I **LOVE** KiCAD! --- Interesting hack

[cal-linux]

Have I mentioned lately that I love KiCAD!?

I had this idea that I came up with to simplify reflow-soldering with a stencil; the problem I was addressing was the part of getting the stencil and the board positioned and immobilized with respect to each other.

My idea was: assuming the board has its four (or >= 4) mounting holes near the corners, and assuming as an example that the holes are 1/8 inch in diameter, then create the stencil with 1/8-inch holes at the positions of the mounting holes, then get four spacers (e.g., this nylon spacer) to be used as pins — align the stencil on top of the board, then slide one pin through the stencil inside each of the mounting holes; now the stencil is immobilized; I usually create the holes at 129 mils, so that with the plating it comes down to 126 or 127 mils; a tiny bit of margin above the 125 mils of the spacer. The holes in the stencil are 127 mils in diameter.

Back in the day, with gEDA PCB, I had to create a separate PCB file for the stencil, where I would just manually (i.e., with a text editor) edit the PCB file to turn the mounting holes into SMD pads at the same position and with the right diameter; then, I would produce the paste layer based on that separate stencil file.

Yesterday, I was finishing up what is being my first KiCAD project where I’m going to order a stencil to solder myself — I was getting ready to make a separate copy of the project and change things, when the lightbulb went on in my head and I realized that I simply needed to change the MountingHole footprint — in KiCAD, the paste layer is a first-class citizen; a layer on its own (in gEDA, the software simply outputs the SMD pads for the paste Gerber file). I then realized that: wait a second, I don’t even need to do it specifically for this layout; I can just change my custom (user-provided) MountingHole footprint and just add the pad on the paste layer — for normal (read, if I don’t need a stencil) layouts, I can still use it, and the extra pad on the paste layer will have no effect. Of course, the issue is that if I send off the layout for manufacturing including assembly/soldering, the fab may use a stencil, and then they will end up with a stencil that pours solder past onto a hole. So, you know, one can have one footprint specifically for the cases when one wants to do this trick with the stencil. Here’s the example MountingHole footprint I created:

(module MountingHole_3.2mm (layer F.Cu) (tedit 5C86C191)
  (descr "Mounting Hole 3.2mm, M3")
  (tags "mounting hole 3.2mm m3")
  (clearance 1)
  (attr virtual)
  (fp_text reference REF** (at 0 -4.2) (layer F.SilkS)
    (effects (font (size 1 1) (thickness 0.15)))
  )
  (fp_text value MountingHole_3.2mm (at 0 4.2) (layer F.Fab)
    (effects (font (size 1 1) (thickness 0.15)))
  )
  (fp_circle (center 0 0) (end 3 0) (layer F.CrtYd) (width 0.05))
  (fp_circle (center 0 0) (end 2.34 0) (layer Cmts.User) (width 0.15))
  (fp_text user %R (at 0.3 0) (layer F.Fab)
    (effects (font (size 1 1) (thickness 0.15)))
  )
  (pad 1 thru_hole circle (at 0 0) (size 4.4 4.4) (drill 3.25) (layers *.Cu *.Mask))
  (pad 1 smd circle (at 0 0) (size 3.225 3.225) (layers F.Paste))
)

The very last line (well, excluding the line with the closing bracket) is what implements the trick.

[EDIT] — Right! I just remembered, another (minor) downside is that now in the 3D view, it shows somewhat of an “eye sore”, by showing a grey flat opaque surface covering the mounting hole (when turning and looking through the bottom, you can see the hole, although it still shows blocked at the other side, at the end of the hole) [END EDIT]

Needless to say (though the subject did say it!), that brought me to one of the many big I-LOVE-KiCAD monents!!

Which brings me to: once more: thanks to the community and the developers (past and present) for creating and maintaining such an awesome software!

[dchisholm]

I have been using KiCAD-generated stencils for the last 18 months or so and I’m quite pleased with the results! A plastic (“Kapton”, if I remember correctly) stencil costs about $US 10, including postage. The time to manually place components on an SMT board is about 1/4 to 1/3 what it was when I used a syringe (and toothpicks) to dispense solder paste. Perhaps more significantly, the soldering quality is incomparably better: instead of getting solder bridges on one IC out of every 3 or 4, it’s now around one in 100. Solder balls are almost totally gone. I see 1 or 2 starved solder joints out of 100 components or so - I suspect that is the result of accidentally scraping solder paste off the pads during manual component placement.

My “stencil frames” are scraps of plywood or HDPE sheet, with pieces of old PCB’s screwed in place to create edges where I align the PCB being stenciled. The stencil itself is held in place with a piece of duct tape along ONE edge only. The tape serves as a hinge, allowing me to smoothly lift the stencil away from the board after printing the paste into place. (It’s important to cleanly lift the stencil away from the board after printing, to avoid smearing the paste placement.) Registration errors between the board and stencil are tolerable up to about 10 mils (0.25mm).

With a little practice I learned how much I could vary the solder paste print from “heavy” to “light” based on how I held the spreader tool (a piece of plastic like an old credit card or ID badge), and how hard I pressed. If you use footprints intended for “manual soldering” of SMT components you may want to define the stencil cutouts somewhat smaller than KiCAD’s default values - the enlarged pads for manual soldering put a lot of unnecessary solder paste on the board, which can create solder bridges and solder balls. Like any of the high-priced layout software, KiCAD gives you a usable stencil aperture with absolutely no effort, or lets you customize the aperture for your specific situation.

The more forgiving formulations of solder paste claim a shelf life of 6 months when stored under refrigeration. My solder paste has been in a desk drawer for over 18 months, but is becoming a little cantankerous to work with.

Using the manual paste-printing methods described above, and hand-placing components with tweezers under a desk magnifier, I am successfully working with component pitch down to about 40 mil (1 mm) even with my superannuated, tri-focaled eyeballs. Six-pin SOT-23 packages, and SOD-123 diodes, require careful attention. I suspect I could work with pitches at least one step smaller (perhaps two steps) using the toolmaker’s microscope.

The “reflow oven” here is a table-top electric skillet from the second-hand store, but that takes a different discussion thread.

Dale

[John_Pateman]

I have used a similar technique for a while - I have a set of ‘registration’ footprints which accept a 2.5mm metal dowel pin and they each have an appropriate sized solder paste layer to ensure that there is a corresponding hole in the stencil. I have also machined a 30x20cm registration plate out of 10mm thick Delrin with holes on a 10mm grid. (In retrospect, fewer holes would have also been fine - you can buy aluminium fixture plates ready made but you need to do a bit of searching to find a cheap one). You can use the registration holes as actual mounting holes for your board or put them on a frame of a panel/mini-panel and get multiple boards stencilled at the same time. The stencil alignment is excellent - but you do have to be quite careful to ensure that the pins are only just through the pcb to ensure that you can lift the stencil cleanly. Two pins are all that is needed for the small panels that I have produced - I just ensure that they are correctly spaced a multiple of 10mm apart using a coarse grid. I usually keep the boards on the alignment fixture whilst populating them by hand and then lift them off before going in the toaster. I have done TQFP 0.8mm without any problems using this technique and I am fairly confident that smaller is doable with care.