Zum Hauptinhalt gehen

Creating a hole in the pcb with no via (no copper feed-through) and no copper pad?

Kommentare

11 Kommentare

  • Boss .

    It should show up in the drill file, mine have always been drilled correctly either with copper and plating or without.

    I suggest checking the component in the library to be sure and compare with just adding a pad of the required hole size and without copper which is what I normally do or what I now do is add it to the pad styles with a description such as" M4 clearance".

    In the 'manufacturing outputs', check the settings used as you can exclude or not select non-plated holes.

    For the board outline, as a separate Gerber layer I do not know if that will be a problem.
    If the hole was produced as a circular board outline (within the actual board) it should not be an issue, I have successfully used this method for slots. There is probably a minimum hole size they will mill and revert to a drill, so if the manufacturer missed this and needed to manually add the hole to the drill file that may explain this.
    I can't think of a way of adding a drill hole to the board outline, if you have perhaps that is the issue?

    0
  • John Wright

    Thanks Boss,

     

    Bottom line...it worked!

    I checked the component in the Library.

    It did NOT contain the pads I needed.

    So, I added the pads as non-plated holes.

    They did NOT show up in the drill file.

    I changed them to plated and they suddenly showed up in the drill file.

    So, I changed them back to non-plated and then selected non-plated holes in the setup as you indicated.

    They then showed up in the drill file.

    I selected same drill file for plated and non-plated holes.

    I need to ask my vendor whether they want 2 different files.

    Regardless of that...it worked!

     

    Thanks again!!!! Woohoo!

    John

    P.S. You da boss!

    2
  • Boss .

    Excellent, pleased to have helped.

    The reason for two drill files is :-
    the unplated holes are drilled with the closest drill to the requested hole size.

    the plated holes are drilled oversize to allow for a reduction due to the plating thickness.

    I must now look up what in the Gerber files actually defines for the manufacturer a hole as being plated!
    Always something else to learn

    0
  • John Wright

    Interesting.

    I wondered whether they drilled the plated holes before or after putting in the copper. It makes sense they would drill before. Then they don't risk taking out all the copper they just put on. Drilling is probably not accurate enough to guarantee the remaining thickness of copper (if they were to drill after).

    John

    0
  • Boss .

    My understanding is they expose the PCB with all the holes filled (blacked out) and etch the copper.

    Next they drill the holes oversize and then plate, so the final hole size is determined by their process plating time.

    I am guessing they must then have to drill the unplated holes, hence why there are two drill files.

    0
  • John Wright

    I guess there must be some board vendors that call for 2 drill files, otherwise you guys would not have ever added that option.

    It turns out my vendor wants both plated and un-plated in the same drill file...sure makes my like easier...alleviates the chance to forget sending a file. It helps, for my design, that all plated holes are a different size than all non-plated holes...that could get pretty confusing.

    0
  • Jayx .

    As far as I know, technically there is nothing in Gerber to indicate if the hole should be plated or not. The same for a drill file. That's one of the limitation of the legacy format and the reason most PCB manufacturers require two separate files for plated and non-plated holes.

    If there is just one file, they need to do an "educated guess", here is nice explanation from Eurocircuits, but other manufacturers may have a different rules: https://www.eurocircuits.com/pcb-design-guidelines-drilled-holes/

    1
  • DesignSpark PCB

    @Jayx, thank you for the link to a good description of how this is handled in manufacturing.

    0
  • John Wright

    My vendor recommends sending drill data in Excellon format. I would guess that this format includes information indicating whether it's plated or not, but I don't know for sure.

     

    0
  • Jayx .

    Unfortunatelly not. Excellon is very old and simple file, originally used to directly drive Excellon drilling machines. Contains only drill bit size and coordinates, nothing else.

    0
  • John Wright

    Thanks Jayx,

     

    In that case, I'm glad I placed a note identifying all non-plated holes and stating the drill bit size and tolerance for them.

     

    John

    0

Bitte melden Sie sich an, um einen Kommentar zu hinterlassen.