How to make NPTH with larger solder mask area?

Hi KiCaders,
Sorry if I got the terminology wrong. I’m trying to make a Tooling Hole that is specified by my PCB manufacturer (JLC).

They say “Tooling holes should be 1.152mm(45.4mil) round non-plated holes with 0.148mm solder mask expansion.”.

I have no problem with the 1.152 round non-plated hole - easy. But I don’t know how to do the .148 solder mask expansion. When I create the pad in kicad, I can put the drill dimension to 1.152 and it will make the solder mask 1.152 as well. If I try to enlarge the solder mask to 1.3mm by setting the hole size to 1.3mm it works, but also puts copper on the pad (just not inside the hole according to the 3D preview).

So if I set Copper to “none” in the pad properties, I get an error message saying:

Error: the pad is not on a copper layer and has a hole
For NPTH pad, set pad size value to pad drill value, if you do not want this pad plotted in gerber files

It’s too bad, because it looks like those settings SHOULD give me the hole I want.

A little work-around that worked:

Make the NPTH as 1.152mm hole and pad. Then manually add a filled circle on each soldermask layer that is 1.3mm diameter… which in itself requires a bit of a workaround of making a non-filled circle as 0.325mm radius and .65mm thickness.

Have you tried to set “Solder mask clearance” in “Local Clearance and Settings” in your “Pad Properties”?

This setting is one of the three tabs on top of the pad properties window:
image

About your workaround…
I think you manually drew a circle (Footprint Editor / Place / Circle) on the F.mask layer? This probably works, but it’s a bit neater to use a pad for this, then set the Pad Type to SMD Apaerture and disable all layers except the F.Mask layer.


In a more general sense, I wonder what this “Tooling hole” is used for, and why it is such a specific diameter.
It is common to use registering holes to locate the PCB into the machines to get Drilling / etching / Soldermask and Silksrceen to line up on the PCB, but that is an internal thing for the PCB manufacturer, and such holes also have to have very specific locations so the panel fits in their machines.
If you use these “tooling holes” for yourself, then your PCB manufacturer does not care about what size they are.

So it probably is something else, but I don’t know what but am curious. Can you tell me where it is on the JLC website and what you want to use if for?

Thanks Piotr, this worked - I’ve never even looked at the “Local Clearance and Settings” tab before!

Thank you paulvdh,
Sorry I meant to include the link to JLC’s website: https://support.jlcpcb.com/article/92-how-to-add-tooling-holes-for-smt-assembly-order

They say it is only for SMT assembly. I’d guess it serves a similar purpose to a Fiducial, but the name “tooling hole” makes me think it is for something mechanical (like physical alignment) and not optical. It would also make a bad Fiducial because it gives no information about the actual alignment of the copper but I have no idea…

The previous orders I’ve done, JLC has manually placed these holes but I’m trying to make my design as easy to manufacture as possible.

I suppose these are needed only if the board is not panelized. If it’s panelized the holes would be added to the panel margin.

Thanks for the link.
I’m still guessing but it does make sense to have such holes for mechanical alignment for paste and SMT placement for PCB’s that are not part of a panel.

My first guess was that your need is similar to fiducials so I have checked how solder mask expansion is made in fiducials.
I supposed that you never seen fiducials so you can’t know that they are similar and so your question.
Even I order PCBs since 30+ years I first time heard about fiducials 3 years ago. Our contract manufacturer never asked for them. I suppose that he just added them making panel of our PCBs.

The video below shows quite clearly one of the ways these holes can be used during stencil printing.

And a still picture in case the video gets removed at some time in the future:

image

Note that there are levers with a long slot and a “pin” at the end. During mounting the PCB is first placed on the pins and then the “levers” are screwed to the mounting plate to fix the position of the pins.

I do not know if JLC uses manual labor as shown int he above video for small series.

“Solder paste jet printers” are becoming more common:
https://www.youtube.com/results?search_query=solder+paste+jet+printer

These can print over a million dots per hour but are still slower then working with a solder paste stencil.
Advantages of such machines are that no solder paste stencil is needed at all, which reduces costs for manufacturing / storage / setup times. On top of that the high degree of automation reduces human labor and they may be more reliable than stencil printers too. These machines have integrated AOI (Automated Optical Inspection) to check if the thing works at all, and also to correct the size of the dispensed solder dot (may change with temperature, viscosity of the paste etc).
This (<3min) video is a nice overview of how such a machine works.