PTH vs NPTH Drill files

I’ve seen plenty of posts about PTH an NPTH but none seem to explain what I would like to know.

Simple, single sided PCB. As far as I am aware all of the footprints have been created as single sided (B.Cu), with bottom solder mask (B.mask), and top silkscreen (F.silkS), but when I generate the drill files I get NPTH for mounting holes and PTH for all of the components.

The PCB design itself consists of only these 3 layers (and edge cuts obviously), and since I have control of the Gerber layers produced these are the layers that I generate in the gerbers.

I’m clearly missing something. How do I persuade the tool to generate an NPTH drill file only, or a NPTH and empty PTH drill file.

I know the PCB manufacturer will adjust the design, within limits, to suit their tools, process and IPC requirements, but I would like to send files that describe what I want in the first place.

THT footprints have pads on front and back Cu layers.

2 layer is the basic offering these days. Is there a reason you want 1 layer only? I suppose you could route only on B.Cu, not submit F.Cu, then you’d have the PTHs left.

1 Like

I just checked a PCB designed by a.n.other and sold as part of a self assembly kit. It’s exactly as I would like my design to be - NPTH component holes, copper and solder mask on the bottom and a silkscreen on the top. The unplated FR4 is clearly visible in the unpopulated footprint holes.

Just talk to your board manufacturer.
If you tell them you only want a single-sided board, and no PTH, then (if they are willing to do that), they can work with the existing Gerbers and drill files.

But, unless you really, really need to do this - it’s a bad idea. leaving out the through-hole plating makes the board much more likely to fail, and, especially for a kit aimed at a novice, makes it much more likely that they will ruin the board.

If you really want that you have to create your own special footprints (in the footprint library editor) with NPTH-holes.
This will result in very special footprints, you have to combine:

  • a central NPTH-pad, with no copper, but bottom mask layer (this is the hole)
  • a small bottom smd-pad (which gets the pad-number), which is located a little bit outside the NPTH pad
  • a filled circle at bottom.copper with the desired pad-diameter, located at the same position as the NPTH pad
  • the small smd-pad and the copper circle must be combined (CTRL+E) to a custom pad shape
    in the board-constraints the copper-hole clearance must be set to zero

Out of curiosity a made the following example: (44.0 KB)

look at J4 in the footprint-editor to examine how the pads are being made.
If you create gerber+drill files you will see the drills for J4 in the NPTH-file.

Nonetheless I second the above statements:

  • talk to the board house
  • 2-layer-pcb with THT-pads is mechanically more robust

If you want a panel with copper only on one side, all holes are NPTH. Are you going to buy a whole panel?

If your PCB producer is so old fashioned that they still do single sided PCB’s, then plating holes also does not make much sense at all.

But KiCad has: PCB Editor / File / Fabrication Outputs / Drill Files / PTH and NPTH in a single file:

@paulvdh :
I tested this option (as I also thought this would be useful) but it is (most probably) no solution for the OP.
This option creates only one drill-file, but inside this drill-file there are still two different sections clearly separated as PTH/NPTH holes.

I think it is not needed.
If during PCB manufacture the process of plating holes is skipped (and if one sided PCB is the task I suppose it is skipped) than all holes will be NPTH even they were done based on PTH holes file.

If you will order single sided PCB and less than 10m² I expect manufacturer will just use his 2 sided workflow with etching one side (using empty gerber for tracks at this side).
I suppose that nowadays for the same cost you could get 2 sided PCB.

Much, much more robust.
35 years ago because of costs we used in some product one sided PCB. Then we found that if terminal block was not 100% pushed to PCB during soldering (not its plastic case but internal metal structure) then when you later used screwdriver to fix wire in terminal block the bottom side track were broken (not by rotation but by pressure). We changed those PCBs to 2-sided and all problems gone.

I’m not so sure about that. single layer PCB’s are quite unusual these days (Mostly FR2 in huge production volumes of cheap PCB’s ). Having all holes in a single file may have a small advantage, if his PCB manufacturer ignores the PTH versus NPTH attributes. My crystal ball is out for maintenance and I thought it useful to mention the option.

Thanks for the pointers.

In the end I created a project specific footprint library starting with standard library footprints and edited them to suit my needs. End result was a NPTH drill file and and empty PTH drill file.

Just exactly what the doctor ordered

The high volume truly single sided boards are punched, not drilled and use paper-resin material
As others have said above, they are obsolete