FEDEVEL
Platform forum

ElectronHerder , 03-08-2025, 06:48 PM

What is the proper way to create a NPTH with a pad? The component is an SMT threaded standoff (Wurth part number 9774030360R). The suggested land pattern is a non-plated hole with a pad. Is this as simple as creating a pad in Altium that is a normal through-hole pad with the "Plated" check box unchecked?

I will be using JLCPCB to manufacture the board. In their list of capabilities on the website, I found two specifications I would appreciate help in understanding.

The first is in the drilling section. The feature is "Min. Non-plated holes", and the description reads "Please draw NPTHs in the mechanical layer or keep out layer". Does this mean the hole should be placed in a mechanical layer or keep out layer instead of Multi-Layer? I have made boards in the past that have NPTHs, and I have drawn them in the Mult-Layer layer and not had any issues. Is Multi-Layer the correct layer, but what they mean is they would simply appreciate the NPTHs to be documented in a mechanical layer? Is it good or bad practice to create two Excellon drill files, one for PTH, and the other for NPTH?

The second specification is in the Traces section. The feature is "NPTH pad annular ring", and the description reads "Recommended 0.45 mm or more. This is to allow a 0.2 mm ring of copper to be removed around the hole for the sealing film to attach. Pad sizes smaller than the recommended value can result in the annular ring being very thin or completely missing". Am I correct in assuming I do not need to remove the 0.2 mm ring because they will remove it when preparing the files for manufacturing? There is one other related feature they list, which is "NPTH to Track", and the minimum value is 0.2 mm. Fortunately, this value correlates with the "NPTH pad annular ring" requirement, and I don't have a question about it. I just thought it would be worth mentioning for completeness, and that it matches the other specification.

Thank you very much for the help.

QDrives , 03-08-2025, 08:18 PM

"*Is this as simple as creating a pad in Altium that is a normal through-hole pad with the "Plated" check box unchecked?*" -- Yes.
"*Does this mean the hole should be placed in a mechanical layer or keep out layer instead of Multi-Layer?*" -- No. If they do not understand how production data works, it is their fault.
"*Is it good or bad practice to create two Excellon drill files, one for PTH, and the other for NPTH?*" -- Altium does that automatically.
"*NPTH pad annular ring*" -- I see that JLCPCB is a master is making and writing things difficult/wrong. If I look at their picture, the annular ring would need to be 0.65mm, unless you use the donut pad design. I assume they drill all holes and then cover the NPTH holes before the PTH holes get plated. After plating, they remove the cover again, but also remove 0.2m from the copper. What they should do is drill the NPTH after plating.

ElectronHerder , 03-09-2025, 06:49 AM

Thanks QDrives! Good point that the annular ring should drawn as 0.65mm from the edge of the hole. But I suppose if they drew it that way, it would confuse people as to why they didn't draw it from copper edge to copper edge. I agree with everything you said except for maybe the last part about drilling the NPTH after plating. Isn't it risky to drill a pad after it has been etched? It seems the drill could potentially tear the pad off?

QDrives , 03-09-2025, 04:22 PM

That is why I state after "plating", not after etching.
https://www.eurocircuits.com/tips-tricks/understanding-annular-rings/

ElectronHerder , 03-11-2025, 12:31 AM

Thanks for the link. I see what you mean. The drilling is performed before etching. Maybe the issue is debris from the drilling process that isn't easily removed before etching? Maybe high-end manufacturers would do that, but JLCPCB keeps their prices lower with a sub-standard result? Actually, I don't think it is substandard, since I can't think of a reason it is critical to get the pad that close to a non-plated hole. Which leads me to another question...

I'm attaching a screenshot of JLCPCB's tolerances for plated vs. non-plated holes. I suspect the non-plated tolerance is largely dependent on the drill sizes they have available. If a diameter is specified that they have the exact size drill for, then the tolerance is probably pretty good. Likely a little larger than specified due to drill wander, or I suppose a little smaller if the drill is near end of life and has worn down come. Does that make sense? The component I'm designing for is an SMT standoff. Why wouldn't a plated hole be desired over a non-plated hole, assuming the tolerance is good enough? I don't mind if some solder goes down the barrel. It seems that would be better for mechanical strength. Is it because plated holes might not be clean from top to bottom, which could impede the pick-and-place machine from placing the part sometimes?

QDrives , 03-11-2025, 07:32 PM

The tolerance for PTH is due to the drill size (lets say in 0.1mm step size) and the plating.
However, why the NPTH would have a bigger tolerance, I do not know.
I never order at JLCPCB.

As for the stand-of, I also do not know exactlt why it would be NPTH.
I can assume that they do not want a Pin-In-Paste method, but Altium can do donut shape for the solder.
Or if you do it even better, add the intersection for the webbing too.