Finished hole versus drill-bit


an old topic but needs to be discussed

some people say manufacturers always interpret the hole sizes as finished holes.
historically i doubt this, the old drill mapping file was to map drills, the size of the drill bit

yes it makes sense to speak in terms of finished hole, but kicad footprint editor clearly states drill size

so if now its finished hole that is industry standard maybe it should say so in the footprint editor.
also i dont know if this info finished versus drill size interpretation is included in the actual drill manufacturing output.


That would be meta information about the project which the current gerber files (the industry standard) not contain - esp not for hobbyist projects. You’re essentially looking over the rim of an old big can of worms there…




kicad should have a radio-button for each pad, finished or drill
even if not supported it can support it later and not all footprints needs to be revised for what compromise was done at the moment


Yes, it is a very old topic. The only thing this thread adds to the discussion is the fact that KiCAD uses the term “Drill” in its dialogs, instead of “Hole”. In my mind, asking for a wording change from “Drill” to “Hole” is a valid bug report. Is this problem present when the dialogs are rendered in other languages, or mainly just in English?

"The overwhelming majority of fabricators expect you to specify the FINISHED size of the hole. The last time I encountered a fabricator who wanted the drill size was at least 15 years ago (perhaps 20). From the perspective of manufacturing philosophy it should be no other way. You, as board designer, have a requirement to create a certain hole size. But you have no knowledge of the processes used by the fabricator to create plated-through holes, much less any control over them. The fabricator will do the initial drilling, pre-plating, plating, and after-plate finishing. If he has these processes under control he can reliably predict the finished hole size much better than you can guess the outcome. A fabricator who tells you to specify the initial drill size is saying, in effect, that he is not using well-controlled processes. "

I wrote that in the thread at Footprint Editor: Enter Final Hole Dia or Drill Dia? . To date, I see no reason to alter or modify that statement. The mapping of initial hole size to finished hole size may vary from fabricator to fabricator. The formula can vary when you ask for copper of a different “weight”. And then there’s the question of mechanical twist drills versus laser-drilling, or other exotic manufacturing techniques that may appear in the future. Tell the fabricator that you want to buy a hole of a certain size, and let him figure out how to accomplish that.

Another thread where I discussed this topic is at Finished hole sizes after plating: how does the calculation work?




but wording in kicad should change then and not be misleading.

i agree with your opinion about the manufacturing.

sometimes when it comes to press-fit its pretty well defined with drillsizes and platings, but then again board will have to be made in some form if standard process anyway so…

conclusion, kicad should change text from drill to finished hole

i file a bug


“ODB++” is irrelevant to this discussion. Whether the fabrication information is passed via ODB++, or Gerber, or Excellon, or Postscript, or DXF, or tape on mylar, specifying a finished hole size is still specifying a finished hole size.

I won’t get into an argument over whether ODB++ is an improvement over the Gerber/Excellon combination. I don’t think it is; since the format has been around for at least 20 years (maybe 30?) but is used by only a small percentage of designers, my professional peers seem to agree with me.



Well, in my view, for through-hole components the inner barrel diameter (i.e. finished diameter) shall be defined (reason: pin should fit into the hole with proper gap). But for vias the outer barrel diameter (i.e. drill diameter) shall be defined (reason: clearance to planes, skin effect, vias may be resin- or copper-filled)


One of our manufacturers told us footprint holes have a 10% tolerance (even in the same board). Usually the have drills with 0.05 mm steps.

It was discussed before with a great explanation from Dale. It is worth it to read his whole post…