The manufacturer of this pot below gives the pcb layout and shows a square mounting hole. In this situation what is the best fit that I can get with an oval or round mounting hole or how do people generally treat these types of mounting tabs in Kicad. I don’t get why the manufacturer doesn’t just show the layout using an oval or something that is more manufactureable than a square hole. Link to an image of the footprint below. Thanks!
Potentiometer Footprint
Usually they give an ideal or “minimum recommended” land pattern. It depends on the manufacturing process how near the ideal it can actually be, but it wouldn’t make sense to give a non-ideal, either, because there’s no one mimimum non-ideal pattern. Just stop wondering and make an oval or round hole, whichever fits better your needs / manufacturer’s capabilities.
Very high volume consumer single sided PCBs are/were punched in paper based PCBs rather than drilled and routed, so square and rectangular holes are possible
I have used a round hole in similar situations and placed the hole so that the circumference intersects the corners of the square hole so that the clips snaps in place properly. That seemed to work fine.
1 Like
You might be interested in Tutorial: How to make a footprint in KiCad 5.1.x (From scratch)? (section Through hole parts)
To make this post complete, I copied the picture here:
The metal that goes in the square holes clearly has hooks that are designed to snap the potentiometer onto the PCB. The 14.3 mm measurement in the right side picture is the controlling measurement for the (hopefully) correct snap action.
Anything but round holes are difficult to for this size in FR4. The pin has to fit though the hole and the diagonal of the hole is 2*sqrt(2) = 2.828427 Maybe you can go down to 2.6mm because not all of the area is occupied by the pin at the same time, but 2.9mm diameter would be safer. For THT pins they would be easy to hand solder or automated with wave soldering.
With round holes the “clamps” also do not sit flush with the inside of the hole, and you could make the 14.3mm measurement a bit smaller, I’m guessing around 13.9mm
Another factor to think about is the ease of insertion. For this the center of the holes should have a distance near to the 16.1mm with of those pins (theoretically minus the sheet thickness) but it’s not a very critical measurement.
For the “Z” direction, just center the round holes with the same 3.3mm as the square holes. It does not matter much that the round holes are bigger then the square holes. The clamping force of those mechanical pins will center the potentiometer on the slanted edges of the round holes.
Also beware of the 2 encircled “alignment feet” on the left side. These should either all be on the FR4 directly, or on copper, so all are at the same height. If you place them on copper, then do not rely on the solder mask, so no other tracks at these areas, but I would use SMT pads in the footprint itself. For even more mechanical strength, you can also solder these tabs to the PCB. In that case, but some small via’s through the PCB at these locations to make a stronger mechanical connection between the copper and the FR4.
For a small order (such as hobby use) this would be sufficient (for me at least). If you are considering bigger production runs you can consider:
- Ordering a test PCB with 10 or so variants in hole spacing and diameter.
- Buying a small router to experiment with parameters that work best.
- Look at datasheets for comparable components and recommendations in those.
Make a square hole on either the ‘Edge.Cuts’ or ‘Dwgs.User’
Can put the shape on edge.cut and move it to a footprint (not intuitive).
PCB companies use Laser, CNC and some use water-jet to cut boards.
Corners are never sharp - they always have some small radius (depending on process).
Below is from JLCPCB - (their English explanation doesn’t clearly say it but, what they mean is any square/rectangle is ok but all will have a small radius’d corner).
Thanks so much for all the practical info. I was really wondering how other people handle these types of tabs in KiCad. Your feedback has been very useful.
Jim
Remember, for small holes like these routing a rounded rectangle might not be possible. The board manufacturer might not have a small enough routing bit to be of practical use here.
Referring to the Link I posted, click on the “Drill/Hole Size” and you’ll get the necessary info about sizes… Probably fairly typical…
I do a circle, because it will held in with solder anyway…
I ended up drawing square cutouts in the Dwgs.User layer and adding SMD pads on the top and bottom layer for soldering in the footprint editor. Once the footprint was in PCBnew I swapped the Dwgs.User layer for Edge.Cuts layer.
That does not solve the fundamental problem that no fab can ever make a cutout of a true rectangle. You still need to account for the size of the cutter which determines the minimum radius at the corners.
My suggestion really is to use oval holes and chose the size as follows:
hole width = final cutout width.
hole length = final cutout length + hole width
For a graphical explanation see the tutorial about footprint generation already posted above.
And yes this might result in a longer hole then absolutely necessary but it is an easy to use rule that is good enough all but some very special cases (the only time this will be a bad idea is when the leads of your component are very near to each other in the same direction where we now increase the hole size to account for the cutter).
I had a similar issue with some Phono sockets, in my case the “clips” were plastic. This was my solution:
In my case, the size of the clip is about 80 to 90% the total length of the oval hole. I’ve had several PCBs manufactured with this size hole, no issues, fits nicely.
Paul
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.