ASME Y14.5-xxxx Profile of a Surface - clarification 3

[JNieman]

I am butting heads with one of our quality department inspectors. He's our lead inspector and we disagree on the application of Profile tolerance of a Surface. I've attached a simple sketch we drew up together to argue over.

He believes that a hole, slot, etc, that intersects the surface being called out, also has a location&size tolerance applied to it BY the Profile Of A Surface tolerance.

The only foundation for his assessment is that is what he was instructed to do in a former position at a well known aerospace manufacturer, and when I slammed by copy of ASME Y14.5-2009 on his desk and told him "Prove it" - all he could come up with was citing 8.2

"Profile" where it says: "A profile is an outline of a surface, a shape made up of one or more featuers, or a two-dimensional element of one or more features. Profile tolerances are used to define a tolerance zone to control form or combinations of size, form, orientation, and location of a feature(s) relative to a true profile."

Those two sentences, he asserts, allows/forces him to check the location and size of a feature at the surface it intersects, if that surface is called out with a GD&T Profile tolerance.

I feel like I'm stuck trying to prove something DOESN'T exist while he stands fast on his status quo.

If I am mistaken, I owe him a sincere apology and a cold drink.

If I am right, I would like suggestions as to how I can further present my case more clearly.

 

[greenimi]

Let me ask something: why in this case (shown OP) profile with NO datum is *NOT* equivalent with flatness? In other words, why profile is used and not flatness? What *extra* controls the profile callout and flatness doesn't?
I know GD and T is a language, but why bring more complexity into the equation when is not needed?

 

[3DDave]

There is overlap among many of the controls. There was a fair argument for eliminating flatness in favor of using profile, but I think flatness has now been promoted to also being able to control the centerplane variation, which profile does not.

Remaining targets are parallelism and perpendicularity, which could be replaced by angularity.

 

[greenimi]

3DDave,

I am not asking to replace the flatness with profile --in favor of using profile in GD and T language-- Flatness have its role/usage and profile its own. The same for perpendicularity, parallelism versus angularity. Why more complicated language to be used when a simpler one is available.

I am asking *IN THIS SPECIFIC CASE* (OP) what advantages someone will gain by using profile and *NOT* flatness? Why use profile? What they try to control?

And one additional question: “how flatness is able to control the centerplane variation?” Can you give me an example, or reference a picture in 1994 or 2009 standard? I am not saying is not true, I am trying to learn from this thread.

Thank you

 

[JNieman]

@greenimi, the example in the OP was mine, I believe I sketched it up during our discussions and it is rather simplistic. Sometimes being too-simple leads to more questions. It suited our discussion only, and for that purpose it sufficed. It is not an example of a good working drawing, certainly.

However, in general, flatness does not relate the surface to anything else. It can be flat, but be several inches away from nominal location, and be acceptable. If PoaS was applied rather than flatness, it would also have to be located at the correct position in space relative to datums or model based data, if referenced. I imagine if there were no MBD or Datums, that it would be akin to flatness, but I hadn't run into that situation yet and yes, it would be poor practice.

Again, the sketch was simply an illustration of a topic. That is the context and scope of this simple illustration. It's a glorified napkin sketch.

_________________________________________
Engineer, Precision Manufacturing Job Shop
Tool & Die, Aerospace, Defense, Medical, Agricultural, Firearms

NX8.0, Solidworks 2014, AutoCAD LT, Autocad Plant 3D 2013, Enovia DMUv5

 

[pmarc]

I am asking *IN THIS SPECIFIC CASE* (OP) what advantages someone will gain by using profile and *NOT* flatness? Why use profile? What they try to control?

greenimi,
Notice that OP already admitted that the callout he posted is incomplete. For sure datum feature references are missing in profile of surface FCF, unless this face is primary datum feature. And these datum feature references are needed to clearly define orientation of considered surface relative to datum(s). Flatness tolerance, unlike profile, can't use datums inside feature control frame - in other words, flatness tolerance is not powerful enough to control orientation of a feature relative to datum(s). This is the main difference between both characteristics in this case.

If the surface in question was primary datum feature, there would be no difference whether flatness or profile of surface was used.

And one additional question: “how flatness is able to control the centerplane variation?” Can you give me an example, or reference a picture in 1994 or 2009 standard? I am not saying is not true, I am trying to learn from this thread.

To be precise, per 2009 standard flatness tolerance can be applied to control form of derived median plane of a feature of size (see fig. 5-9). This is not exactly the same as control of form of center plane, because center plane by definition can't have any form error - it is a perfect plane derived from unrelated actual mating envelope of a feature of size. The whole concept did not exist in '94 version of Y14.5 - straightness tolerance was applied instead (see para. 6.4.1.1.3).

 

[ewh]

I have seen profile used for an entire part before, but very rarely. ALL dimensions are basic and no other tolerance is indicated on the drawing. (I am unable to view the picture link)
In my own experience, parts always seem to have features of varying requirements and a single profile tolerance never meet all of the requirements without unnecessarily restricting features that could have looser tolerances.


“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[axym]

nwrichard,

I believe I understand the logic behind your assertion, that profile of a surface can control the location of adjacent perpendicular features by the presence or absence of material. By specifying surface profile on one face of a brick-shaped part, you could also control the length and width. While it makes an interesting discussion, I can assure you that this logic is not used by the standards committees or industry in general.

