Hi,
I need to add mounting holes for these “SMD” metal spacers to a footprint.
As can be seen in the document, I need to make an NPTH, but with a solder ring w/ paste on the side/layer the spacer gets soldered to.
So far I tried to create such a mounting hole by adding an NPTH, and rings around the hole on the front copper and paste layers, and at first glance it looks as it does the business, but on closer inspection, copper pours are not kept out of the area of the mounting hole, even when setting the pad clearance to some positive number (is that a bug, btw?), so that won’t work.
Any suggestions on creating such mounting holes where any copper is kept away from the hole, except for the one on the layer/side where the thing needs to be soldered?
Circular NPTH (size=drill) with pad and mask clearance set to 1mm - as can be seen, the copper polygon is not “cleared”:
I hereby certify that I am not simply asking someone else to design a footprint for me.
This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.
I’m a little confused by the combination of words you used…
I suspect what you want is:
• SMD Pad to Solder the Spacer to
• Want the PAD to be that specified in the Drawing
• A Location Hole in the PCB/Footprint for location
If that’s the Case, there is No need to even think beyond that (meaning, no Cu in hole… just a SMD Pad with a hole…
Hmm… It seems that drawing directly into the copper layers causes the pad clearance to have no effect, but after restarting kicad, the pad clearance for an npth pad actually had an effect on the filled zones in the pcb, so that’s good (don’t know if the footprint wasn’t properly updated or something).
@BlackCoffee I can’t get your footprint to load, was it done in kicad 6? I’m using 5.
When you say I need a “location hole”, what do you mean exactly - an npth pad?
If so, I think it still needs some clearance to avoid the metal apcer to short to any zones on inner layers.
Yes, location hole is NPTH (npth’s don’t have pad, unless you want to make one. I just made NPTH on top of the SMD pad. That yields a Location Hole per the drawing).
You can Tweak the .mod (or, make a new footprint to get desired clearance (good experience for you…)
My intent was not to provide Exactly what ‘I guessed you wanted’ rather, to provide an Example that you can tweak for learning/use)
The SMD pad is per the drawing you provided (7.4mm diameter)
EDIT: Added screenshot of the SMD Pad and the NPTH hole on top of it (with hidden Spacer model…)
These footprints could need some hacks involving graphical shapes to get them correct, at the very least for the solder paste layer. You don’t want solder to wick into the NPTH and some board manufacturers might need some additional cleareance between copper and the NPTH.
Wuerth Elektronik are providing eagle libraries for their parts as a starting point. Find your part in their online catalog, you can then import the eagle library in kicad and either modify it further or copy some pads or settings.
That’s all good, I didn’t expect you to build a finished footprint for me - also, I need the 977 403 095 1 part
@sschaak I drew a fat circle on F.Cu that doesn’t extend all the way to the hole, and a circle on F.Paste with slightly smaller thickness for the paste, but it’s probably a good idea to check the Eagle footprint for dimensions on these things since the datasheet doesn’t really specify this
I am surprised that NPTH is used for it.
When we used terminal blocks at single layer PCB we had a problem that sometimes the pad was broken during fastening the wire. To avoid that problem we used 2 layer PCB just to have PTH.
If you use PTH I think the spacer will be mounted more firmly.
In KiCad library there are even mounting holes with several small PTHs around the center hole to make the construction more robust.
The parts with a smooth through-hole should not experience any significant torque and the threaded parts have a specified maximum torque. I haven’t seen any board mounted spacers or studs used for high torque applications, usually they are just standoffs for daughter boards (think M.2 for SSDs/Wifi/WAN or mezzanine boards). If you really need higher forces, you should use via-reinforced mounting holes and the usual standoffs.
Using a PTH has several drawbacks for most types except externally threaded ones with a solid bottom:
solder and/or flux can wick into the threads or obstruct the through-holes
the usual THR or pin-in-paste process using the fully automated SMT machines cannot be used due to the large hole size and causing the problem above
selective soldering can also cause obstructions and solder wicking and is often done after manually placing the THT components, increasing costs
slightly off-topic; i’ve been looking at those Wurth spacers as well, but they’re expensive and i don’t like using single-source parts. Does anyone know of crosses for these types of parts? Even if it’s not cheaper I like knowing there’s another manufacturer out there.
@StecklerCircuits I have been using these the Wurth spacers on a couple of boards (using the Kicad Wurth- footprints), and they work well. I could not not find any other vendor that had the size I needed, and I could not find any direct vendor crosses. The footprints seem to vary by vendor. If I recall, Keystone makes something similar. However, the Wurths work great for putting on a standoff using a standard SMT process.
I previously posted a link to McMasterCarr and intended to also post a link to ‘All Electronics’. I’ve bought many things from them that were somewhat difficult to find elsewhere (because, in addition typical things we use, they also inventory closed-out and surplus items).
Here’s their link to StandOff’… Prices are usually Pennies (example, qty 10 for $1)
