I´m doing a project and thinking about doing a custom PCB, therefore I´m designing the board on Kicad.
I had to design a custom footprint for my audiojack, however I´m not sure if I selected the correct pads.
The width of the part´s connector is roughly 1mm, therefore I put a hole size of 1mm on the pad settings.
My jack is similar to the Ledino available on Kicad, however this one uses an oval and rectangular pads.
Should I copy Ledino´s or keep with circular pads?
I´m attaching pictures of my pads and the part itself.
Did you notice that the “datasheet” view is from the bottom, while KiCad footprints are top-down? You have to mirror the footprint.
Oval vs. round hole doesn’t matter much. It depends on the manufacturing and assembly process.If you will solder manually, round holes may be easier to use when the component is placed (flat tabs may be bent and not fit directly into a narrow slot), but round holes drink more solder. Some not so advanced board manufacturers may prefer round holes because they are easier to drill.
Oval vs. round copper shape may have only small effect, and only for soldering. Long oval pads may be better for hand soldering because there’s more room for iron and solder in one direction. The rectangle shape is used in the official KiCad libraries to indicate pin number 1. All in all, it doesn’t matter much if you just can do the soldering easily. Otherwise you can make the decisions based on aesthetics or on the latest lottery numbers.
I also believe that round holes are just fine. Using “oval” holes can be a problem during production. Round holes are just drilled while “oval” holes need a router bit that goes sideways through the FR4.
A while ago I also made:
Showing the bottom (and thus mirrored) view in datasheets is a PITA. Good of eelik to catch that. In that mini tutorial I wrote in 2017 I also printed the layout in mirror image to have the PCB pads shown from the bottom of the part, and it’s not entirely certain if you would catch this mistake with that method. But anyway, it’s always a good idea to have the parts and do some kind of fitting before you send out Gerbers to a PCB Fab.
Just a general concern: If the connector is going to be plugged in and removed more than once or twice, it is probably worth making the pads much larger, in order to improve the mechanical strength and decrease the risk of solder breakage, pads coming off from the substrate etc. due to the mechanical forces when plugging in and removing the connector, as well as pull from the cable.
I tried adding the footprint to my project but now I get an error:
Error: J1 pad T not found in components:Jack HUInfinito.
Error: J1 pad S not found in components:Jack HUInfinito.
Error: J1 pad R not found in components:Jack HUInfinito.
Error: J2 pad R not found in components:Jack HUInfinito.
Error: J2 pad T not found in components:Jack HUInfinito.
Error: J2 pad S not found in components:Jack HUInfinito.
I tried changing the names of the pad without sucess. Also, the connections don´t appear in the PCB file.
In KiCad the matching between schematic pins and footprint pads is done directly with the pin numbers, and these have to be the same for the schematic symbol and the footprint. So to fix it you either have to renumber the pins in your schematic symbol, or the pads in the footprint.
Pin “Numbers” are actually 4 digit alphanumeric strings, so you can also use “chessboard coordinates” such as common for BGA’s.
This is a CUI SJ1-3515N or compatible, which looks about right. J_3.5mm_TRS_SW_B.kicad_mod (2.7 KB)
Holes are 1.6mm. As @hmk says, make the pads a decent size for mechanical strength.
I used descriptive text names for these thru-hole pins, not just numbers, but it’s up to you.
I leave the symbol as an exercise for the student.
When I do a part like this, I sketch it out and re-dimension each pad from the centroid (this part is thru-hole so centroid is not a pick point but still). Then in editor I place a pad at centroid and do exact move, repeat for all pins, add silk…
Plop your new foorprint down on a test board, print at 100%, and see if it looks about right when you place a connector on it.
I changed the pad names to TRS, but for some reason it won´t update on the PCB file when I press the button update PCB from schematic. It´ll keep using the 1,2,3,4,5 pads instead of T,R,S,3,5.
And there is also the possibility to update the footprints with: PCB Editor / Tools / Update Footrpints from Library
If you’ve changed a Footprint, you’ve probably copied it first from a KiCad library into a project specific library. You can change that copy all you want, but as long as you do not change the footprint links in the schematic symbols to use your new library, then it will just keep on using the old library. There are a bunch of different ways to fix this. One is to hover over a footprint and press f to change the footprint link of a single schematic symbol, another is Schematic Editor / Tools / Edit Symbol Fields. Yet another option is to change the footprints on the PCB, and than push those changes back to the schematic with PCB Editor / Tools / Update Schematic from PCB.
I’m surprised you didn’t know/remember this Update PCB from Schematic option doesn’t update footprints. It changes the footprints which are changed in the schematic, i.e. if the footprint name is changed in the symbol properties.
Oops,
I sometimes mix up things, there are so many things in KiCad that can be done in different ways that I can’t remember them all. So I verified, changed a footprint in a project specific library, and updated the PCB, and it does indeed not update it. PCB Editor / Tools / Update Footprints from Library does update it though.
That gitlab link does trigger some memories…
I guess that the changed text disconnected it from previous experiences.
I still find the new text misleading though, as it does not change footprints. From what I gather it only updates the footprint links. Below a screenshot form the Footprint Properties in the PCB Editor. (It’s from a customized 1206 resistor) It also uses “Library Link”.
A general suggestion. If you have one of these jacks, BEFORE you order boards, print out a 1:1 of your board. Lay the physical switch on your printed board and verify the pins are what you want.
Believe me I learned this early. Things like this switch, custom transformers etc are so easy to invert this is well worth the effort.
I use similar Audio Connectors but, I use Mono (not Stereo) thus, fewer Pins.
The pins on mine are 1mm wide and I don’t worry about their ‘corner-to-corner’ length on the diagonal as there’s enough material removed from the holes in drilling to not worry about it. Yes, use a Round hole.
BUT - Important!! These connectors will NOT endure repeated plugging in/out - they are designed for Panel-Mounting, that’s why they have Threads and Nut. There are No Glue-Posts (which, are actually not for Glue but, rather, for Heat-Staking)
[Note: I have Patents on Connectors and spent years seeing all sorts of connector designs - and, failures… - get the spec-sheet for the one’s you plan to use…]
Sure, you can glue it to the PCB but…
ADDED: Something similar to this may be more appropriate - it has the alignment/Staking bosses screenshot below…
I didn’t go to the referenced post so I didn’t see your comments.
However I would disagree with reversing the print. I’ve always shied away from reversing anything. My experience it only adds another possibility to make a “moving too fast” error. However, I guess whatever works is OK.
BTW my first professional PCB’s were hand taped.
When I’ve made a footprint for a part, I’ve make a really small PCB that is just the footprint using OSHPark. Spend < $10 and you know the footprint is good. If this is an old or odd part where I’m measuring pin locations manually, this is a must. Then when you cut the > $20 PCB, there are no surprises. Most of my final cut PCBs are in the $30 to $80 range using OSHPark.
On some projects where there are more than 1 new footprints (especially with all through hole devices) you can often fit 2-4 foot prints on a small PCB because they can stack on each other. The PCB for a 4 foot print was $8, so it was $2 per footprint to be sure you had it right.
