Datum shift when datum is a thread, quick question 2

[greenimi]

I have a bore ID with a positional callout of Ø.003 at M with A at M, where datum A is a ID thread with size PD tolerance of .0055 (difference between max. PD and the min. PD).
Engineering wants to remove the M from the datum ID thread A because --per their statement-- a better alignment should be achieved between the ID thread and the bore ID.
I proposed to leave MMC at the thread and tight the positional tolerance (to even zero at MMC, if necessary) becasue the thread will be always assemled with some clearance. I know that the manufacturing will freak out when they see position zero at MMC with A at MMC!!
The question for you which of these 2 options is more effective to achieve better alignment between the thread ID (datum A) and the bore ID?
Worth to note that this part is assembled by having an OD thread with a OD bore component going into the part I am questioning and these 2 parts should be aligned (thread-thread and ID to OD).

Wihch of these 2 options is more appropriate in your opinion:
1.) Remove MMC from the datum A (ID thread)
2.) Adjust positional tolerance (again, to even zero) at MMC with ID thread at MMC.

Thank you for your help

If the issue is not so simple and you need additional information, please let me know.
Or maybe the issue is "six of one half of dozen of the other"

Please kindly advise.

Thank you again

 

[greenimi]

I forgot to mention that the thread is a straight thread 1/4 size (so, NO taper thread, pipe thread, ACME or anything like special threads)

 

[Belanger]

FYI -- this notion of M on threads is debated even among the GD&T experts. I'm in the camp that says it's OK to leave the M. While you don't feel any physical "jiggle" like you might with a clearance hole, there is still some tolerance even on a thread's diameter.

Plus, the M symbol is the ticket to functional gaging. So that's another advantage of leaving it. However, I would hesitate to take the tolerance to zero on a thread, although I advocate it for clearance holes/pins. I'm sure the other guys can weigh in on this.

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

http://www.gdtseminars.com

 

[greenimi]

Is it somebody active on this forum from the other side of the fence or the other camp? (to recomand to use the datum thread at RFS on a straight thread). Again, I am only talking about straight threads.
I read some old posts regarding this issue here on the forum (including some references to some books by James Meadows chairman of Y14.43 gaging standard, if i am not mistken) and everybody seems to recomand the same thing --leave the M there at the datum thread--- due to functionality and inspectability--if a product works/function in one way, leave the inspector to verify it in the same way---
I am curious what other side have to say about this and what are their arguments about using RFS at straight datum threads.
Thank you again

 

[DeanD3W]

greenimi,
I don't think applying MMC (or LMC) to a threaded feature is a good idea at all.

With the M following a tolerance value for a position or orientation tolerance (parallelism, perpendicularity, or angularity, that is) a bonus tolerance might exist, or if the appropriate modifier (MINOR DIA or MAJOR DIA) is applied a surface interpretation can unfortunately be used.

In line with your post here, if a threaded datum feature is referenced at M then shift may be used.

I've just stated what most everyone here already knows and which I think we will all agree upon. The part we don't agree upon is whether this is a good practice, or not. I believe it is not a good practice because it will enable acceptance of parts that may not function... The practices related to material condition or material boundary modifier allow the use of shift of a feature with respect to a DRF (mmc following a tolerance value) or an entire part with respect to a DRF (mmc following a datum feature letter). This shift can be used to more readily meet tolerances. This assumes that in assembly this looseness of fit that is modeled with the tolerancing can be used in a beneficial way, to enable everything to fit together, when without the shift the parts would not fit together. The problem with this approach for threads is that when threads are tightened the parts tend to center on each other and the shift or looseness of fit is not controllable or useable in a systematic and beneficial manner.

I think RFS/RMB is the best choice for threaded features.

To simplify inspection I think the modifiers "MINOR DIA" or "MAJOR DIA" placed below or beside the feature control frame are an acceptable way avoid the need for expensive tooling to find pitch cylinder axes. I'm not willing to go further and allow MMC on threads though. I see that as a case that lacks function-based justification.

Dean

http://www.d3w-engineering.com

 

[greenimi]

So, it's a matter of education or it's a matter of aplication? Other MVP's opinions?
I would like to educate myself with as much information as I can before I go and talk with our engineering department
Thank you gentlemens

 

[fsincox]

I think it is a compromise of conflicting interests. I am hoping this thread will become a catalog of the various points of view.
As I have read, threads tend to be self-centering, because of the opposed tapered faces, particularly as they are tightened for torque/loading purposes. When used in high stress applications the extra tolerance error could become a concern. Engineering wants to play it safe, so to speak. However, some threads are not even used for those purposes, say just for pushing or pulling.
Manufacturing and inspection would like to make their measurement easier and faster to keep production going so, mass production tends to leads to gauging demands. Gauging the major/minor diameter is easier than the theoretical pitch diameter.
Balances must be found and that is why each application needs to be looked at and simple, general rules are not given.
Frank

 

[DeanD3W]

Very well stated, Frank.

In my previous post my statement may have been a bit too emphatic against MMC being applied to threaded features... "Never say never" as they say... For some applications MMC may be OK, all things considered.

Maybe my opinion, put in better words would be... For typical threaded hole accepting fasteners applications, especially the critical or high stress applications that Frank brings up, I think RFS/RMB is the only justifiable choice.

Dean

http://www.d3w-engineering.com

 

[Belanger]

And my comments may be perceived as being too pro-MMC
I didn't mean for that; I agree that there is no absolute statement about this; it's on a case-by-case basis.

