Hi All, my first post so hopefully im asking the right questions.
I’ve attempted to move from eagle to kicad a number of times, but this is the first time i’ve really managed to start understanding KiCAD and so far im pretty happy. But i’m putting together a small board and have a hit a point where i need to create my own footprint. The Footprint is not an easy one either (M.2 connector) this one to be precise. But there were a couple of things i couldn’t quite figure out… firstly how i make just a drill hole for its two plastic legs the component has and what f.mask is actually trying to define when your creating smd pads (it appears to be a solder mask clearence im guessing?) and so im not quite understanding what impact that has on what would appear on the final board?
I’ve assumed for the drill holes i just create an unnumbered pin with its drill hole the same size as its pad size
In any case, here is my first attempt and I wouldn’t mind some feedback (bearing in mind its draft).
Thanks All.
Component outline & courtyard? Physically interfering with other components would most likely suck. AND the pad-width is definitely off. Should be 0.3mm.
1 Like
Set the pad type to npth, mechanical and it should be ok.
One of my mechanical holes from an hirose connector:
Marked are the important bits.
(Drill size is of course dependent on your part.)
As mentioned by @madworm, your padwidth is not optimal:
when desinging your footprint look at page 3 of your pdf. (There the padsize is given as 1.55x0.3mm)
page 1 has the dimensions of the connector, page 3 the recommended footprint measurements.
1 Like
I changed the smd pad sizes in an text editor and also changed the pad type to npth.
Here the file if you want it.
M.2.kicad_mod (5.1 KB)
1 Like
@takigama
Don’t populate the VAL and REF fields in the footprint editor… those are being populated by the symbols, the footprint only defines where those values appear and how they are formatted.
Just use VAL** and REF** (and if you need more of the same use %R and %V).
The origin of your footprint doesn’t agree with the one in the pdf. The vertical center line is clearly given (red)… for the horizontal one I would settle for the pass mark holes (green).
I see why you didn’t draw the housing as the measurements along the short axis for it are missing.
But you could at least have put a courtyard around it 
I assumed the pins overshoot the housing by 0.6 mm and came up with this:
Conn_TE-M.2-0.5-67P-doublesided.kicad_mod (7.9 KB)
PS: the pass mark holes were too big… physically the pins are 0.8 and 1.45 respectively. TE already gave them plenty space by defining 1.1 and 1.6 drill holes - no need to go bigger than that.
PPS: The pads where 0.025 mm off vertically vs the pass mark holes 
PPPS: not a bad job though for your first 
2 Likes
Thanks so much everyone, that was really informative!! 
quite a few things there i didnt realised i’d made mistakes on or hadnt thought through (like the center line). I cant quite figure out where i got a pad width of 0.14 from.
I’ll be pushing these up to github with appropriate attribution once I finish making a complete component (though the 3d model will probably come in a later version) and after that there a few other components im hoping to get done as well
I’ve updated this one and put in the missing pins as its useful as a generic m.2 for any type of keying and uploaded to my kicad libraries github https://github.com/takigama/KiCADComponents
Its also been tested now so everything lines up as it should.
I’ve now built and tested a board using this connector, does indeed all line up very well:
4 Likes
