1.5 mm hole in PCB

I’m am trying to make a 1.5mm hole to push a battery clip wire through to act as strain relief on my PCB but it never comes out as a simple clean drilled hole at that size and I do select NPTH, I just want a drilled hole on there I have tried using mounting holes but I still get a metal ring round it at 1.5mm any thoughts please ?


NPTH (Non PlaTed Hole) only specifies the inside of the hole itself.

If you: Pcbnew / File / Plot / Plot format: [Gerber] / [Generate Drill Files … then it should make two files. One for the plated holes, and one for the non plated holes.

If you have a ring of copper on the surface of the PCB that you do not want, then you have to edit the properties of the pads.
Set the “Pad type” to “NPTH, Mechanical”, and set the “Copper:” to “None”.

And to verify that these settings are correct, you can look at your Pcb in Pcbnew / 3D Viewer [Alt + 3] and then: 3D Viewer / Preferences / Display Options and then unselect the options for [ ] Show board body and [ ] Show solder mask layers. This makes your PCB mostly transparent so you can view what’s inside as in the screenshot below.

The final thing however is to inspect the Gerber files themselves. Those are what is sent to a PCB manufacturer and what they make.

1 Like

Hmm? I have specified a mounting hole without connections symbol in eeschema and assigned it a plain mounting hole footprint in a project and it was definitely manufactured without any pad or plating, just drilled. Only problem for you is the smallest one in the library is 2.1 mm. But you can probably see how it’s done in the library and make your own.

1 Like

I had a quick look at the pad properties of MountingHole / MountingHole_2.1mm and to my surprise the copper layers were set to [ All copper layers ].

Pad size is set to circular with the same diameter as the drill, and I was a bit concerned this may produce thin slivers of copper during manufacturing (Because of tolerances). So I put it on a PCB and made a set of Gerber files. Those holes did not have anything on the copper layers, so they look all right.


You can make holes on the PCB by drawing them on the Edge_Cuts layer. They’re just Holes (or other desired shapes)… That’s how you make Cutouts/etc on the PCB and Holes are often/usually, not listed in Netlist or BOM…


Holes, slots etc in Edge_Cuts are intended to be routed out.
A 1.5mm hole is far too small to route out and should be drilled as a NPTH.
Many Fabs treat routing as an extra cost step


If you set 'copper ’ to none you get an error saying that its not on a copper layer however my mistake was to not adjust the " Size X " to 1.5mm as well as “hole size X” now I have this set the hole appears normally as I wanted, not sure why but thanks for your help


It seems in the case of a smaller pad you must set ‘hole size X’ and 'Size x ’ to the same value and I didn’t notice this ! thanks for your help.


Won’t argue the point of

But, I, and many others Mill and Drill our own PCB’s thus, we can (and do) put whatever we want on the layer that makes sense for the project at hand. As a business, I’ve farmed out Multi-Layer jobs that were milled and drilled (I don’t make my own multi-layer boards).

I generally put NPTH holes on the Edge_Cuts layer and Route them with the same 1.5mm End-Mill Bit that I use for routing the board’s shape. Sometimes I use them as a Drill-Bit…

JLCPCB specifies the smallest Hole for NPTH as 0.50mm and to be put on the Mechanical Layer (i.e., the Edge-Cuts layer).

They also specify the minimum Drill-Hole size of 0.20mm

If you think about it, why might they specify Two different minimum hole sizes (one for Drills and one for Mechanical (meaning, to be routed)? Obviously they intend to Route the 0.5mm hole and Drill the 0.20mm.

Additionally, they spec minimum Non-Plated Slot dim’s of 1.0mm on Mechanical layer, thus, they must be using a small mill-bit. They do not charge extra for this (small drilling/routing).

Images below from JLCPCB

Plenty of coffee, free time and a rainy morning inspired me to demonstrate on a low-cost 3018-Pro mill. It’s useful for PCB’s and other light projects… It does almost as well on light-weight projects as does my real mill and was $100 versus the Thousands I spent on the real one…

Naturally, a PCB fab-house wants to make money but, most can (and will) do holes and slots of reasonable small size without extra cost - depends on details but, you get the idea and, all you need do is design, get it quoted and ask questions…

The example Demos Making ‘Holes And Slots’:

• Used scrap PCB (just crammed in what you see)
• Did not bother to Flip the board when generating Gcode so, Text is backwards
• Used a 0.7mm End-Mill Bit for the Holes, Slots and Contour
• Routing - No Drilling or Drill-Bits used
• Did not bother to finish the PCB contour

Hole Diam’s and Slot Width’s: 1.5mm, 1.0mm, 0.8mm

Photo on 8-21-21 at 1.18 PM

Useful stuff…cheers.

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