Submitting Gerber with partial footprint outside edge, can i?

Have a 4 pos rotary switch, DP4T and want to put a small sub board on it.
Sub board only needs to be 1/2 the size of the rotary, and for economy sake we’ve ended up with a footprint hanging off the edge of the board in the final Gerber.

This suits us, but how will the fab house take it (JLC in this case)?

If it’s undesirable i then have a couple of questions…

  1. Is there a way to plot the board with anything outside the edge cuts ignored?
  2. Outside of creating a footprint for half the component is there any other way to have the offending pins ignored?

Not asking out of laziness, but rather the possibility of learning something clever.
More than happy to roll a footprint if need be.

Note, not displayed in picture, but after manufacture the PCB will have the left ends cut off into smaller boards. There is a 4th board that is longer horizontally just off screen in the pic that prevents us doing a V-score for the ends to be cut.

Sample attached.


Your best bet is to try and ask JLC if it is acceptable to them.

Send it to JLCPCB but dont pay for it just ask for a review at checkout.

I do this all the time. But, I don’t use JLC.

Why not make a new footprint, with the external pads removed? Then no more fuss with the fab.
Its only a few minutes work.


Yeah I would do this, OP. Otherwise you might get asked Is your board the right size, did you mean for the edge cut to be there? slowing you down more than a few minutes.

Appreciate all the replies.
Doing a new footprint was never an issue, was just thinking more along the lines of furthering my knowledge of KiCad features.

It felt like the possibility existed there might have been a clever way to opt not to have items outside the main edge cut render in the gerber, or to switch pins/pads off on a footprint.

Thanks again all, cheers!

I make footprints all the time. It is a straightforward way (that is not difficult) and makes life easier in a variety of ways. Including: 15 minutes with your computer mouse is better than 2 hours struggling with a soldering iron and other assembly tools. Make footprints that make your assembly (and the rest of your job) easier. It is worth it.

Why not submit two versions one trimmed and the other not, and report back what happened? I am curious and others probably too.

Trying this, I see that the Gerber plots have the pads outside the edge cuts outline. This means that the fab has to either remove the pads manually, waste PCB material with a bigger board on a shared sheet or end up with your pads falling onto someone elses job

I was trying to politely ignore these, but the “Just make footprins” comments are totally missing thew point and I’d appreciate if people could refrain.
I was fairly clear in my first post about this being more about learning KiCads potential than about making a footprint.

I’m well aware making footprints are an essential skill for using KiCad and am also well aware of noobs posting looking for ways around it.

I made it clear that this was not one of those posts.

Additionally there would be no struggle with tools, it is the same component, exactly.
The board is being fit to one half of a rotary switch being secured in a confined space.

Not trying to single you out BobZ, this post id for everyone that missed the point.

1 Like

You think you only asked 2 questions but you actually asked 3, the first one being in the title. That’s why you got some of the responses you did.

I thought I was pretty clear of what i was asking.

Point 2 specifically should have stopped “Just make a footprint comments”
How much clearer can i be than…


The problem is you suggested there might be three possible courses of action by you:

  1. Submit as is and hope JLC ignores it.

  2. Some way to restrict the plot output.

  3. Some way to mark the pads as to ignore.

Some answers were saying don’t do 1 but didn’t have answers for 2 or 3.

How you phrase the sentences affects the responses. For example in phone and other automated instructions it’s recommended to put the imperative last. Hence Google Maps says: In 100 metres turn left, not Turn left in 100 metres, because the second half might be missed or be heard too late.

Coming back to your query, I would reorder it like this:

I would like to do 2 or 3. The reason is if I do 1, JLC might mess up. I’m willing to make my own footprint to avoid this but I’d much prefer to prevent this with 2 or 3. Is there a way in pcbnew?

1 Like

Even the rephrasing of the questions may not solve the communication problems.

This is an internet forum dealing with a specialised subject and the OP is interested in:

Obviously, reading through the early replies, there is nothing clever to learn. Alternative solutions then appear so the postings skew towards those solutions.

It is the nature of the beast.

It would be nice to get a warning that the Gerber plots have important layers which have plotting outside of the edge cuts.

Cropping it automatically could have unfortunate consequences for those who use edge cuts to indicate scoring points.

The goal of the manufacturing files is to leave nothing to guesswork. The low cost fabs are not going to spend money phoning you or time on ignoring stray pads

My first approach would be to Edit the footprint (you have two choices: 1) the :Library one, 2) the one Placed on the PCB (thus, avoiding the Library one).

Second approach: With a TextEditor, edit the Gerber file and Delete the Pads/Holes/Mask/etc… take care; be sure to check the Pad/Net labels to avoid deleting the wrong ones.

Screenshot shows edit example…

Locating the Pads

Deleted the Pads/holes

1 Like

This is a perfectly neat little trick.

The need has passed now but I’m going to practice it anyway.

Thanks for sharing!

Just to finish-up by completing the Second Approach (editing the Placed Footprint)

Double-Clicked it, Edit_Footprint (NOT the Library Footprint)
Select and deleted the Three Pads hanging off the board.

Exported Gerber and shown in Gerber Viewer… The whole process to about 15 seconds…


Results In Gerber-Viewer

1 Like

For me, it’s just to obvious to edit the footprint itself for this:

  1. Select it.
  2. Press [Ctrl + e] to load it in the footprint editor.
  3. Delete the parts that stick out of the PCB.
  4. Close the footprint editor (It then asks you if it replace the modified footprint on the PCB, select OK.
  5. For neatness, you can put it in a project specific library, and then also update the link in the schematic symbol.
1 Like