is what I use… I think I drew it myself? Anyway, it works for SPDT.
2 Likes
Hi,
so I’m learning KiCad…
I wanted to edit the jack’s footprints to put oval pads instead of circular ones (as an exercice, but this could also make soldering easier with less empty space to fill with solder)
So I downloaded Tayda’s datasheet to find out the pins/lugs sizes, and I found that the footprint matches the “Viewed from copper side” view.
Is this (these in fact, Sam’s and analogoutput’s) footprints designed for soldering the jacks on the “copper” side of the board, well, on the “other” side than “normal” components ?
1 Like
Answering myself…
The Tayda jacks are symmetric about the “center-GND pin” diagonal, so they can fit on both side of the PCB.
But the pin labelling (assuming T is tip, and S is ring) is for mounting the jacks on the component side of the PCB.
Everything is OK, lesson learned 
1 Like
This footprint https://github.com/holmesrichards/kicadfootprints/blob/master/Jack_6.35mm_PJ_629HAN.kicad_mod (with round holes) works with Tayda jacks and has pins labeled properly.
4 Likes
S is sleeve. R would be ring…
1 Like
Usually, yes, S is sleeve.
But there is a GND pin, which is the sleeve…
1 Like
The Tayda jacks are stereo with five pins: Tip, tip normal, ring, ring normal, and ground (sleeve). The datasheet I downloaded from Tayda doesn’t use labels T, R, S, it just shows the connections pictorially. The footprint I use looks like:
(viewed from the component side)
5 Likes
Any chance you could re-share this?
(module SPDT-toggle-switch-1M-series (layer F.Cu) (tedit 61227C47)
(fp_text reference REF** (at 0 -7.4) (layer F.SilkS)
(effects (font (size 0.75 0.75) (thickness 0.15)))
)
(fp_text value SPDT-toggle-switch-1M-series (at 0 9.4) (layer F.Fab)
(effects (font (size 1 1) (thickness 0.15)))
)
(fp_line (start -3.7 6.6) (end -3.7 -6.6) (layer F.CrtYd) (width 0.12))
(fp_line (start 3.7 6.6) (end -3.7 6.6) (layer F.CrtYd) (width 0.12))
(fp_line (start 3.7 -6.6) (end 3.7 6.6) (layer F.CrtYd) (width 0.12))
(fp_line (start -3.7 -6.6) (end 3.7 -6.6) (layer F.CrtYd) (width 0.12))
(fp_line (start 3.42 -6.35) (end 3.42 -6.34) (layer F.SilkS) (width 0.12))
(fp_line (start -3.43 -6.35) (end 3.42 -6.35) (layer F.SilkS) (width 0.12))
(fp_line (start -3.43 6.34) (end -3.43 -6.35) (layer F.SilkS) (width 0.12))
(fp_line (start 3.43 6.35) (end -3.43 6.35) (layer F.SilkS) (width 0.12))
(fp_line (start 3.43 -6.35) (end 3.43 6.35) (layer F.SilkS) (width 0.12))
(fp_text user %R (at 0 -2.2) (layer F.Fab)
(effects (font (size 1 1) (thickness 0.15)))
)
(pad 2 thru_hole circle (at 0 0) (size 3.1 3.1) (drill 2.1) (layers *.Cu *.Mask))
(pad 3 thru_hole circle (at 0 -4.7) (size 3.1 3.1) (drill 2.1) (layers *.Cu *.Mask))
(pad 1 thru_hole circle (at 0 4.7) (size 3.1 3.1) (drill 2.1) (layers *.Cu *.Mask))
(model "${KICAD_USER_LIBRARY}/aoKicad/ao_tht_3d/User Library-7101SYZBE CK switch.step"
(offset (xyz 0 0 9))
(scale (xyz 1 1 1))
(rotate (xyz 90 -90 0))
)
)
(Cut and paste that into a file named SPDT-toggle-switch-1M-series.kicad_mod)
1 Like
Fantastic, thank you!
Gahh. I just noticed this.
Alps RK09K 9mm vertical board mount pot footprint:
Alpha RD901F 9mm vertical board mount pot footprint:
Spot the difference?
It’s not as if Alps uses that pin numbering. From https://tech.alpsalpine.com/prod/e/pdf/potentiometer/rotarypotentiometers/rk09k/rk09k.pdf:
Weird.
Nice catch.
