1
\$\begingroup\$

I download symbols and footprints from the component supplier into a project's library to go faster but I realized that many of the standard components footprints are slightly different in KiCad, like for example the SOT-23-6 so my question is: is it better to stick to KiCad footprints or just use the suppliers footprints?

\$\endgroup\$
1
  • 1
    \$\begingroup\$ This is unanswerable. The only realistic path is to compare them in detail and apply pragmatic knowledge of process. If you are assembling or reworking by hand under a microscope you can probably survive things which would produce unacceptably low yield in an automated process. \$\endgroup\$ – Chris Stratton Jun 5 '20 at 3:28
3
\$\begingroup\$

There is more to good footprints than just "matching the pads to the pin". Depending on the dimensions and distances the results of soldering can strongly vary. Good footprints can reduce the risk of shorts and grave stones for example.

From my personal experience, I strongly advise using the IPC-7351 footprint recommendation because the standard library coming with KiCAD did not really live up to the expectations (at least back then I started) and even the footprints described in datasheets sometimes resulted in less optimal (reflow) soldering for me.

There was a rather prominent repository of a KiCAD library derived from the IPC-7351 recommendations but I cannot find it anymore. However, it seems like there is still a version around https://github.com/alexisvl/kicad-pcblib . I typically use the "Least" but only because I do a lot of tiny crowded PCB with reflow soldering. The "Most" version should be adequate for everyone with decent knowledge about hand soldering.

\$\endgroup\$
2
  • 2
    \$\begingroup\$ The current library uses IPC-7351B rule set (with some influences from the future C variant) to derive footprints for standard packages (like your run of the mill resistor, SOIC like, DFN/QFN like, ...) All of them are script generated with scripts found in github.com/pointhi/kicad-footprint-generator/tree/master/… and github.com/pointhi/kicad-footprint-generator/tree/master/… \$\endgroup\$ – Rene Pöschl Jun 5 '20 at 15:32
  • 2
    \$\begingroup\$ Of course the official library has a few limitations. We can for example not make a specific footprint for every possible 0603 resistor out there so we use a reasonable example to get the part dimensions and tolerance ranges (for the most common ones we use the predecessor to IPC-7351 as the dimension source which was also checked against a random selection of parts available at farnell) And we need to make assumptions fo rthe manufacturing tolerances (here we use the example value given in IPC-7351B) \$\endgroup\$ – Rene Pöschl Jun 5 '20 at 15:34
1
\$\begingroup\$

Best approach would be to ask people who will solder these components. For one component, KiCAD footprint may be better, for another - the supplier one. We ended up making our own library of components based on existing one.

\$\endgroup\$
0
\$\begingroup\$

How different? But usually the supplier knows the part (while KiCad has some generic footprint). You should also check the datasheet to see which one better fits the mechanical drawing (and remember to enlarger them a bit if you plan to hand-solder them).

\$\endgroup\$
3
  • 2
    \$\begingroup\$ Do not trust any footprint that you have not verified yourself. Even the ones available for download from a manufacturer. It is your responsibility to make sure it is right. \$\endgroup\$ – Chris Knudsen Jun 4 '20 at 19:47
  • \$\begingroup\$ Well, why not start by comparing the supplier footprint and the mechanical drawing? Have you had bad experiences following the mechanical drawings on datasheets? Also, after that there will probably be a prototype PCB and in that step we will catch all the problems in pad sizes. \$\endgroup\$ – jDAQ Jun 4 '20 at 19:56
  • \$\begingroup\$ Still, if the OP already has the components he could just print (with a printer and so) the many footprints he'd like to test and see how the components fit those pads. But I assumed he does not have the components with him. \$\endgroup\$ – jDAQ Jun 4 '20 at 19:58

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.