threaded hole depth feature of size?

[supergee]

Hi,

IF I OVER SIMPLIFY There are two approches to dimensioning : one for feature of size and the other on for the rest. Feature of size are feature with two opposed surfaces. hole depth, in that sence are not feature of size. direct tolerancing on the dimension is used on FOS dimensions. everty thing else is controled with geo tolerancing.

in the case of threaded blind holes, there are the thread depth and the tap drill depth. I could imagine using geometric tolerance for neither. I can't find a clear way in y14.5 2018 nor y14.6 2001 to show HOW to tolerance the said depths. can you help? I'm including 4 choices to tolerance the depths.

 

[3DDave]

It is pretty rare to try to tolerance the extent of threading because that normally is a function of the number or extent of full threads for which the typical concern is that there are enough of them, a minimum. There is less concern over the depth of the tap-drill diameter as the mating screw is assumed by convention to reach no further than the extent of the full threads. The tap drill diameter is only an artifact of the thread tapping process as is the presence of a conical feature at the bottom.

Were one to weld a fully threaded bushing to a flat plate, there would be no tap drill diameter or conical feature and only the number of full threads not affected by the weld would be of concern.

Is there a mechanism you are creating that requires a particular range to the angle of turns of full thread that you are controlling with the extent of full threads?

Normally the satisfaction of setting the max depth of the tap drill/the operation that creates the minor diameter, and the minimum amount of full threads is enough. Whatever overlap there is doesn't matter to the function of the threaded feature.

 

[Burunduk]

I guess you could use profile to avoid ambiguity but you'll be frowned upon for an "overkill". Y14.5 and most "GD&T" trainers don't want to be frowned upon but they don't want to show ambiguous examples either so they don't show any tolerances for hole depths, chamfers, etc. Y14.41 possibly had no choice.

 

[ctopher]

I call out the tap info, and leave tap drill size up to the machinist. Then, use basic rule of thumb that I have always used "basic rule: the tap drill depth should be at least one thread or one pitch beyond the chamfer of the tap".
If there is a clearance issue, then I call out drill depth.

 

[jassco]

Well, each feature shall be toleranced per ASME Y14.5-2018 section 4.1 (a).

Also, direct tolerancing on the dimension is NOT exclusively used on FOS dimensions.

4.1 FUNDAMENTAL RULES
Dimensioning and tolerancing shall clearly define engineering
intent and shall conform to the following:
(a) Each feature shall be toleranced. Tolerances may be
applied directly to size dimensions. Tolerances shall be
applied using feature control frames when feature definition
is basic. Tolerances may also be indicated by a note or
located in a supplementary block of the drawing format.
See ASME Y14.1 and ASME Y14.1M. Those dimensions
specifically identified as reference, maximum,
minimum, or stock (commercial stock size) do not
require the application of a tolerance.

 

[SDETERS]

For Example D I would put .380 Min full thread and put .599 Max This way the manufacturing can figure out their best approach.
I like to call thread depths out on sections, as in Example D. This way it is clear to the person using the print.
We do not call out the Tap drill. Unless there are other certain design considerations.

 

[supergee]

Thank you all for the replies!

@3DDave, I was preparing an example in what a good GD&T drawing should look for my students and, like @Bunrunduk said, I didn't want to overkill my dimensions but i don't like leaving things ambiguous: I first learned GD&T from experimenting with bad parts made from bad drawings.

@Bunrunduk, I like the 14.1 solution because if I see an inspector checking the form of the unthreaded portion of the hole, i'd fire them for waisting time and money.

@jassco, thanks for the quote. I am constantly fighting to make people understand that direct tolerancing is ambiguous that I removed that part from my brain.

for the others Steters and ctopher, I like your input. I'll communicate those to my students.

Gee

 

[Wuzhee]

It is imperative to know that in thread connections, the first 3-4 full turns take up 99% of the force applied. Additional turns henceforth are unneccessary.
For a usual threaded hole the minimum depth must take into account the length of the thread starting spiral then an additional few turns for bottom clearance.
Also pre-drill sizes vary in relation to tapping tool. A threading tap, a thread mill, a thread forming flute require different pilot holes.

I would advise against tolerancing thread depth and pilot depth. Minimum thread lenght is sufficient most of the time.

I have seen people overdo position on threaded holes with MMC callouts. If one can answer what is the advantage of this (and how you validate) I'm fully listening.

 

[3DDave]

With MMC one can justify the use of a solid precision thread gauge that is made to match the MMC of the tapped thread. Pretty easy to make.

