of the 3D parts. I have made boards using most of the footprints I made since they aren’t in the kicad library.
OK. The zip file is good, but I would prefer having one .pretty library folder and one 3D folder and one symbol library file, so that they all could be included in KiCad by adding them to library tables without copying or moving files.
I checked the 2-pin terminal block footprint and 3d model. The footprint doesn’t meet the KLC requirements. Please read them carefully. For example, there’s no fab outline in the footprint. The font size is wrong. **REF is wrong. There may be other problems. You really have to learn the conventions and edit accordingly, otherwise the contributions won’t be accepted.
I don’t know the details about what’s required for the 3d models but at least your models don’t have colors which the users would expect from the standard library.
FYI, OnShape is an online mechanical CAD package. It is fairly popular in the Maker community because is both free (the “educational version”) and only requires a modern web browser. Some maker oriented organizations (for example library or school based) don’t necessarily have installation rights for their computers, and it is harder to convince a new person just learning 3D CAD in a maker class to install unknown software.
Comparing it to FreeCAD (what I’m learning and personally use), it is easier to learn and use for someone new to 3D design. But because someone, somewhere, has to pay for the server that runs OnShape’s back-end, there isn’t any guarantee that it will stay free or will stay available. OnShape is “Free like beer”, where FreeCAD is “Free like speech”. No one knows if OnShape will eventually do what AutoDesk did to 123D Design.
One more note about the 2-pin terminal block footprint. According to the relevant section of KLC (https://kicad.org/libraries/klc/F7.7/) those THT holes should be round, not oval. And even for non-KLC compliant footprint it’s weird that the holes are currently too small for the pins. You said
But this kind of error doesn’t arouse much confidence.
The pins arent too small the 3d model is a slightly larger. I already made boards using those terminal blocks.
I checked against the datasheet.
Checked datasheet the barrier terminal block is fine. The ohmite heatsink 3D model is right from the manufacturer support site. There are no errors in any in my footprints as I checked them over. The 3D models are missing from kicads library they are in the zip file if the devs want them. The pads dont need to be round, wider pads are more optimal I use nearly none of kicads footprints, I modify them since they are cumbersome to work with.
Here is an extra block, with dimensions taken from the datasheet https://datasheet.lcsc.com/szlcsc/Ningbo-Kangnex-Elec-WJ45C-B-2P_C8397.pdf, on top of your footprint pad. Dimension are nominal + tolerance which becomes 1.55x0.85 mm. It can easily be seen that the pin doesn’t fit into the hole. The same can be seen in the footprint/3D model combination. It may fit in real life but it’s not guaranteed. The board manufacturer has tolerances, too. The pin may be reaching the smaller limit inside the tolerance given in the datasheet. Take another board manufacturer and another part batch and it’s possible it doesn’t fit.
KLC requires that there’s 0.1mm empty space around the largest possble pin, but so that the rounded ends of the hole don’t count. Instead of 1.8x1.0 mm the hole should be 2.6x1.05. Like this:
You may have different personal preferences. I do, too. But if you want to contribute to the official KiCad library you have to obey the rules. The rules are strict and probably nobody would use those rules for their personal (or company) library. But there must be rules which make sure that the symbols/footprints/models are consistent and work as expected under all circumstances.
I think most people find out that they should design their footprints from scratch to make them KLC compatible. And most come to the conclusion it’s not worth it, so they give up. Which is fine because the bottleneck at the moment is doing the manual checking of contributions, not too small amount of contributions. And that’s one good reason to learn and obey KLC before trying to contribute.
Detailed description on how to decide on THT hole size (part of my larger how to make a footprint tutorial): Tutorial: How to make a footprint in KiCad 5.1.x?
But also the library convention https://kicad.org/libraries/klc/F7.7/
Here are 4 TO-247 3D models which kicad is missing. https://ufile.io/tvdlwp2d
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.