This will help... see these links to a couple other threads in the past where this was discussed.

http://eng-tips.com/viewthread.cfm?qid=266740

http://eng-tips.com/viewthread.cfm?qid=285951

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

http://www.gdtseminars.com

 

[greenimi]

I guess this thread has not become yet the catalog of the various points of view as Frank wants. May I ask other MVP's of this forum for their opinion (pmarc, Evan, MechNorth, CheckerHater, drawoh, etc) about "thread at MMC" or RFS. Which "camp" are you in?
If it's an application based, how a product engineer or a design engineer would like this determination? How does he know if MMC is detrimental or not?

 

[MechNorth]

The bigger issue is that thread-based results are notoriously difficult (impossible?) to reproduce, and therefore are of questionable value. Not speculation, by the way, but based on a number of studies by US, German, Canadian and other national institutes (and a couple others as I recall), which established that results are not repeatable, based on major, minor or pitch diameter. So, the value of them as a datum feature is extremely dubious in my opinion. Adding to that is the difficulty of even establishing a pitch diameter on such a small thread. If you're looking for a ballpark datum, try the minor diameter (internal thread) and add (M) if you want the float. It's not precisely the same, but the best labs in the world can't differentiate it anyway.
If I need to use a threaded feature as a datum feature, I'll go with major diameter (external) or minor diameter (internal) and go RFS in most cases. BUT, I really try hard not to use threads as datum features.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[greenimi]

Jim,

That is interesting approach and for me it's also surprising since we all know that threaded holes derive a negligible, non-quantifiable amount of bonus tolerance (or datum shift if the datum is the thread) from their pitch diameter.

My initial thought was to use the thread as a datum feature because it's a self centering and the amount of "wobble" is very small, it is a negligible amount that we usually don’t try to put a number on.


So, you are recommending to have the feature (the ID bore)as a datum and have a thread positioned to the ID bore ?

 

[MechNorth]

For an internal threaded feature, I typically use the minor diameter for establishing the feature axis or the datum axis. Where possible, I avoid using the thread to establish a datum axis. If alignment is important, I've added a cylindrical or conical feature that does the actual alignment, and therefore can be used repeatably as a datum feature.
You're right that threads do have a certain amount of centering, but you're presupposing that the body attached to the thread is properly centered on the thread (may be reasonable expectation if you know the process manufactures it this way, but not so likely otherwise).
It would be helpful if you could post a sample graphic.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[greenimi]

Jim,

A sample grafic is attached. Hope this helps.

Scenario A: datum A -thread-
Position of the ID bore could be with A at MMC or A at RFS (datum shift or no datum shift)

Scenario B: datum B- ID bore-
Position of the thread could be with B at MMC or B at RFS (with or without bonus tolerance, how much? not easy to say, non-quantifiable amount)

 

[MechNorth]

Ah, perhaps neither should be primary datum. If the part with the threaded base shuts off on the horizontal face, then that should be the primary datum feature because it controls the assembly first. After that, the Datum-B feature would be better as a secondary datum feature because there is little tolerance on the diameter, which probably means little play between the two parts (assumed); you would get more play on a 1/4" fastener. Don't forget to orient the secondary feature wrt the primary datum. I would probably add (M) to the position of the threaded feature (at MAJOR DIA on the male part or MINOR DIA on the female part), wrt primary/secondary. Whether or not (M) adds anything of value to you depends on whether the tolerance is large or trivial compared to the rest of your assembly. If scale is proportionate, there doesn't seem to be much depth of engagement on the "pin" feature at the bottom, however because it is the secondary datum feature, it should be adequate (not adequate as a primary though).
And don't forget to add a chamfer so that the pin will easily guide itself into the pocket.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[fsincox]

I agree, it looks like the face should be primary.
Frank

 

[greenimi]

I guess the picture itself does not reflect the functionality of the assembly. Should be revised a little per the new drawing attached.
Sorry for the mistake, but after Jim's replay I realized something is not quite right with my sketch (incomplete by intent)
I have attached the revised one.

I guess in this last case datum B is the Bore ID (primary datum). The question still remain and here I am not sure how will have more influence in orienting the assembly the thread or the bore ID?

 

[MechNorth]

Wow. Not much engagement on either; about 2mm on the thread, and less than 1mm on the pocket. In this case, I would be tempted to go with A-B (multiple datum features) with the thread spec'd at the minor diameter (on the bore); both features RFS, or both features (M). Note, though that when the thread minor diameter [A] is referenced at (M), in conjunction with the pocket at (M), you will likely get a conical zone for the datum shift. That may make it a bit more of a challenge to verify. RFS eliminates hard-gaging options, but also eliminates the complexity of a conical datum shift.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[greenimi]

Jim wrote:
"If you're looking for a ballpark datum, try the minor diameter (internal thread) and add (M) if you want the float. It's not precisely the same, but the best labs in the world can't differentiate it anyway.
If I need to use a threaded feature as a datum feature, I'll go with major diameter (external) or minor diameter (internal) and go RFS in most cases. BUT, I really try hard not to use threads as datum features."

Jim,
Related with this statement I have a followup question:

When the threaded holes are measured using the minor diameter (for internal holes), are we able to utilize the bonus tolerance, since the minor diameter of the hole isn’t the functional portion of the thread that is engaged by the mating screw?
Can we treat the bonus MMC driven from the minor in the same way as we would for clearance holes?

I am asking this, in general, and might not be applicable in my case, but good to know for future projects.

 

[MechNorth]

The standard doesn't give any guidance on this, but it's not prohibited (putting (M) on the thread minor diameter). So, you would get the bonus. As you indicated, it's not comparable to the shift at pitch cyl diameter. As I noted, I wouldn't go that route; RFS at least doesn't add any "false" bonus.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com