Measuring Position of UNJ Threaded Holes 1

On a CMM, it is easier to confirm the minor diameter of a hole rather than its pitch diameter. With a pitch diameter, the CMM Operator would have to thread a plug into each hole and then confirm the plug position. Take it out and then thread it into the next hole - yuck!

If you were producing a large run, then the answer is easy - minor diameter so that we could make a checking fixture.

On a short run, it would depend upon the tolerance allowed. If the positional tolerance is just a normal tolerance for this application, then I would suggest minor diameter. If the tolerance was quite tight and a stack up between the minor and pitch could affect the result, then I would suggest pitch diameter.

Normally, I would go for minor diameter.

Dave D.

How would the CMM operator go about measuring the position of the minor diameter? A gage pin?

Also, wouldn't it be reasonable for the inspector to change their inspection method if a particular hole was close enough to being out of tolerance for the difference between pitch diameter and minor diameter to matter?

If you place "MINOR DIA" below the feature control frame, then the CMM operator would check the minor diameter and it would not make any difference whether or not the feature is conforming or nonconforming. The CMM Operator checks the minor diameter.

How to measure? The CMM Operator will take a number of points around the inside diameter of the threaded hole to develop a centre. It is then compared to the true position of the hole and its actual position is reflected. If the hole was off 0.2 mm from the true position (theoretical), then the actual position would be a diametrical value of 0.4 mm.

He does not place a gauge pin in the hole as far as I know. That would be extremely difficult since the hole usually is perpendicular to the face (primary datum) and there would a slop between the pin and the minor diameter.

PS - I probably would not place a MMC on the threaded holes if you are producing only 1 part.

Dave D.

Not to be flippant, but for the bulk of this discussion, how it will be measured is irrelevant. Instead, think about the function!

ASME has pitch diameter as the default because the function of most threads is to engage with another thread, and the pitch diameter is where threads "grab" each other. Think about a cross-section view of a bolt threaded into a tapped hole -- the roots and crests of the threads don't really touch each other, but the pitch diameter serves to make the threads center themselves. Thus, functionally, the pitch diamter is often the one we want to examine for position tolerance.

I would state MINOR DIA not because it's easier to measure, but only if the threaded hole is acting as a through hole. (Similarly, MAJOR DIA would be stated for a bolt that merely passes through a clearance hole.)

Then -- after the function is accounted for -- we would need to assess the measurement method. Yes, MAJOR/MINOR is probably easier to measure, but I'm just saying that that shouldn't be the primary driver.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

I kind of agree with JP on this one, function comes first. Inspectablity and producibility are a close second, though, so we always need to think about them.

My thought is that one should always call out what they want/need on the drawing and let the manufacturing/inspection guys work out the details of how to make/inspect it (being experts in manufacturing/inspection).

Of course, it's never that simple: It doesn't make any difference what you put on the drawing if it's not inspectable or producible. Still, for a feature like a threaded hole, I think it's best to specify exactly the dimension that you care about and let the inspectors determine the most cost effective way of assuring that the machinists have met it.

Perhaps inspecting the minor diameter is sufficient to verify the position of the pitch diameter.

Can a gage like the one attached be used to measure the position of UNJC/UNJF threads in a CMM?

flash3780,

Yes, gages like that can be used.

While pitch diameter is the important feature, it is used as a datum for measurement less frequently due to inspection difficulty. This is true for fasteners and tapped holes, internal threads and external threads.

Functional gages and laser/optical devices can measure the pitch location. Try these suppliers:

The surfaces making up the minor diameter can be quite irregular and corrupt the position measurement. There are gages available that are designed to engage the pitch diameter. Why not use them?


Tunalover

I always use the True Position Locator on my CMM measuring, it works fine with me. You may find the TRU-POS here :

SEasonLee

There have been many studies conducted by national labs in the USA & around the world re the repeatability and accuracy differences associated with inspection of thread position based on the pitch, minor and major diameters. They (national labs) can't replicate their own results for the same setup within very tight tolerances.

Here's what I've worked with before. For an inner thread, enlarge the pre-drill hole slightly so that it is consistently formed and not affected by the root diameter of the cutter, and specify position at the minor diameter. For an external thread, reduce the outer diameter slightly so that has good form and is not affected by cutting the thread, and specifiy position at the major diameter.

For inspection of internal threads, I suggest a cylindrical probe on a CMM and a helical scan pattern. For external threads, I prefer a vision system if at all possible.

The improved quality of the minor (internal) or major (external) thread diameter improves the repeatability of the measurement, though not necessarily the position of the ACTUAL thread. Along with this, I also recommend that designers throw as much tolerance as possible toward the location of the thread to mitigate the errors of the inspection method. Talking with people who worked on the white papers & did the research & analysis, they had no issue with this methodology and several subscribed to it themselves.

Jim Sykes, P.Eng, GDTP-S
Profile Services TecEase, Inc.

Jim,
From your post it sounds like you're suggesting the manufacturer bump up the tap drill size a bit to get a more consistent minor diameter and measure the thread's minor diameter directly with a CMM (how small can you go with a CMM probe?) rather than using a plug gage.

However, from a designer's prospective, you're suggesting tolerancing the pitch diameter, but with a generous tolerance to allow for the error induced by the inspection method.

Is my understanding correct? If so, I'm not a metrology expert, but it's along my lines of thinking.

If the inspector decides on a thread position gage (reposted from earlier), will a UN gage work to measure the position of UNJ threads?

