Skip to main content

New layer for non plated through holes



  • Michael Harvey

    Hope I can help. I assume a non plated hole will become a screw mount hole. My screw mounts are plated and connected to common Ground with a top and bottom Cu greater than the screw head. However you can try the following to make a hole.

    Create a Component for your hole and include it in the schematic. (1) create Schematic Symbol to show the mounting hole, (say a circle with a cross in it) (2) create a PCB Symbol <new Item>, add a pad (important, use the THU pad, not the SMD pad. ie, the one that looks like a donut). (3) in Design Technology add a new pad style for your hole, Round  6mm, hole size 6mm, not plated. It will warn you that the drill removes the plate, of course. (4) change the style of the pad to the new style just created. (5) make the component. The every time you want a hole, just add another component in the schematic and the holes will be same size. It looks OK in 3D. It is part of .DRL file and it will not need an extra manufacturing layer.

    Another way to make a hole is instructing the final routing in the manufacturing of the board outline. When in PCB view, <add><board><circle>. or <add><board><square>. It is a little hard to control the size every time for many holes. As mentioned above, my mounting holes are plated with top and bottom pads and are grounded in the design and I just add then as a component. This controls the size ever time and does not freak out the PCB manufacturing (they do not have warn that the second drilling is drilling out the plate).


  • Kevin Craske

    Thank you for your suggestions. I have created a component as you suggest but have hit a problem. My PCB fabrication house requires non plated through holes to be on a different layer as from what I understand, this allows them to identify which ones not to plate.

    I have created a new layer, I think, but cannot get the new component to go to that layer. It does not give me the option to change layers as usual. My new layer also does not seem to be available on any component.


    On this one I think I will just allow the holes to be plated and dive deeper into technology files and how layers interact with components and layout.

  • Boss .

    A similar discussion came up a month ago.

    Look at Jayx's comment and link which are useful to understand the issues.

    I'm not aware of a way to define by layers, could this be a language/translation issue and they just want separate drill files (which are generated when producing the plots)?

    Can you share the manufacturer's URL so their requirements can be examined?

  • Kevin Craske

    Thanks for the link. I must say I am surprised this has caused a problem. I would have thought it was a common requirement.
    Interestingly I downloaded a footprint from the RS web site for a component not in the library and it has a location peg so a corresponding hole is specified. The pad width is smaller than the drill size so there is no pad, however it looks like the hole will be plated.
    Interesting point about losing things in translation. The fabrication is being done by JLCPCB and I must say they do answer emails quickly. It's probably my shaky knowledge which is causing the problem. I will continue trying things.
    Something I have noticed. I created a new layer, NPTH, and tried to place my 'hole' on it. However, the layer was not given as an option on the change layer menu. On inspection of layers in the technology menu, the new layer was not ticked and I could not tick it.Just by luck I added a line and went to change it's layer and found my new layer available. I put this line on it and hey, I was then able to now change layer for my 'hole' to my NTHP layer.
    I have learnt a lot by just trying and trying again. So far it seems that I have produced a drill file which includes all holes and a drill file which includes just plated through holes. Not succeed in generating a file which has non plated through holes only.
    It would be good to produce some really good PCBs as this project, for me, is big, about 2250 sq cm across 7 boards.

  • Boss .

    Some further thoughts...
    As there may be some confusion between the words layer and plots, you could try submitting separate drill files for plated and unplated.

    In the Plot outputs change the current plot to plated only.


    Now use Add Plot and set up for unplated as shown below. For the layer you need to select Through Hole.

    When you produce the Gerbers there will be two separate drill files with plated and unplated separated as shown. (In the Gerber Viewer they are referred to as "Layers"!).


    This is my best guess as to what is required.
    If you try this let us know the result.

  • Kevin Craske

    Thankyou for the suggestions, the problem solved.


    A matter of not understanding completely about generating the Gerber files, never having wanted non-plated through holes as a bit lost in translation with JLCPCB support. I must say, JLCPCB have been helpful.


    My solution for a hole, not plated through and no pad.

    1  Add a pad

    2  Change the properties hole size to the size I want the hole, make the pad width less than the hole size. Ignore the warning. Untick plated through

    3  When generating Gerber file, chose options - NC Drill - tick separate files for plated and unplated holes

    4  Rename files produced according to the requirements of JLCPCB

    It was reading others comments which led me to this. My boards are now being produced.



Please sign in to leave a comment.