MMC or no on Pos Tol for threaded holes 1

[fcsuper]

I looking to opinions about whether or not MMC (or LMC for that matter) is needed or even useful on positional tolerances to locate plane old threaded holes for mounting.

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

http://groups.yahoo.com/group/solidworks & http://twitter.com/fcsuper

 

[KENAT]

fcsuper, just recently I posted the link in another thread to

http://www.tec-ease.com/tips/june-03.htm.

So while I've never looked at it in detail my understanding is that invoking MMC allows the use of hard gauging or something like that.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[powerhound]

I never use it because I believe the only way it can be properly checked is with a hard gauge and no one wants to create a hard gauge for every hole pattern they make.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X4
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[KENAT]

Powerhound, does it mandate a hard gauge or just support its use if desired?

If the former then in many cases it might be best left off.

However, if it is't forcing use of a hard gauge then surely it's better to leave it in to allow use of a hard gauge if desired?

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[fcsuper]

So, based on this, if it is not critical enough to require a hard gage, then perhaps it isn't necessary? Or simply using it allows for a hard gage that may never be employed? When I'm aligning parts, I'm not relying on threads, but using pins. So, still just asking for opinions here. If aligned of the parts is important and I use a pin, wouldn't the MMC work best when applied to a pin instead the threads?

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

http://groups.yahoo.com/group/solidworks & http://twitter.com/fcsuper

 

[drawoh]

fcsuper,

I take it you are applying MMC to the positional tolerance itself, and not to the datums.

Given that tapped holes are very accurate, and that they are self centreing, I see no point applying tolerances at their MMC.

JHG

 

[flash3780]

This was recently brought up in another post (I originally thought that it was not appropriate, but the link KENAT provided clearly shows that it is).

http://www.eng-tips.com/viewthread.cfm?qid=264018&page=1

I don't know of a good way to check thread position without a threaded gage pin. However, specifying the thread position at RFS forces the inspector to check the hole position with other means (although I'm not sure what those are). From my understanding, there is nothing lost in allowing for hard gaging on a print, even if none is used.

Another thing to note is that ASME Y14.5-1994 defaults to the pitch diameter of the threads - which is likely what you're interested in anyways. If you're interested in controlling anything else (for some odd reason), you must specify MAJOR DIA or MINOR DIA.

 

[dingy2]

The only practical way of applying positional at MMC on a threaded hole is with the term "MINOR DIA" below the FCF. One cannot make a hard gauge without that term since positional would default to its pitch diameter.

On a threaded pin or stud, one should use the term "MAJOR DIA" below the FCF if positional at MMC is desired.

Frankly, if the hole pattern is not vital to its function or mating relationship, forget about MMC and just reflect positional in RFS. The Inspector will still have to make a threaded plug to check its position though even on a CMM.

Dave D.

http://www.qmsi.ca

 

[KENAT]

dingy2, so what's your take on the link I posted above?

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[Belanger]

Dave's comment also raise a question in my mind. He is certainly correct that a position tolerance applied to a threaded feature would be understood as applying to the pitch diameter (per the Y14.5 rule) unless otherwise specified.

But what does that rule really mean? Do we interpret that "pitch diameter" as being the actual pitch diameter of each manufactured part (the diameter where the thickness of the threads equals the spacing between the threads)?

Or do we interpret the phrase "pitch diameter" to mean the desired pitch diameter (or nominal, if you will) for the thread spec being given?


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

 

[MechNorth]

Use of MMC on a thread definitely does NOT require a hard gauge, but does allow it. By extension, it also allows use of other MMC-simulation technologies. First though, as Dave indicated, a note for AT MAJOR DIAMETER or AT MINOR DIAMETER really SHOULD be included in the callout because as JP indicated, there's still the question of which Pitch Diameter is being considered. The reality is that thread gauges are freaking expensive (in my experience) to buy, use and maintain. I worked with plates with hundreds of holes ... the time & gauge element costs involved in inspection would have been on par with the cost of the plate in some cases. Now, back to the MMC at MINOR / MAJOR DIAMETER callout; aside from hard-gauging, inspection can be done by similar technologies such as a CMM with a cylindrical probe, by a vision system, and maybe others.

Of course, MMC at MAJOR / MINOR DIA should only be used when the fastener is NOT being used as an alignment feature. Yes, it's bad practice to use a screw for alignment, but we all know that it happens regularly, particularly when the alignment isn't super-critical.

JP, to your question, wouldn't it be the design PD if it's being used as a datum feature, and actual DP if it's a regular feature? Just a thought.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[Belanger]

Good input, Jim. I'm still thinking it refers to actual PD, no matter whether it's a toleranced feature or a datum reference. I hold this notion because it seems like parallel logic to our understanding of GD&T applied to regular thru-holes. And if the MMC modifier is invoked on the pitch diameter, we'll have some value to compare against the design size.

That said, this "bonus tolerance" (or shift) will be pretty negligible.

I think this is why many people dislike MMC on a thread -- because in the final analysis they can't "see" any looseness. But think about it: a threaded hole could potentially have some bonus, and perhaps be a tiny bit off center. When the bolt is torqued down, it may simply hit its torque spec a little sooner. So there's no looseness to speak of, but the bonus effect did play a small role.

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

 

[dingy2]

Kenat:

You asked me what I thought of the checking fixture or method expressed by your Tec-Ease attachment in your original post. Tec-Ease usually have pretty good examples but this one is not at the top of the list. As a matter of fact, this example might be flawed. If a Toolmaker was given the drawing of the gauge, could he/she make the gauge? Not really!

The Tec-Ease gauge design does not show whether a full diameter or a threaded diameter pin would be inserted in each of the two (2) holes. It is a threaded diameter that should bottom out on surface datum A so the gauge pin thread length would be 10.2 mm. If the FCF does not state "MINOR DIA" then it is its axis derived from the pitch cylinder. (Screw Threads 2.9 - ASME Y14.5-2009 & 94). JP - I believe that it is its pitch cylinder rather than a theoretical one.

The full diameter that should protrude through the 15 mm projection is shown here in the Tec-Ease example is 10 mm. That makes sense but it would not make any difference whether we use 10 mm or, maybe, 12 mm. The gauge hole for the projection would be a diametrical tolerance zone 0.8 mm beyond either 10 mm or 12 mm. In the Tec-Ease example, it is a diameter of 10.8 mm. In our Tec-Ease example, one would have to insert each of the two (2) threaded pins through the projection plate (15 mm thick) and then thread the ends all the way down into the threaded holes until they contact against datum A surface. This simulates assembly. If either of the pins does not thread in the holes, the part is nonconforming.

There should also be hard pins in both datum B and C holes of virtual condition size, shape and orientation in the case of the slot.

If I were a Designer (and I'm not), I would place "MINOR DIA" under the feature control frame of a pattern of threaded holes as long as there was not a projection of an sort. A hard gauge of the minor diameter's virtual conditional size would be made and we would treat the threaded holes as plain holes. It is pretty easy to check on the shop floor.

If we had a projection value of any sort, I would not use "MINOR DIA" under the FCF but still reflect it in MMC such as the Tec-Ease example.

Dave D.

http://www.qmsi.ca

 

[rgb210]

Dave,
You are correct in your assesment of the hard gage used in the example if it were used to verify the upper segment of the position tolerance for the two threaded holes. The holes in the gage would need to be 10.8 dia for a 10.0 gage pin and datum simulators would be required for datums B and C.

The example given states it is for verifying the lower segment of the position tolerance, so I think the dia is correct and referencing datums B and C are not required.

Robert Bohot
GDTP-S