Thin Datum Surfaces 5

[AMontembeault]

I have a sheet metal part, which is more or less square, with a bilaterally symmetric, sinusoidal contour cut on one side. I set my primary datum "A" at the large planar surface of the part, secondary datum "B" as the midplane of the part, and tertiary datum "C" as the edge opposite my contour. The contour is controlled by line profile with respect to A|B|C.

The problem we're running into pertains to ASME Y14.5-2018 section 7.9, specifically that all datum features must be controlled by appropriate geometric tolerances and/or size dimensions. Putting flatness on A, and perpendicularity on B with respect to A, and perpendicularity on C with respect to A and B makes sense in theory, but in practicality its proving to be very difficult to measure, given how thin the part is and how little real estate is available to probe with a CMM.

The only way I can think of to inspect this part is through the use of fixtures/functional gauges, but was wondering if perhaps anyone had run into something similar and might have better ideas. A change in the GD&T, or a different method of inspection?

 

[Burunduk]

AMontembeault,
What you describe is an inspection related problem, not a drawing specification related problem.
It can possibly be handled by inspection related solutions, not by changing the design intent reflected by the drawing. A suggestion -most shops that use a CMM also have an optical comparator available. A comparator has its shortcomings, but it doesn't require probing, and you may find it reasonably reliable for detecting the perpendicularity variation in question. I am not an inspection guy, and I only make this suggestion based on my limited observations in this field. Someone with broader knowledge in metrology may address this better.

 

[pmarc]

Regarding the solution of applying surface profile on the very thin peripheral faces of the sheet metal part:
If everyone is aware and accepts that the profile tolerance will be verified only at a single 2D section (at some probe-contactable height above datum A), and that the normal orientation of the surfaces relative to datum A will not be controlled, wouldn't it be more appropriate to change the drawing tolerance to profile of a line, to reflect that? Although profile of a line is usually checked in more than one cross-section, I don't think it is a mandatory requirement for all cases.

Burunduk,
Thin peripheral faces are still faces. So unless the line profile tolerance zones are fully constrained with respect to the referenced datum feature(s) (which would not be the case in the line-profile-wrt-A scenario), I believe surface profile should be used to avoid incomplete definition.

The fact that "everyone is aware and accepts that the profile tolerance will be verified only at a single 2D section (at some probe-contactable height above datum A), and that the normal orientation of the surfaces relative to datum A will not be controlled" is something that should be reflected in the inspection plan, in my opinion.

On a side note, if the datum features on a thin part fully constrain all degrees of freedom of the profile tolerance zone, e.g, in the |A|B|C| case, I have seen people applying line profile instead of surface profile to sucessfully get a buy-in from those that did not necessarily like surface profile, even though from the interpretation standpoint the two callouts were no different.

 

[greenimi]

On a side note, if the datum features on a thin part fully constrain all degrees of freedom of the profile tolerance zone, e.g, in the |A|B|C| case, I have seen people applying line profile instead of surface profile to sucessfully get a buy-in from those that did not necessarily like surface profile, even though from the interpretation standpoint the two callouts were no different.

Pmarc,
What would be the differences then between profile of a line and profile of a surface?
On the profile of a line: wouldn't you need to qualify "all the lines" on that particular thin feature? So in essence why that (measuring "all the lines") will not become or made up the entire surface?
I don't see much of the difference, even from the theory point of view.....

 

[pmarc]

greenimi,

I thought I said that there would be no difference between line profile and surface profile in the |A|B|C| case.

 

[axym]

Hi All,

Here are some thoughts. The first one is that this topic is a rabbit hole, and it's going to get weird! The features on "thin" parts can confound some of the traditional GD&T approaches and give us headaches in CMM inspection as well. The features are technically 3D surfaces but function as if they are 2D lines.

There are several things going on here, but let's start with Feature C. Let's say that the Perpendicularity tolerance for feature C is 0.1 mm to A and B. The requirement is that all of the points on the surface C must lie within a zone 0.1 in thickness, with the requirement that the zone is exactly perpendicular to both Datum A and Datum B. There is no requirement to measure it in a certain way, but most CMM software imposes certain restrictions. Feature B is technically a planar surface (there will be a vertical surface in the CAD model, however thin). In order to apply a Perpendicularity tolerance, most CMM software requires that the surface be measured as a Plane. This becomes inconvenient with thin parts, if the diameter of the CMM stylus is comparable to the part thickness. We might only be able to touch points at one depth, and we need points at at least two different depths to define a Plane feature. I would say that this particular issue represents limitations in the CMM hardware and software. If we had a CMM that collected points differently (smaller stylus or perhaps non-contact scanning), then we could measure points at different depths. The part might be thin, but it's not infinitely thin (it must have a finite thickness).

