Plated Slots for JLC PCB

I have created a PCB with Kicad 7.0 with plated slots for toggle switches and barell jacks and send this for production to JLCPCB. The slots were visible both in Drill file (DRL) and the DrillMap file (GBR).
The board came back with the plated slots missing from the PCB. :unamused: So I have the exposed copper on top and bottom, but there is no hole or slot.

Has anybody here succeded in using plated slots with JLC PCB?

From my understanding the tiny PCB drills can only go down and back up in a PCB and will break if moved sideways while in PCB.
For milling I would consider separate tool. But according to drill map KiCad combines drills and mills into one tool.

Talk Bot from JLCPCB suggested “you could design the plate or copper in necessary layer
but the slots need in the same layer with the board outline in case any missing.”
For me putting plated slots in the PCB-Outline layer doesn’t sound sensible, because this data is used to separate the PCB from the big panel after production which is always done as non plated.

Any feedback appreciated!
Best regards

11_dim.GBR (2.0 KB)
14_pth.DRL (2.2 KB)
14_pth.GBR (128.4 KB)


I have no experience trying to order plated slots with them, but according to their documentation you should create these as a through-hole pad with an “elongated” hole.

That’s probably why the minimum plated slot width at JLCPCB is 0.5mm, so they can use a larger, more robust drill for that. Otherwise I don’t think you have to worry about that.

Agreed. That definitely doesn’t make sense for such holes in pads.

You should probably e-mail them. It’s possible that they simply made a mistake. Usually they’re pretty nice and responsive.

They have a button “Confirm Production file” under “High Spec Options” :woozy_face: I will try this for the next order with an entry under PCB remark.

Maybe that will help.

Best regards

1 Like

When generating Fab-data there is an option in the “Generate Drill data” dialog that allows to select the Excellon mode for oval holes:
Default is to use the routing command. But there is an option to use an “alternative drilling mode”.
Has anybody tried this?

Yup . . .

From the 3D view . . .


. . . JLCPCB made them just like in the 3D view. They are just a oval pad with an oval hole. Nothing special.

1 Like

Again, I just would mail jlcpcb regarding your last order. It’s possible that they simply made a mistake loading your files and usually they have no problem with either explaining you what you did wrong or sending you fixed boards if they made the mistake.

Yessir! Oval pads and no problem ever.

My local PCB manufacturer said that some not typical things I can make in many ways. The key is to be clear what is my intention.
Since 90s for many years the oval slots we defined using the wide track (2mm wide track has round ends) at the separate layer and informed them that this layer is the milling map (from line width they know that we intend to use 2mm milling cutter). It was enough to get PCB as we wanted. Those time we used Protel 3 in which there is no difference between track and graphic line (it is while I said track).
Then (about 2010) I got info that instead of it I can do that oval with tracks (lines) at edge cut layer (little more work - 2 lines and 2 halves of a circle instead of one line). I have checked and it also worked. When moving to KiCad I got the possibility to use oval holes - the next way to specify this. Also works.

When I asked how to specify pads at PCB edge, like you can see here:

I was told that if my THT pad (with hole) will be cut by PCB edge than it is clear for them that I want to have plated edge pads.
So, what I understand from what you said that data at PCB-Oultine is not always used as not plated something is not always true.

For me putting plated slots in the PCB-Outline layer doesn’t sound sensible, because this data is used to separate the PCB from the big panel after production which is always done as non plated.

Agreed. That definitely doesn’t make sense for such holes in pads.

I have to disagree, this approach is also used by other pcb manufacturers. For instance multi-pcb and aetzwerk both treat " each milling with copper connections on TOP and BOTTOM will be plated" as plated slots (cited from their website). If the milling is put into a special layer or simple on the edge.cuts layer is not important.

I agree with your disagree.
For many years (when I had no oval holes in software) to get pad with oval hole I used to draw oval at PCB-Outline layer.

No problem getting jlcpcb to make slots for me either – just an oval pad with an oval hole. However, I add a note and arrow to the edge-cuts layer to point out slots and v-grooves. Probably annoys them as they need to tidy-up the edge-cut layer, but they have never missed one:

hi all,
many thanks for the support.

In the order preview everything looks good.

I have send out a new order with

  • Confirm Production file checked
  • and a remark “Board has Pads with PLATED SLOTS. PLS check DRILL file! 板上有带镀槽的焊盘! 请检查钻孔文件!”

Anybody with better Chinese than Google translate, please assist in a better translation :wink:

1 Like

No problems with producing slotted holes for a barrel jack at JLCPCB. I used the BarrelJack_Wuerth from library Connector_BarrelJack. If opening this and look at the pad properties you find Pad and hole shape set to Oval, pad size X 4mm, Y 1.8mm and hole size X 3mm, Y 0.8mm.

1 Like

Yes, I’ve had boards made at JLC containing oval pads with elongated holes before. I think I just used some of the footprints included with KiCad, e.g. barrel jacks, USB connectors, etc.

1 Like

I strongly suggest you use existing library footprints. I’ve had several pcb made by JLC using standard libs for pcb mount barrel connectors. This is a much easier path to success than creating unique footprints.

Today I received my order from JLCPCB! Plated slots arrived as designed in KiCad. I used the standard settings from KiCad, only used Protel file names. I thought they might be more familiar with them.
Pls note my previous post:

The board looks great:

A big :+1: :+1: :+1: to the KiCad team for this great software!


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