I too had been plagued with inverse potentiometer syndrome, and had been convinced I’d either poorly wired it up in the schematic or flipped/rotated the footprints in my layout. I just went back and double checked the library footprints - the bourns ptv09a-1 in the KiCad THT library are also afflicted with this same pin reversal phenomenon. I thought to myself “I should add cross referencing the footprint to the datasheet pinout to my sign-off checklist”. I opened my checklist - it’s already in there. So maybe I should add going through the sign-off checklist as the first item in my sign-off checklist…
3 Likes
I probably should add “Don’t say ‘yeah yeah it’s probably all right, next item?’” to my checklist.
Added:
It’s even worse than I thought. Looking through the pots footprints it appears nearly all the vertical ones have pin 1 CW. The only exceptions being the Alphas and TT_P0915N. Yet all the horizontal ones have pin 1 CCW.
Jack footprint with oval holes:
(module Jack_6.35mm_PJ_629HAN_slots (layer F.Cu) (tedit 613C19D3)
(fp_text reference REF** (at 0 -9.5) (layer F.SilkS)
(effects (font (size 0.75 0.75) (thickness 0.15)))
)
(fp_text value Jack_6.35mm_PJ_629HAN_slots (at 0 10) (layer F.Fab)
(effects (font (size 1 1) (thickness 0.15)))
)
(fp_line (start -7.994 -7.99) (end 7.954 -7.99) (layer F.Fab) (width 0.12))
(fp_line (start 7.954 -7.99) (end 7.954 5.926) (layer F.Fab) (width 0.12))
(fp_line (start -7.9 -1.5) (end -7.9 -7.9) (layer F.SilkS) (width 0.12))
(fp_line (start -7.9 -7.9) (end -1.5 -7.9) (layer F.SilkS) (width 0.12))
(fp_line (start 7.85 5.8) (end 7.85 5.85) (layer F.SilkS) (width 0.12))
(fp_line (start -7.994 7.958) (end -7.994 -7.99) (layer F.Fab) (width 0.12))
(fp_line (start 7.954 5.926) (end 5.414 7.958) (layer F.Fab) (width 0.12))
(fp_line (start 7.85 -0.4) (end 7.85 5.8) (layer F.SilkS) (width 0.12))
(fp_line (start 5.35 7.85) (end -0.5 7.85) (layer F.SilkS) (width 0.12))
(fp_line (start 5.414 7.958) (end -7.994 7.958) (layer F.Fab) (width 0.12))
(fp_line (start -9 -9) (end 9 -9) (layer F.CrtYd) (width 0.12))
(fp_line (start 9 -9) (end 9 9) (layer F.CrtYd) (width 0.12))
(fp_line (start 9 9) (end -9 9) (layer F.CrtYd) (width 0.12))
(fp_line (start -9 9) (end -9 -9) (layer F.CrtYd) (width 0.12))
(fp_line (start 2.5 -7.9) (end 7.85 -7.9) (layer F.SilkS) (width 0.12))
(fp_line (start -7.9 7.85) (end -7.9 2.5) (layer F.SilkS) (width 0.12))
(fp_line (start -4.5 7.85) (end -7.9 7.85) (layer F.SilkS) (width 0.12))
(fp_line (start 7.85 5.85) (end 5.35 7.85) (layer F.SilkS) (width 0.12))
(fp_line (start 7.85 -7.9) (end 7.85 -4.7) (layer F.SilkS) (width 0.12))
(pad T thru_hole oval (at -6.4 0.5) (size 2.5 4.5) (drill oval 1 2.7) (layers *.Cu *.Mask))
(pad S thru_hole rect (at 4.74 4.74 45) (size 4.500001 2.500001) (drill oval 2.7 1) (layers *.Cu *.Mask))
(pad R thru_hole oval (at 0.5 -6.4) (size 4.500001 2.5) (drill oval 2.7 1) (layers *.Cu *.Mask))
(pad TN thru_hole oval (at -2.5 6.4) (size 4.5 2.5) (drill oval 2.7 1) (layers *.Cu *.Mask))
(pad RN thru_hole oval (at 6.4 -2.5) (size 2.500001 4.500001) (drill oval 1 2.7) (layers *.Cu *.Mask))
(model "${KICAD_USER_LIBRARY}/aoKicad/ao_tht_3d/User Library-jack-4.STEP"
(offset (xyz 0 0 23))
(scale (xyz 1 1 1))
(rotate (xyz 0 0 0))
)
)
2 Likes