With RFS, one should use a specialty gauge that can only touch where the pitch diameter is, but that will be a variable, so one needs a more expensive expanding gauge. The ones I've seen grind off the outer part of the thread down to where the pitch diameter is.

If there is a projected tolerance then the RFS gauge will likely need to have a special extension on it that still has access to cause the expansion to happen.

Functionally, just put a bolt in it and use that; for RFS use a nut to pull the bolt up and center it on the threads. It doesn't matter that it won't make contact with the pitch diameter.

It needs to be a good quality bolt, not a rolled-thread cheap grade for big-box-store bolt.

 

[Burunduk]

With MMC one can justify the use of a solid precision thread gauge that is made to match the MMC of the tapped thread. Pretty easy to make.

With RFS, one should use a specialty gauge that can only touch where the pitch diameter is, but that will be a variable, so one needs a more expensive expanding gauge. The ones I've seen grind off the outer part of the thread down to where the pitch diameter is.

If there is a projected tolerance then the RFS gauge will likely need to have a special extension on it that still has access to cause the expansion to happen.

Functionally, just put a bolt in it and use that; for RFS use a nut to pull the bolt up and center it on the threads. It doesn't matter that it won't make contact with the pitch diameter.

It needs to be a good quality bolt, not a rolled-thread cheap grade for big-box-store bolt.

Position at MMC for a threaded hole technically requires a virtual condition external threaded gage fixed at the true position. Gage size would be MMC of the internal thread's pitch dia. (unless the default was overriden by a note) minus the position tolerance. Resulting in an external thread of non standard dimensions on the gage.

 

[supergee]

Position at MMC for a threaded hole technically requires a virtual condition external thread gage fixed at the true position. Gage size would be MMC of pitch dia. (unless the default was overriden by a note) minus the position tolerance. Resulting in an external thread of non standard dimensions.

Theoretically, you are right. I winder, practically, how would one screw a threaded inserts while keeping true position? especially with a pattern...

 

[Burunduk]

Theoretically, you are right. I winder, practically, how would one screw a threaded inserts while keeping true position? especially with a pattern...

They won't, that's why position at MMC for the thread is nonsense.

 

[Garland23]

They won't, that's why position at MMC for the thread is nonsense.

That's why a projected tolerance zone should be used. Then the MMC idea makes perfect sense.

 

[3DDave]

An MMC thread gauge can have it's displacement from true position measured. There is no requirement to change the thread to match the position tolerance nor to locate the gauge at true position, "technically."

"Technically" a gauge plate with clearance holes made to match the position tolerance + diameter of exposed MMC thread gauge body would work as an acceptance fixture. Screw in all the MMC thread gauge bodies and set the gauge plate over them.

 

[Burunduk]

That's why a projected tolerance zone should be used. Then the MMC idea makes perfect sense.

If you are referring to using a functional gage with virtual condition holes sized to accept the protruding shanks of the mating screws considering the shanks' max. dia. and the threaded holes' position tolerance, then yes that is functional. You would also need to assemble some kind of gage screws or something similar to thread location gages with a protruding shank made at the MMC of the mating fastener. But unfortunately it's not supported officially. There is nothing in the standard to indicate that once the projected modifier is used, the surface interpretation of the MMC tolerance applies to the mating fastener.

3DDave, I think the above also goes for your suggestion if I get your idea of "MMC thread gauge" and the gage plate right.

 

[Wuzhee]

https://www.tec-ease.com/gdt-tips-view.php?q=109

I found this on the subject. Interesting read, it helped me understand with visual examples. (I'm a picture book guy )

 

[Burunduk]

https://www.tec-ease.com/gdt-tips-view.php?q=109

I found this on the subject. Interesting read, it helped me understand with visual examples. (I'm a picture book guy )

1. Nice explanation, but they forgot to standardize this interpretation (yes, it's the same guys that are in the Y14.5 committee).
A virtual condition for a surface interpretation of a hole is for a hole's surface. As much sense as it makes for a threaded hole, saying "OK, in this case it's for the male mating part" is one hell of an "extension of a principle".

2. You can see in the visual example in the end that they are suggesting the use of M10 go gages (adjusted for the purpose to have the MMC screw shank extension). A go gage has the most looseness with the recieving thread, so this play can be used to tilt the thread gage from its self-centered condition to make the plate with the holes fit over. In the assembly, where the male fasteners will fit more closely, you will not have the same ability to make it work.