Hello friends,
I would like to contact the forum and ask for help to create a footprint for a LORLIN CK-1059 rotary switch. The rotary switch has one level with 12 positions and end stop.
Unfortunately there is no footprint for this rotary switch or similar.
Does anyone know or have this footprint for KiCad in their library?
The switch symbol for schematics is available in the library. I have tried to create the footprint myself, but it becomes too imprecise simply by measuring and setting pads. I just canāt manage to create 12 even positions of the pads of 15Ā° degrees on a circle and also to create the 4 positions (one is only needed, but the rotary switch is available in 4 levels) of the pads on the inner circle.
Honestly, I donāt know how! It must be very precise according to the data sheet.
I will be happy to provide further information on the rotary switch (data sheet)!
Please help or information!
Thanks a lot!
VoJo
Thereās a footprint wizard for creating various kinds of arrays. A circular array of pads is one of the choices. You may have to combine two circular arrays.
PS: 360Ā° Ć· 12 = 30Ā°
I have just tried (KiCad V 8.0.9):
- in footprint editor I have placed a pad at position X=10mm, Y=0,
- in Prefernces-Footprint Editor-Editing Options I have set āStep for rotateā¦ā to 15Ā°.
- right-click at pad and āPositioning Toolsā and 'Copy with reference, reference I set at 0,0
- now Ctrl+V and keeping cursor at 0,0 R rotates pad 15Ā° around 0,0.
KiCad gives you many tools to do things. There are two above. Another one is the array tool:
- Place one pad at a point on the radius (e.g. 11.10, 0)
- Use the array tool (Ctrl+T, or via menu) to make a circular array of 12 pads, as a full circle (=30 degrees), around the origin.
- Use the Move Exact tool (Shift+M, or via menu) to rotate by the 15 degrees
but it becomes too imprecise simply by measuring and setting pads
You can enter the pad positions to the nearest nanometre - even with just a calculator and patience you can compute the sine/cosines as you need to full accuracy (Iām sure someone will tell you they did it with a abacus or a book of trig tables āback in the dayā, and even 0.01mm is already way more accuracy than you actually need). In fact, even then, you only need to compute these three positions and the rest are co-ordinate swaps and mirrors:
Actually I used to do it with a 5 function pocket calculator, using the methods in this book, which I still have:
But I never had a practical use for those methods, it was just a obsession for a nerdy kid for a while. The educational system was geared to traditional methods such as trig tables. And soon scientific calculators became cheap enough.
Sorry for waxing nostalgic.
The footprint editor has a toggle for polar/cartesian coodinates, which should make placing the pads easy
Hello friends,
Thank you all very much for your help. First of all, of course I made a mistake in my calculation: 12 x 30Ā° = 360Ā° and not the 15Ā° steps I specified. In the component diagram from the manufacturer LORLIN, the 1st solder pin is 15Ā° clockwise from the center and the following solder pins are 30Ā°. That was my mistake and thank you for the correction.
However, I still selected 15Ā° in the settings and so I was able to set the soldering point very precisely in 2 x 15Ā° steps at the end of the auxiliary line with exact auxiliary lines and also correct it to the exact dimension in the properties. Now everything is really very precise.
It would be desirable for the future to make it easier to divide a circle into segments in KiCad, as in a drawing program, and then simply add multiple segments. That would save several hours of work.
I have searched the entire library for footprints to find a component that is arranged in a circle with a large number of solder pins. Nothing was found!
When Iām done, Iāll post the rotary switch here for you to use. My design also directly includes the solder pins for 1pin x 12 positions, 2pin x 6 positions, 4pin x 3 positions. On the 3pin x 4 position rotary switch, the center pins are twisted and donāt fit into the general layout of the component. This would have to be redesigned.
Many thanks to all the helpers here in the forum.
Regards
VoJo
hello davidsrsb,
where should this be in KiCad 9.0?
Thanks for your help!
VoJo
Youāre still lucky 
Every now and then we get someone whoās searched the entire internet and found a symbol/footprint. Then they come to the forum asking what to do with the tons of errors KiCad is reporting.
Here it is:
hello Johnbeard,
Iām too stupid, I canāt find this menu item in KiCad 9.0. Where exactly is that supposed to be where you are in your video? With Ctrl T takes me to the array menu, but not via the menu items you showed. Can you please tell me again where to select the menu item.
Thank you very much!
VoJo
hello Peter,
thanks for the hint ā¦ it should read: no component.
Thank you very much!
VoJo
Itās in the Create from Selection menu in the context (right click) menu.
Maybe start a blank project and just play about with all the tools to see what they do. And read the manual: PCB Editor | 9.0 | English | Documentation | KiCad. Once you are familiar with the tools, itāll only take a few minutes:
Hello @VoJo
Take this advice:
It is absolutely the best thing for you to do. You will always need new symbols and footprints Making your own is far easier and quicker, after some practice, than scouring the internet to find something that probably needs alterations.
Anyhow, here is a blow by blow description to making your footprint just to show you how easy it is when you have learned to use the tools available.
File > New Footprint > Save. Give the footprint a name and highlight a Personal Library in which you want it placed. > OK.
Set your grid to mmās on RHS.
Set your grid to .1mm at top.
Place a pad exactly 11.1 mm above the footprint anchor. see dx & dy.
Right Mouse Click the pad and open its Properties.
Change to THT, set the shape, size and hole size. ( I used round, 4mm Dia. & 2mm hole ). > OK.
RMC the pad again > Create from Selection > Create Array > Circular Array.
Leave Centre positions at 0, tick Full circle and Rotate items, item count = 12, pad numbering = 1, increment = 1, > OK.
You will get this:
Leave your footprint highlighted.
Go to Preferences > Preferences > Footprint Editor > Editing Options > Step for rotate commands, and alter the degrees to 30 > OK.
Whilst your footprint is still highlighted, RMC and Mirror Horizontally then RMC again and Rotate Counterclockwise. Remove highlight.
You should now have something looking like this below:
Change Grid to 0.05mm.
Place a new pad 3.35 mm above the footprint origin.
Iām not sure how many pins you have in the middle. If there is only one, you have now finished placing pads.If there are four, make another array by:
RMC pad 13 > Create from Selection > Create Array > Circular Array, but this time leave everything as before EXCEPT item count now = 4 and numbering start = 13. > OK then mirror horizontally this new internal array. You should end up with:
Finally add your F.Silkscreen, F.Fab & F.Courtyard circles and the job is complete.
As @johnbeard wrote, and I quoted: practice and experiment with the tools and READ the documentation; itās the best way to learn; and YES, it only takes a few minutes for a footprint like this.
More time is wasted not starting at the beginning than avoiding the inevitable. I think Iāve said this before. My son has an IQ of, well frankly, I donāt even really know. When heād get a new game he wouldnāt even start it till he read the manual. Some of them pretty lengthy.
The symbol and footprint editors are perfect examples of things people spend more time looking for something pre-made than had they read the manual and started from scratch. (Not that I personally EVER did such a thing. 
)