If we think about the Perpendicularity tolerance on feature C, what does it really control? I agree that there is a "psychological" aspect that applies here, because of the term "perpendicularity". What does it mean for feature C to be perpendicular to A and B? All points on feature C must be within a zone 0.1 in thickness, with that zone oriented exactly perpendicular to A and B. We can say that this controls the feature's orientation or "tilt" relative to A, but we really don't have to say that. We only say it because Perpendicularity is described as an orientation tolerance. When feature C is very thin and has essentially zero depth, the "orientation" aspect relative to A effectively drops away.

Feature B defeats some of the usual GD&T approaches as well. Feature B is technically a feature of size (outer width) made up of 2 parallel planar surfaces. The traditional GD&T approach would be to control this feature with a Size tolerance and a Perpendicularity tolerance. On a very thin part, even measuring the size can be ambiguous and require assumptions, but I won't go into that just now. The Perpendicularity tolerance definitely causes major issues when the part is very thin. What does the Perpendicularity tolerance actually control? The center plane of the feature's UAME (Unrelated Actual Mating Envelope) must be within a tolerance zone that is exactly perpendicular to Datum A. So to measure this we must establish the UAME, and that's the hard part! On a thin feature with slightly tilted or irregular surfaces, the UAME can be extremely difficult and error-prone to establish (especially the orientation of the UAME, which is the only thing we care about in this case). If we're using a CMM and can only measure points at one depth, it's impossible. With physical equipment, the UAME would be the "minimum circumscribed slot" of feature B. Imagine putting vise jaws around an outer width feature on a sheet metal part, to establish its center plane. I would go as far as to say that width features on thin parts defeat Y14.5's definition of the UAME and the resulting center plane.

So where does that leave us? Feature B still functions somehow, even if we can't measure the perpendicularity of its center plane. So what could have been specified instead of Size and Perpendicularity? As others have suggested, Surface Profile is always an option. There is another more obscure option that I would like to bring up as well, that is probably much closer to capturing the real requirement on feature B. If the Perpendicularity tolerance was specified at MMC instead of RFS, then we could apply the Surface Method. This is described in the text of Y14.5-2018 (Section 9.3.5), but there is no example illustrating it. In a similar way to Position at MMC, an orientation tolerance at MMC can be interpreted as creating a VC boundary for the surface of the feature. In the case of outer width feature B on the OP's thin part, the specified Perpendicularity tolerance would be added to the MMC size of the feature. Inspecting the Perpendicularity would amount to verifying that the feature fits between two parallel planes that are spaced apart by the VC size, and oriented exactly perpendicular to Datum A. This could be done easily with a hard gage, or calculated from the CMM points even if they were all at the same depth. There is no requirement to establish the UAME and center plane.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[greenimi]

Inspecting the Perpendicularity would amount to verifying that the feature fits between two parallel planes that are spaced apart by the VC size, and oriented exactly perpendicular to Datum A. This could be done easily with a hard gage, or calculated from the CMM points even if they were all at the same depth. There is no requirement to establish the UAME and center plane

Evan,
When/if ASME committee will decide to scrap the axis interpretation for features modified at MMC/LMC (as proposed) we will have not much to talk about regarding this case, doesn't it?

 

[3DDave]

The axis interpretation is required when the location tolerance is greater than the feature size such as would be used for the pattern locating tolerance in a composite feature control frame.

 

[axym]

greenimi,

I think that we'll still be talking about cases like this for quite a while. If the Y14.5 committee decides to go all-in on the surface method for tolerances at MMC/LMC and scrap the axis/centerplane method, this wouldn't go into effect until several years from now when the next version of Y14.5 is released. Even then, I would say that the axis/centerplane method will still be widely used in industry. It's so well entrenched - the vast majority of inspection uses the axis method, thousands of CMM programs use it, and axis / bonus tolerance calculations have been a cornerstone of GD&T training for decades. There will still be plenty of drawings referencing 2018, 2009, and even the 1994 standard.

It will be interesting to see how things shake out regarding the surface method versus the axis/centerplane method. Calculations for measured values based on the surface method were only recently included in an ASME standard (Y14.45-2021) and most CMM software packages don't currently support it. This will change, but I'm not sure how soon.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[axym]

3DDave,

I agree that the axis/centerplane method is needed when the location tolerance is greater than the feature size. Y14.5-2018 mentions this case in the note in 5.9.4.1 - it states that in the case of a negative VC the surface interpretation does not apply. This provides one argument against scrapping the axis method (see previous post above).

I would say that it wasn't really necessary to specifically disallow the negative VC. If the location tolerance is greater than the feature size, then the position tolerance shouldn't be apecified at MMC the first place. This situation doesn't correspond to the function of clearance with a mating part feature, and it wouldn't make functional sense to allow more location tolerance as the feature departs from MMC. It would be an RFS application, in which the axis is controlled.

