This pad stack is for “dome”, or “snaptron”. It is switch “snap” board.
Any idea how to make this type pad? Kicad footprint editor does not contain this type pad. Looks only way is make circle to copper layer, put pad inside circle line and put second pad inside. But, drc not love this type idea.
Is it any “official” way to make this type pad? Eg. “make pad in other software, export DWG, import…” or any other idea?
I would imagine, draw a circle on a copper layer of the center radius, set to the equivalent width, and use the square point as the anchor pad, then add a normal SMD round pad in the middle, By rights as it contains no holes, kicad DRC should be happy,
If you are on K v5 you can use a custom pad: (GAL must be used)
NB dimensions done without looking at the DS
snaptron.kicad_mod (574 Bytes)
Thanks, my Kicad is 5.0 looks last version.
But, there is no this “merge”.
So, I make SMD-pad. Then I make circle. (I test both, layers “F.cu” and “dwgs user”, no difference).
Then I select both, circle and pad, and mouse left button…
There is no “Merge”. “Create pad from selected shape” say only “cannot convert… unsupported items”. Selection “Explode…” make nothing.
So, it looks easy, but maybe this my Kicad is any old version (5.0) and there is no this “Merge”?
Thanks to ready file. But, looks I need this prefs also later and this is reason I try find…
So… is this “merge” any special additional tool? Maybe it must download from any source? Or, my Kicad is too old or too new?
Select the circle and the normal pad, then “Create Pad from Selected Shapes”. IIRC the center of the normal pad must be inside the graphic shape (in this case meaning the inner and outer bound of the circular line).
Ok, now it works. It must be inside circle and it works.
Need much more study. Eg. now I put normal SMD pad inside this circle and “Pad properties”, “2” (it number) but no any effect. Is it any preference whick “lock” it pad? So how I can lock out preferences? Now I have little pad “2” middle of circle (it innner, it is not connected to circle). I cannot edit it…
EDIT. Solved. It icon on tool bar is not right way. First, move text away and then double click…
Also worth knowing is that after you have created the combined pad, you have to “Explode” it to be able to edit the circle and the normal pad again.
Sorry, one question and then all.
Middle pad (0,0) is 3,81 mm. So pad1 = outer circle and it is ok.
Middle pad need: outer dimension 3,81 mm. Double-sided: 3,81 mm, opposite side 1.5 mm, hole 0,9 mm, metallized. BUT. Hole center not in 0,0— eg. 0,3 mm from center. (First picture in this thread.)
Is it any way move it drill hole to other place than 0?
Try “Shape Offset” in the pad properties. Or you can place two pads, one SMD and one through hole and give them same pad number.
You can edit the combined pad using the Tab ‘Custom Shape Primitives’
https://drive.google.com/file/d/1UxJ6HGXe5GWfpCgqUetb2UrU4g214W1O/view?usp=sharing
Ok. First time test Kicad. I have Pads experience from 1996, and now I try this.
Looks not so easy as in Pads, but ok. Eg. this hole with offset need two pad. Maybe there is any way make it with one pad, but in my Kicad it offset is “grey”. All this area must be open in solder mask top, under dome switch there is no place for solder mask.
This was very good test. Looks “pad stack” setting in Kicad need more “jinx”. Eg. if I need thru-hole “different pad form and size in every layer” is very difficult. Also buried looks impossible. Eg. Pads style pads stack need several pads with same pin number: one pad per layer.
But, looks good.
One comment on domed buttons we have used way back…
The sticky tape used to hold them in place, was prone to softening and release, over time, and we also saw domes flip upside down, and never click back, after some cycles…
End result, they were designed out, to never be used again.
This seems to offset - actually I think the hole stays put, and the pad moves, but the relative offset is what you want.
Thinking about the usage of these pads, I don’t think using the offset would work in KiCad. Simply because KiCad doesn’t have robust padstack handling. (Hopefully that will change, but I don’t know where it is on the roadmap if it is there at all.) The pad on the back would be the same size as the pad on the front. I think in this case one would want a via-sized annular ring on the back side. Thus I would build it with a round SMT pad and a via sized THT pad offset from center, both with the same pin number (2 in this case). And, it seems that is the way @elkesan described it in his previous message.
KiCad handles padstacks, as a stack of individual layer pads, so if you want differing sizes on differing layers, you just stackup those definitions.
eg this has differing pads on F.Cu and B.Cu
IIRC what is missing from kiCad is a means to easily define inner layer pad stacks.
Semantics I guess. KiCad handles it as a stack of individual pad objects. Instead of a single pad-stack object with individually configurable layer settings. i.e. not a single pad with different top, bottom, and inner annular rings, and a flag to exclude pads on inner layers if there isn’t any connection.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