Maybe this will help. ASME Y14.5 (Dimensioning and Tolerancing) and Y14.5.1 (Mathematical Definitions) both define a profile tolerance zone as applying in a direction normal to the true profile at every point on the true profile. This is how a surface profile tolerance locates features - in the direction normal to the true profile. Your argument goes past this, by trying to control the boundaries of the surface in directions that are parallel (not normal) to the true profile. In other words, you're trying to use the profile tolerance to define the extent of the surface. The ASME standards don't do this.

You've also cited the Tec-Ease web site and other "qualified, certified schools" as supporting your opinion. The only evidence you've presented to support this is that they state that profile tolerances control the location of surfaces and could be used to control all of the surfaces of a part. These are both true, but don't support your assertions for JNieman's drawing. In order for the surface profile to locate the other features on the part, it would have to be applied to those other features. Currently the profile tolerance is applied to just the one surface.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[powerhound]

nwrichard,

This thread has actually provided at least two views from qualified, certified trainers that are different from yours. Does this qualify for "in writing."?

To Evan's point; your assertion that profile of a surface can be used to locate features does nothing to support your argument. I'm not surprised that Tec-ease would make that statement since it is true.

I'm interested to know if you still stand staunchly by your viewpoint or if you are actually entertaining the notion that maybe JNieman got it right.

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[ptruitt]

nwrichard,

Some of the folks who post here are the best of the best when it comes to ASME Y14.5-2009 and have helped shape Y14.5 over the years. They disagree sometimes, but not with respect to this. Take some time and look deeper. They have set me straight on many occasions.

Peter Truitt
Minnesota

 

[powerhound]

JNieman,

Can you update us on this? Has your company responded positively to our input?

Thanks,

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[dtmbiz]

(apologies: cannot see posted doc’s; so I am visualizing)

Ref: ASME Y14.5 1994 Fig 6-20 and 6-21. Interrupted surfaces

The standard states that a profile control establishes tolerance boundaries.

It is simple enough for me to inspect the surface feature in consideration,
to verify if all of the surface elements lie within the specified boundaries.
The key (IMO) is to inspect the surface that does exist; not, what does not exist.

The slot is a feature that creates an interrupted surface.
The specific Profile Control for the surface in consideration,
does not control the features that interrupt it.
(unless leader lines associate it to the Profile Control frame;
don’t believe that is the case here)

Features that interrupt a surface are simply different features.

They are defined and inspected by their dimensions and geometric controls.

IMO: “Thinking is over rated”. This is being over thought.

Don't:

 

[CheckerHater]

The specific Profile Control for the surface in consideration, does not control the features that interrupt it.

Exactly!

You can also back it up by profile definition in Y14.5.1M:
“A profile tolerance zone is an area or a volume generated by offsetting each point on the nominal surface in a direction normal to the nominal surface at that point.” (Para. 6.5)
By definition tolerance zone cannot extend outside of nominal surface, because there is nothing to offset.
So the gap in nominal surface creates a gap in tolerance zone. (See picture)

 

[JNieman]

This discussion has been on the backburner, for now. I grew very tired of arguing what I think is long-settled, and have no idea what conversation may have transpired in the quality department. I do not know, in general, if his incorrect practice has been applied to /any/ parts going through the shop, but I've been keeping tabs on the tools and parts going through the shop that are of particular interest to me, and have not seen anywhere that our current disagreement would impact them. So because of this, I've refrained from bringing it up. I hadn't even discussed it since he posted here.

_________________________________________
Engineer, Precision Manufacturing Job Shop
Tool & Die, Aerospace, Defense, Medical, Agricultural, Firearms

NX8.0, Solidworks 2014, AutoCAD LT, Autocad Plant 3D 2013, Enovia DMUv5

 

[powerhound]

So he expected to get a cold drink but was only willing to give a cold shoulder.

Inspectors...pfft.

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[jflongwell]

To nwrichard:
As a professor in a certified college and ASME GDTP S0667, I caution you against using instructors as basis for standard compliance. I know of many other fellow faculty that teach GD&T incorrectly. They have learned it by teaching themselves.

The tolerance zone would not be applied to the slot, a separate FCF is needed to create another tolerance zone, or use the "all over" (2009) symbol.

John

 

[s4more]

Hi guys there is a solution for this argument within the standard itself.

the use of 'between' modifier i.e. the double leader arrow.

See 3.3.11 Between symbol
"The symbolic means of indicating that a tolerance
or other specification apply across multiple features
or to a limited segment of a feature between designated
extremities is shown in Figs. 3-11, 3-14, 8-6, and 8-7. The
leader from the feature control frame is directed to the
portion of the feature to which that tolerance applies. In
Fig. 3-14, for example, the tolerance applies only between
G and H. G and H may be points, lines, or features."

fig 3-14 shows application to a profile tolerance.

Although in the case of the attached drawing by JNieman in the opening post, the extent should be unambiguous in my view, using the above solution especially for peripheral profile tolerances would eliminate any chance of misrepresentation.

 

[powerhound]

S4more,
While this argument will probably never be officially resolved due to a lack of response by nwrichard, there's no question in anyone's mind that his notion was incorrect and he's just bowed out rather than acknowledge that he actually learned something. That's the whole purpose of this forum anyway, not to prove who's wrong or right.

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II