If I get a solder paste stencil supplied with my boards, is it a good idea to have a couple of locating holes in the pcb and the stencil so they can both be aligned easily on a couple of dowel pins?
If that’s worth doing, whats the best way to do it? Draw a circle in the edge cuts layer on the PCB and then draw another circle in the mask layer?
There are Targets… bottom RHS of PCB screen.
Sorry, only half read your question.
There are Mounting Holes of many diameters in the Kicad Footprints. That is probably what you are looking for.
I have some ‘hole’ footprints that are 2.6mm diameter which include the paste layer. You can slip a 2.5mm metal dowel through both stencil and board (the extra 0.1mm helps for clearance and removal). The dowels are easily available, made in stainless steel and have a slightly beveled end. For single boards, you can place a couple together as a stack with the stencil.
For multiple boards, I have an A4 size x 10mm thick sheet of Derlin plastic which I machined a grid of 2.5mm holes at 10mm centres. If you place your alignment holes on the board at a multiple of 10mm, you can pin the stencil and board in alignment.
It makes it easier if the stencil is only a little larger than the boards.
Nice setup. Thats exactly what I want to do.
Are the holes just holes or through plated with copper etc? Do the PCB fab places prefer one over the other?
NPTH. One manufacturer unhelpfully removed them on a board as they assumed paste over a hole was a mistake. Now I always include a note to explain them.
I added a footprint of a circular pad with a 3mm hole and a 3mm diameter solder paste circle.
Does the solder paste circle need to be filled in? The solder paste area is not showing up on the PCB layout
When I plot the drill map to an SVG file, the holes I want are shown as crosses (stars) with no circle. Is there something else I have to add to the footprint drawing to get a circle to show up in the drill map polt?
This is a recent project that JLCPCB produced for me. The alignment holes are 2.6mm diameter for 2.5mm dowels - allowing a bit of tolerance is helpful.
Alignment_Hole_2.6mm.kicad_mod (891 Bytes)
My solder paste is showing up as an unfilled circle?
Also the holes are showing as just star shapes in the drill map, no circle around them?
Perhaps you could post a screenshot of the pad properties you have set - you need to have a NPTH and you need to tick the front and back paste layers as well as all copper layers. (See my screenshot above - this is from 5.99 but 5.1 is very similar).
You need to check the Gerber output - make sure there is a drill hole and also a hole in the stencil (i.e. there is an aperture in the ‘Paste’ layer).
I always include a production note with these as my ‘error’ has been ‘corrected’ for me by ‘helpful’ board houses before now 
I would also ensure the holes are slightly larger than your planned dowel size - if you are using 3mm dowels, a 3.1mm hole will allow a little clearance but still closely constrain the stencil. You will find a 3mm hole will be very difficult to get the stencil off the dowel.
OK, I changed the hole diameter to 3.1mm to get some clearance, good idea!
I still didn’t see any solder paste showing, but then when I was flipping the layers and objects on and off, a red filled circle appeared which wasn’t there before. So it seems to have worked, but not immediately.
Just need to work out how to update the footprints in the PCB. I seem to have to just add the footprint again, after deleting the old one. Is this because the hole is not in the schematic? I have Update Footprints checked in Update PCB from Schematic.
OK, found the Update Footprints. I have to select a footprint, right click on a footprint to bring up the options and then there is an update selected or all footprints option!
Too bad the solder paste still isn’t showing up on the hole in the pcb…
It’s odd as the red circle seems to come and go on the footprint editor, depending on if the layer is selected:
That looks OK but you should check the Gerbers to ensure that the holes exist in both stencil (i.e. in the paste layer) as well as the board. A note in the fabrication instructions is recommended. The layer select mechanism brings the selected layer to the front.
Just hover over the footprint on the board layout and press ‘e’. You can then change the old footprint to your new one - you can change all of the same footprints together. If you have the holes called out in the schematic, you can change them there and update the board from the schematic.
I usually put these holes on a multiple of a 10mm grid and then can place the pins in a tooling plate drilled at 10mm centres which improves the stability for larger boards. For small boards you can just use a couple of pins and a couple of boards stacked together to provide some support.
Yes, it looks ok in the footprint editor, but there’s no solder paste showing in the pcb layout?
I guess it just wont show the solder paste as it’s the same size as a hole? If I add a rectangle of solder paste, over the hole, it shows up on the PCB.
The solder paste circle does show up in the gerber so that’s fine. It will be on the paste stencil. It’s just odd that it won’t show on the PCB editor in KiCad.
All done and PCB’s and Stencil look spot on! Thanks for your help everyone!
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