Flash, you can source CMM probes from a variety of OEM & aftermarket suppliers. I've seen cylindrical probes used on threads as small as M4, though I don't know the actual probe size. I'm actually advocating specifying the tolerance at the minor diameter for an internal thread and at major diameter for an external thread. The qualifier for that (as always) is that you have to rationalize it to the size of thread being considered. You CAN find a pitch cylinder by ball-probing a large thread (eg M30), so you may be better off in that case to use the thread pitch cylinder. Definitely can't directly probe the thread to find an M8 pitch cylinder. As mentioned by others, quantities matter in the decision too.

I worked on plates about 4'x6', with almost 600 M8 taps for a specific function, a bunch of M12's and a few M24's. We looked at using thread gaging inserts in conjunction with a CMM. At $80/M8 gauge (low-grade at the time), that's $48k for gage elements alone. Then the extra care involved; hand-chase each tapped hole to deburr it; carefully insert & seat the gauge plug into each, probe each plug, remove & clean & store the plugs. Then, of course, you have regular calibration on the gauges.
When I looked into the white papers, it was clear that the extra expense of using the gauges at pitch diameter would be prohibitively expensive and time consuming. We went with specifying the minor diameter for pretty much all internal threads of modest size.



Jim Sykes, P.Eng, GDTP-S
Profile Services TecEase, Inc.

MechNorth-
You said "They (national labs) can't replicate their own results for the same setup within very tight tolerances." What were the "very tight" tolerances?


Tunalover

I still maintain that you should specify the tolerance on the dimension that matters (in this case, the location of the pitch cylinder) and allow the inspector to choose the most cost effective way to inspect it.

The possible position error between pitch diameter and minor diameter of an internal thread is a known value. If the inspector chooses to inspect the minor diameter, they would simply add the possible position error between the pitch cylinder and the minor diameter to their "out of position" amount during inspection, correct?

If the part fails inspection the "quick way" the inspector may choose to look more carefully before scrapping the part.

Flash3780:

The CMM Operator will not chose whether to inspect the pitch or minor diameter, that is the decision of the Designer. Position will default to pitch diameter or if it is desired to have the minor diameter confirmed, the Designer would place a "MINOR DIA" under the FCF. The CMM Operator will check either the minor or pitch diameter that is required by the drawing.

You said "If the part fails inspection the "quick way" the inspector may choose to look more carefully before scrapping the part."

That doesn't happen. It is not the Inspector's authority to scrap parts but to reflect whether the part is conforming or nonconforming. The final disposition of "scrap" is a management decision.



Dave D.

Dave, pls don't talk in absolutes. You are (from memory) primarily of an automotive background; presumably heavily unionized with defined roles & responsibilities. I can tell you from lots of experience in all sorts of other industries that inspectors can, and do, disposition materials with great frequency. I, without being a manager or inspector, was dispositioning materials. Many companies run an MRP (materials review board) which dispositions without direct management input.

And, unfortunately, inspection often will inspect an internal thread at its root diameter rather than pitch cylinder, regardless of what the drawing says, because they have throughput and cost expectations on their work too. Not a perfect world, but the one that most of us live in. In fact, the majority of engineers/inspectors/machinists that take their first GD&T course are shocked to find that the controls apply at the pitch diameter. That doesn't mean that we quit doing things properly, but the reality is that comparatively few understand, much less properly use the pitch cylinder.

Tunalover, (personally, I'm a SalmonLover ... with a bit of maple-dijon glaze on the barbie ... mmm) I had the white paper from Sandia National Labs, one other US lab and either a Brit or Aussie national lab. The Sandia report is public, as should the rest of them be; I don't recall the tolerances other than they considered them to be tight (it was 10 years+ ago), but the details were in the reports. Maybe available online now.

Jim Sykes, P.Eng, GDTP-S
Profile Services TecEase, Inc.

And, unfortunately, inspection often will inspect an internal thread at its root diameter rather than pitch cylinder, regardless of what the drawing says, because they have throughput and cost expectations on their work too.

Click to expand...

No big deal if they do, just as long as they're not equating the minor diameter position to the pitch diameter position. If a drawing allows .015"DIA of position tolerance on a tapped hole, and measuring the minor diameter shows they hit it within .002" in a particular direction, grab a cold one cuz you're done.

However, if when measuring the same hole you find that it's out of position by .007" in a particular direction, you'd probably better look a bit more closely at that one, because your measurement method has limited accuracy.

However, regardless of how they check it, it's best to define the feature we care about directly rather than indirectly.

Where possible, we leave the machining methods to the millwrights and the inspection methods to the inspectors. They are, after all, experts in their respective fields.

Jim:

You are correct that some CMM Operators may take it upon themselves to scrap a product if it is nonconforming. In a structured quality system such as in companies that are in compliance to ISO 9000 or TS, it is not usually the responsibility of the Inspector.

Material Review boards are a structured method for dispositioning through management approval but this method is used infrequently.

I also agree that most people do not realize the positional on a threaded hole default to its pitch diameter and they would probably confirm the easiest feature which is the minor diameter. GD&T training $$ just are not out there right now and this is a complex subject.





Dave D.

Dave, and all of us, really, should qualify some of what we say for "trends" or "common practice" as being based on specific industries.
What you, Dave, have experienced is definitely not what I've experienced in a large cross-section of industries; military vehicle, aircraft & satellite, rocket, home appliance, automation, composite materials, mould, machinery, energy, and others, and even some automotive (Tier 2 & below typically). What you describe is consistent with what I've seen in unionized, parent company & Tier-1 automotive suppliers. I'm sure that it happens in many other unionized environments where job descriptions & limits/restrictions are well established & enforced, but from my exposure, non-union shops often spread the responsibility around the functional group.

Jim Sykes, P.Eng, GDTP-S
Profile Services TecEase, Inc.