Review of DC Barrel Jack PCB footprint - Things don't add up!

I had a quick check - there is a Barrel Jack FP in the 4.0.7 stock libraries without the rounded pads - a quick check of the dimensions suggests that it is the correct size for your application. It is in the ‘Connectors’ library.

1 Like

if you search for

then you get the footprint.

You can then compare your new one with what they give you …

you can always check it mechanically with the manufacturer 3D model
still not always 3D models are fully accurate… a review with the physical model is always necessary

1 Like

That’s my problem. I have got the spacing correct as far as I believe but there is a still a problem, and I would like support to find out where I made a mistake.

@John_Pateman This may be the case - but I would also like to learn how to do this!

For reference, this is the footprint for this connector that i will add to the official library BarrelJack_Wuerth_6941xx301002.kicad_mod (2.4 KB)

Pull request:

On Kicad 5rc02, there is a helpful ‘Caliper’. Not sure if it is present in 4.0.7. The dimensions seem to accord with your initial requirements.

Where did you find that? From that site?

I just want to understand the mistake I have made in making the footprint - please can we focus on that for now?

In particular:

Issue 1:
Pad 1, should be 13.6 to the very back of the jack.
On my footprint, it is 13.25
This doesn’t seem right.

I just made it myself. (In accordance with the library convention because i also started the process for this to be added to the future kicad library.)

1 Like

These are just two screen shots from the FP Editor. I am using V5 so it might look slightly different if you are using 4.0.7 - in particular, I am not sure if the ‘Caliper’ tool is available in 4. To measure something, you might have to use the spacebar technique in 4.0.7.

Place your cursor over the middle of a pad and press the space bar. Move the cursor to the point of reference - i.e.e the edge of the connector and look at the dX / dY or Distance reading on the bottom of the window to measure the distance between the two points.

As I said, this is the standard Barrel_Jack footprint from the stock Kicad ‘Connectors’ library.

Whilst it is an essential skill to be able to make your own footprints, in this case, there would seem to be a suitable footprint available in both the 4.0.7 and 5 standard KiCad libraries.

I already told you how to fix that, move the left (front) edge of the component outline.

1 Like

That shouldn’t be necessary though, the outline is the correct length, 14.5 and the spacings appear valid.

Maybe you could take a look by importing the file because you won’t see what I am saying until you take a look.

In that case you move the entire outline to the left. But your pin spacing is incorrect. How is that possible if you followed the guidance of everyone else and set your grid accordingly?

Ok - Helpful…can you be more specific, where is it incorrect and how can I fix it?

@Rene_Poschl you made a footprint and it looks ideal - thank you. Would it be possible for you to record the process of making that again – that way I could actually review what you are doing and how you work through each of the bits needed?

Just look at the coordinates of your pads. Pad 1 is at X=0 and pad 2 is at X=-5.45 where did you get that dimension from? To fix it just enter the correct position. And pad 3 will need to move as well. Then you can move the outline.

1 Like

Hmm, so should it be -5.8 perhaps?

Taking position of pad 1 as offset 13.6 and then position of pad 2 is 7.8

Therefore 13.6 - 7.8 should be the gap between them which is 5.8?

1 Like

That is Correct. Since the drawing uses the front of the connector and the center as references for the measurements you could have assumed that to be the origin of the part and then used the same dimensions as on the drawing to locate other elements of the footprint.


I moved the whole footprint so that the front (left) edge was at 0 and then it took me less than a minute to set all of the dimensions correctly to the same values as in the drawing. Your outline was also inaccurately drawn, the lines didn’t even end and begin at the same coordinate with errors of 0.02 mm. You need to learn to either use the grid when using the mouse to move/align items or edit the coordinates directly.


Here you go: Tutorial: How to make a footprint in KiCad 5.1.x (From scratch)?

1 Like can download foot print

Or you know take the one created by the head of the official library :wink:
(It will be in the v5 library if everything goes well)

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