Footprint for FPC 0.5mm connector


I am tryin to make a footprint for

The footprint looks really complex for a 0.5mm connector. What parts of these do I need to implement?

Also for the orientation, can I simply twist the cable and assume anything that makes it easier for me to route or should I look at how the input FPC is coming in?

Page 3 of 9 has the dimensions for the Recommend Board Layout.
This part is complex enough, and the drawing not the best, that I would purchase one of these to have “in-hand” while creating this footprint.

That drawing doesn’t look bad to me. For handsoldering you can use a rectangle pad for the mounting pads, will make it a lot easier for you. This migth even work for reflow soldering if you take care where you place paste.

Thankjs for the help

That’s the pads you want… I’d not do the small bite-outs in the corners for the mounting plate fixing pads.


And this is a footprint from me for a FPC 0.5mm connector from TE I did some time ago (ignore the pin#1 marker under the footprint, bad practice):


Make sure that if you use the version where the lever COMES OUT to mark that space as a keep-free zone in your footprint and also draw in the FPC (end position inside the connector - insertion depth - and width/path outside of it for some length) - all so you don’t place other components in that area.
The insertion depth is useful once you want to specify the FPC length :wink:

for above footprint:
yellow - Cmts.User (I use this layer for collission information after assembly/during use)
light grey - F.CrtYd (contains the extended lever for this particular connector as there really should nothing be in that space ever, the FPC can probably go over flat SMD parts past that area, your pdf specifies 0.96 mm from top of board to center of FPC)


Also note that by my personal nomenclature your connector would carry a TOP in the name, depicting that the contacts on the FPC will be made on the top and not on the bottom. This might be important information down the road as this (together with the counterpart on the other board) will decide what kind of FPC you need… contacts on same side or other sides :wink:

PS: personal tip - make 100% sure you connect the correct pins from one board to the other, taking into account the flipping over of the FPC or any other stuff. Really think 3 times here and don’t be afraid to use paper+scissors to create a real life model (pin#1 markers for each end + side of connections) to make sure you got it right.


I am a little confused about where in the PDF it says that the contacts on the cable must be on the top? I thought the connector is suc that I could always flip the cable .

The last image in the previous post shows the “Conductive Side” of the cable being on the top. The PDF includes two different connectors, one has the contacts on top the other has them on the bottom.

1 Like

This is what my TE connector model looks like cut open:

Those kind of connectors press the FPC onto those contacts from one side via the sliding/lever action. Dependent how it’s designed on the inside. That’s why I wrote that you need to check 3 times that you got it all understood and checked, before you commit.
Also just ‘flipping the FPC’ will cause the signal being on pin#1 to become signal on the last pin and vice versa…

1 Like

How did you cut open the model? Is there some specific tool that you use?

Autodesk Inventor
Only works because I made the model myself, and it’s not even very detailed.
But I actually modeled it from the 2D pdf datasheet that I had for it, so :wink:

The models that ship with KiCAD might not be on that level - which is not bad - as those kind of details are useless for the purpose that KiCAD 3D models are made for. I essentially went overboard there.

If you get manufacturer CAD models they might be even more detailed (larger file size, slower 3D view) and contain every piece that they are made off and if you open them in a free tool like FreeCAD you might be able to see it all (take STEP format).

1 Like

Must be quite a bit easier if you have already done it in 3D!

I still think that my recommendation to have a physical part in hand could likely assist in understanding how to create a KiCad Footprint for the part. And, this concept does not apply to only this particular part.

P.S. Pretty nifty 3D CAD images!

That was for the FPC… you cut a piece of paper and treat it as a FPC, mark the connector sides and also pin #1 on each end (make sure you understand that this is a 1:1 cable and that there are no crossings).

If you’re rolling your own flexible cable pcb it’s a little different and you’re exceeding my current state of knowledge, as I haven’t done anything there yet. I’m referring to stuff like this:

1 Like

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.