I don't see a connection to composite FCF's though.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[3DDave]

OK - Should I have said PLAHTZF and FRITZIF? Both would use the MMC modifier to eliminate the need to find whatever the centroid of the pattern would be applicable to the PLAHTZF.

Did composite tolerancing change in 2018 in a way that is different than before?

 

[Burunduk]

Not all inspection devices are well-suited for all possible types of geometries.
Switching to another inspection method could make this whole discussion irrelevant.

 

[axym]

3DDave,

I still don't see the connection to composite Position FCF's. As far as I know, there has never been a requirement to find the centroid of the pattern. The requirement always involves a framework of tolerance zones or VC boundaries, whether it's the PLTZF or the FRTZF or referenced RFS or MMC. Can you provide a reference from Y14.5 that mentions the centroid? I know that the centroid is sometimes calculated by CMM software in order to measure the XY coordinates of the "center" of the pattern, but this practice does not follow Y14.5 theory.

The workings of composite FCF's didn't change in 2018 - it's fundamentally the same as 2009 and 1994.

Composite tolerancing didn't change in 2018.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[3DDave]

"I still don't see the connection to composite Position FCF's."

I am at a loss then. It seems like that is the most likely case but there we are.

No, no such references - Y14.5 committee whiffed on the subject of patterns at RFS so I'm doubly confused by your insistence they would be required to use RFS for large tolerances.

 

[axym]

3DDave,

RFS isn't required for large Position tolerances - it's required in the specific case where the Position tolerance is large compared to the absolute size of the feature. Where the VC boundary goes down to zero, or less.

So if we had 50 mm holes with a Position tolerance of 10 mm at MMC, that's no problem at all. The VC boundary would be 18 mm, and we could make a gage with 40 mm pins that the holes would have to fit over. But if we had 2 mm holes with a Position tolerance of 10 mm at MMC, that's a problem. The size of the VC boundary becomes negative, and there is no volume of space inside the hole that the surface won't possibly encroach on. So we can't use the surface method, and it wouldn't make sense to specify the tolerance at MMC. It would only make sense to control the axis, and hence specify the Position tolerance RFS instead of at MMC.

To me, this applies in the same way whether it's a single-segment Position tolerance or a PLTZF or a FRTZF.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[3DDave]

I'll pretend you are writing to a novice audience Evan, and not to me. I've needed to locate mounting holes on large vehicles for mating brackets - the location could vary by a foot or more and still be fine but the individual members of the pattern needed to be closely located. I'll presume you have never had the need for that case. It's a straightforward mathematical analysis that doesn't require RFS.

 

[axym]

3DDave,

OK, I think that I might finally be seeing what you're getting at.

If you used a composite Position FCF for the mounting hole application you described, and we assume that the holes are 1" in diameter, then:

-The upper segment pattern-locating tolerance (PLTZF) would be 12". This would have to be RFS, because if it was at MMC then the VC would be negative. You couldn't use a hard gage with pins to check this tolerance.
-The lower segment feature-relating tolerance (FRTZF) would be, say, 0.1". This could be specified at MMC and checked with a hard gage with 0.9" pins. The lower segment tolerance could be specified RFS, but it wouldn't have to be.

Is this what you meant in the post from Feb 18, where you first mentioned the pattern locating tolerance? I agree that the negative VC is much more likely to occur with the pattern-locating tolerance than with the feature-relating tolerance. I hadn't made that connection to composite FCF's before - my apologies for being so slow to get it.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[Burunduk]

Evan,
Thin datum surfaces are not the only problem with sheet metal parts.
Where there are holes in a sheet metal part, the holes can't constrain the simulator of the unrelated actual mating envelope to derive an axis as required by the standard.
My proposal is to eliminate sheet metal parts from the industry.
All parts should be made with sufficient thickness so that the Y14.5 concepts can be applicable.

 

[Belanger]

Burunduk, I realize your comment is tongue-in-cheek, but anybody dealing with sheet metal would never make a hole the primary datum! So there's really no need for the UAME. It would always be a secondary or tertiary datum, meaning RAME, and then an axis is achievable.

 

[Burunduk]

Hi Belanger,
OK, no primary datum holes for sheet metal then.
How about position at RFS to locate holes or slots? The UAME is needed to simulate the axis or center plane that has to be checked for conformance. 
Do you say that position at RFS can't be applied on sheet metal?

 

[drawoh]

AMontembeault,

Read ASME Y14.5-2018 Section 7.20 RESTRAINED CONDITION. You need to tell everyone how to constrain your part for fabrication and inspection. Most of the time, when I design a flat piece of plate or sheet metal, I state that Datum[ ]A applies when the part is clamped to a flat reference surface.

--
JHG