The yellow area on your footprint is the copper. Your jack has three lugs which need holes or slots to pass through the board. At present you have small holes in rectangular copper pads. Have a look at the 3d view (alt + 3) to see what this FP will look like.
You can see the feet of the component in the datasheet. In this case, especially if you solder it manually, the footprint can be almost anything if three requirements are met:
The feet go into the holes (i.e. the holes must be large enough).
It must be easy to solder (i.e. the holes must be small enough).
The manufacturer is happy with it.
Most probably normal circular pads would be OK, the hole diameter should be about 3mm and the copper ring width around it about something like between 0.2mm and 1mm. (EDIT: ring width must be much more than 0.2mm for solderability and durability.)
Look at the foto or drawing of the part again. It does not have round pins. The cross section of the pins is what has the measurement 3x0.8mm.
This means you either need a slot for every pin that can fit 3x0.8mm or you need a round hole of size 3mm (plus a bit more)
Right now you have a round hole with diameter 0.762mm (Where does this drill size even come from?)
If you want to go with plated slots you might check with your manufacturer if they can produce them. (Or if it will cost extra to get plated slots)
If they can then there are a few options available how you can define them in kicad.
One option is to use the oval drill feature of kicad (set the drill shape to oval hole and set the two drill size parameters to the required size)
Another option is by using the edge cuts layer do define a slot. (For manufacturers whose software does not understand the oval hole definition made by kicad)
I suggest you ditch the suggested footprint and think about how you would create a footprint if you had only the physical component at hand.
This isn’t a general comment about creating footprints, just for this case. You could learn more by taking into consideration the actual physical characteristics of the component rather than trying to duplicate the existing footprint.
Hi @renegadeandy
supposing you are looking for this component
694108301002 https://www.google.com/search?q=694108301002
you can get the footprint for kicad directly a this site: http://componentsearchengine.com/ placing the code 694108301002
in the searcher. http://componentsearchengine.com/search.html?searchString=694108301002
You will get the ECAD model for many sw with kicad included.
And then you will have a fp to modify as you would decide.
Unfortunately you need to register to get it, but the license for the footprint is really kicad like.
The footprint will be in the old ‘.mod’ format, but it can be imported/loaded by KiCAD footprint editor.
PS: I’m NOT in any way affiliated to RS nor SamacSys companies, I simply found they are offering a nice service (for the moment free and with an usable license plan)
Because you seem to have a 2.8mm pin and a 0.762mm hole. It doesn’t fit. I meant you are trying to copy the footprint from the datasheet footprint specifications. I was suggesting you forget that example footprint and think only the physical characteristics of the component. That way you would have noticed what is actually wrong with your footprint.
Drill bit size is always circle, there are no oval drill bits. Oval holes (slots) are usually made by moving a round bit, not just by drilling.
What do you mean by that? Do you mean that KiCad made it by default? Again, it’s the size of the actual physical hole in the board and the component foot doesn’t fit there.
