If you're asking about using that term as a specification on a drawing, the answer is that it's usually discouraged. According to the ASME Y14.5 standard:
"The drawing should define a part without specifying manufacturing methods. Thus, only the diameter of a hole is given without indicating whether it is to be drilled, reamed, punched, or made by another operation. However, in those instances where manufacturing, processing, quality assurance, or environmental information is essential to the definition of engineering requirements, the information shall be specified on the drawing or in a document referenced on the drawing."
That's paragraph 4.1(e) of the 2018 edition.
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
This standard covers Nomenclature, Definitions, Sizes and Tolerances of High Speed Steel, Straight and Taper Shank Drills, Combined Drills and Countersinks, Plain Bell Type, In Both Inch and Metric Sizes
3DDave, Thank you for commenting. I was hoping someone would because I have seen this type of call out as well......a long time ago. I had some old SAE standard in my head as a possibility but ANSI 1979 sounds like the right time frame. I though "drill" had a specific definition as well as an associated set of tolerances but that was too many bourbons ago to accurately recall. I agree with the rest of posters, that I have not seen this callout used on any "modern" design drawings, that said, I am always surprised to find certain legacy industries that still may use very dated / old school terminology in certain settings.
I am QC not engineering. We have a couple of young engineers that are using 'Drill' and then put a +/-.002 tolerance. I thought Drill had been removed by ASME at some point, obviously not from your comments. I will have to impress upon them that if they want a hole give a diameter plus the tolerance.
"DRILL" is most likely used by either those from old schools or those who did not get trainings. +/-.002 can be too tight depending on size of the hole.
The correct way to choose tolerances for machined holes is to look it up in The Machinery Handbook or ANSI Standard Tolerances (ANSI B4.1-R1987). It is called "IT grade". If you drill a hole of dia. 1", you won't be able to achieve +/-.002". Alternatively, you do a capability study on economical precision.
You need to specify tolerances to meet your needs and leave machining methods to specialists.
Also, if a fraction size drill (ie 5/16) a fraction tolerance needs to be called out somewhere. Otherwise the machinists could use the same drill bit, wearing in diameter over time.
From my experience.
Your +0/-.002 tolerance is potentially fun. Drills make oversized holes. Machinists know this, and it is documented in the Machinery's handbook. They can do all sorts of jiggerypockey with pilot drills and such. All the more reason to nownot say "DRILL" on the drawing.
The table in Machinery's handbook was from tests on iron, I think. If done properly one can get undersized holes in metals with large coefficients of expansion; one can even take a dia 0.250 bit and make a 0.125 hole in a rubber sheet. If diameter is important then don't depend on a drill bit.
"Drill" goes on a factory floor process sheet to tell the shop floor worker what to do, as the sample image above is for. That allows the correct allocation of planned time and resources. Otherwise you get workers as a QA buddy of mine discovered, RIP Hank, on the factory floor, using a reamer to make a hole because the drawing had a small tolerance. Not often, as he put it, does one see a reamer glowing dull red.
