FOS (Parallel edges as Feature of Size) ???

[dtmbiz]

Input please....

(See attached drawing)

A drawing uses a position tolerance control for centering a flat by using 2 edges identified as a Feature of Size.

Do straight line edges constitute “opposing elements” as mentioned in the 1994 version’s definition of feature of size?

 

[KENAT]

Can you argue the corners are 'opposed elements'?

Posting guidelines faq731-376

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

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

 

[powerhound]

My opinion is that while this does meet the definition of a feature of size, it is a difficult check because a CMM will yield varying results (but not by much) and the "caliper test" will be dependent on the perfect state of the ID jaws and a perfectly sharp corner.

I believe that this is legal but not very inspection friendly.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[dingy2]

This is a tough one.

I viewed the width as part of the intersecting points for the two surfaces with the 1 inch dimension the other component. While I can see the parallel elements of both inclined sides as a feature of size, I have a hard time acknowledging that a couple of interesting points are a feature of size.

Dave D.

http://www.qmsi.ca

 

[powerhound]

I agree with you Dave. I have a hard time with it too, but it does satisfy the "opposed elements" requirement. There has to be a better way to do this.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[MechNorth]

Strictly speaking, it may be a FOS per the definition in Y14.5, however the INTENT is for the points to be directly opposed per what used to be called the Caliper Rule. In real terms, this isn't an FOS, and position shouldn't be used.

We don't know the function of the part, so we can't say whether the center of the flat is actually critical. That being said, here are some thoughts based on my own experiences with similar parts & features;
- with tapered features, generally the location of the tapers has always been more relevant than the center plane of the flat at the bottom
- if the center plane at the bottom is critical, then there should be minimal vertical walls at the junction with the tapered sides to ensure that the flat does the centering rather than the tapers; generally manufacturing really hates sharp internal transitions, and will apply a tooling radius with or without a vertical wall also added
- assuming that the tapers provide the centering effect, the best way to control them is to use a surface profile (with a basic angle); a composite profile will link the two tapered surfaces even more tightly

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[Belanger]

Righto, Jim. I was just about to say "profile of a surface."

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

http://www.gdtseminars.com

 

[dtmbiz]

I agree that the edges do appear to fit the definition of FOS, however it doesnt appear to meet a "practical" defintion in terms of inspection (IMO).

The flat at the base of the angled surfs is important in this case Jim. My suggestion of a profile callout was validated by your comment. I am glad that you pointed out the "INTENT" and Caliper rule. Also interesting comment about the minimum vertical walls.

I have been told that, "... this has been the callout on a customer dwg for over 15 years". I hate to hear that argument because if it isnt in compliance with the standard and 'practical' application, I really dont care how many years the callout existed!!!
(Anyway, 15 years ago would have probably taken the callout back to the 1973 version...)


My thanks to all for your greatly appreciated comments!!!
Hearing from you folks helps me to keep my sanity at times.
Ignorance of the standard and/or an unwillingness to think thru a callout in practical terms is extremely frustrating to me at times.

 

[fsincox]

Jim,
I am confused, We seem so close, assume for my discussion this is a "V" block, I would then argee "we are concerned about the centering effect", but, how we leap from there to profile of a sufrace. This is a big leap for me so we will ignore the center completely? If I was locating somthing to the "V" wouldn't the center be just the point I want to determine?
Frank

 

[dtmbiz]

fsincox

The problem in this case is reality. The drawing shows sharp corners, however in reality there are radii in those corners. It is a machined part with a general note of .010-.030" inside radii.
Now how is it a feature of size when we go to the part, not the drawing?

I suggested to create a target line on each of the angled surfaces above the edges. "They" insist that the dimension stay where it is shown.

 

[powerhound]

"... this has been the callout on a customer dwg for over 15 years".

I think everyone of us on this BB has dealt with that philosophy at one point or another. They get good parts in spite of the drawing, not because of it.

A large company here in my city went through a huge cost saving exercise several years ago. They sent all their prints out to get requoted and they went with the lowest bidder in each case. The result was that all the tribal knowledge that their previous vendors had developed over the years in order to give this company what they needed (despite what the prints said they needed) was lost and they had a massive influx of parts that met print but were non-functional. This company is still one of the worst offenders I've ever dealt with in terms of terrible prints.

I am not exaggerating when I say that I would see things like "flat within a diameter" or "profile of a surface at MMC" on a regular basis. Anyway, they are still like that and they insist their print are good, it's just a matter of getting a machine shop to correctly interpret GD&T.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[MechNorth]

Frank, how do you locate an inclined plane (or 2) wrt the datums? Not +/- (not an FOS). For the V-block fixture example you cite, the two tapered sides establish a center datum plane). You then are comparing the location of the centered feature to the datum plane established by the v-block. Or am I missing something in your question?

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[fsincox]

Jim,
That is kind of what I am exploring, here. I want a way to specify define/control of the center derived by the "V". I am maintainining this is what many of these V's are often used for defining a centerplane as you mentioned. I understand you want me to use profile on the tapered faces but how should I reference the centerplane?
Frank

 

[MechNorth]

Two ways to do this that I can think of;
1) The datum feature callout would be in-line with the basic dimension of the included angle, then the profile FCF would point to the two inclined surfaces and reference the primary datum. CAD systems don't typically hold associativity between the datum callout and the dimension leader for angles ... don't know why.
2) Use a single profile FCF with two leaders pointing to the two inclined surfaces, and hang the datum feature callout off of the FCF. The FCF would reference the primary datum.

Arguably, either profile FCF could reference the secondary (centerplane) datum as well, though that will inevitably bring up the self-referencing datum, and isn't worth the effort in this case.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

I agree with Frank that I think the surfaces of the symmetrical V is not as important as its center plane. Profile of a Surface is doable but using that requirement does not emphasize its center plane. The positional tolerance at MMC shown on the drawing for the intersecting points is inappropriate since, I believe, we are interested in the center plane of the symmetrical V taken from the surfaces of the V.

The drawing is somewhat incomplete since an angle has not been specified nor the dimension to the top of the V. I am going to go a different way.

From 2009 edition page 156
"7.7. Symmetry Tolerancing to Control the Median Points of Opposed or Corresponding Located Elements of Features
Symmetry is that condition where the median points of all opposed or correspondingly located elements of two or more feature surfaces are congruent with a datum axis or center plane."

Notice that the above statement did not state feature of size but surfaces. I have never used nor ever recommended that use of symmetry but I think this is a great example of its value. I have attached a bit of drawing in a word program so the arrow heads on the angle are not the best.

To confirm symmetry, I would use a CMM and take 2 opposing points on the V surfaces parallel with the bottom and find the median point. I would compare this to the datum center plane using a +/- .005 tolerance. Take about 4 or 5 pairs on the surface at either the same height from the bottom or at different heights. All should be within the .010 symmetry tolerance.

What do you think?

Dave D.
www.qmsi.ca

 

[MechNorth]

Don't think so, Dave. What happens as the "V" increases in width along the length of the part? The point-to-point averaged centerplane (derived median) would still be straight, but the V would be useless. You need to control the faces of the V as well, and I would argue that the control of the faces of the V is what establishes the control of the centerplane (indirectly).

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

Jim:

If the feature was a slot (parallel sides), we would place a positional tolerance on it to control its location. Would we place a profile of a surface on each of the sides? Probably not. We would probably use a vernier and check the slot width in a few spots and that is it. The location would appear to be vital to its function and mating relationship rather than the surfaces.

The original drawing had linear tolerances for the intersecting points for the angle. The angle was not given so I made one up and there would probably be a default angularity tolerance of, say, +/- 30 minutes. The surfaces are controlled similar to the surfaces on a slot. It may not be the tightest control but controlled.

I agree that the V surface may not be perfectly flat nor the angle perfectly on 45 degrees just like the surfaces of a slot. It is the center plane location that the Designer is interested. The application of symmetry on the V surfaces directly controls the center plane relative to datum B.





Dave D.

http://www.qmsi.ca

 

[MechNorth]

As a veteran designer, I don't tend to position the centerplane of a rectangular slot either. If the slot is horizontal, I am most commonly concerned about the bottom face. For a vertical slot, I look at the functionality/stack to see which side is more critical (there always is one). That's the reality of physical assembly & function as opposed to design function. In both those cases, a profile control is more functionally accurate than a position control. I would probably use a +/- width to control the second face.

In the case of a V-block, the centerplane is established by both faces. In your proposal, there is a tolerance on the 45deg +/- 30'. There is also a tolerance of +/- 30' on each face as it goes into the page [y]. So, the derived median plane (not actually a centerplane if you use symmetry) may still be dead center, but the mating part being aligned by the slot may now deviate to either side [x] by +/- 30' ... in reality, it WILL be at the extreme in [+xy] or [-xy] because the inspector will set it up to minimize rock. As a result, your mating part will not ever be properly oriented wrt the intended centerplane.

Profile controls (composite perhaps, to refine the relationship between the two inclined faces) controls the location and orientation (and form) of the two faces wrt the datums and wrt each other. It is an indirect control on the centerplane, but far more repeatable and controllable.

As for inspection, using 4-5 sets of opposed points on the inclined faces for a symmetry control ... well, that doesn't tell you what the entire face is doing, does it. For the profile controls, you put a feature simulator (true geometric counterpart) on each of the surfaces and probe off of the simulator, giving you an accurate reflection of the net effect of the entire feature.

Plus, symmetry really sucks.



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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

Jim:

I agree that symmetry really sucks too but in this situation, I think it would work better than profiles. This is the first time that I have seen a symmetry application rather than using positional. It depends upon the Designer in this case. Is the Designer really interested in the surfaces of the V or the derived center plane? The original drawing indicated the relation between the actual center plane of the feature and the datum.

Dave D.

http://www.qmsi.ca

 

[MechNorth]

There are times that we have to do things indirectly in GD&T; to me, this is one of them. I do understand your reasoning, I just don't support it because of the overwhelming issues that I anticipate with using symmetry.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com