Diameter Callout 1

[GTFiji]

This question almost seems too simple to post, but here it goes.

I have a diameter callout on a drawing that is preceeded by the diametrical symbol. The dimension with tolerance is 80.0 +/-0.15 mms. Is it acceptable to measure this dimension via CMM by taking a large number of hits around the perimeter (ie 50 or more) and then letting the program calculate a best fit diameter using those points to answer the callout? Is there a "standard" method driven by the callout?

Thanks.

 

[KENAT]

What drawing standards are you working to as it may make a difference, ASME Y14.5M-1994, ISO or some other?

KENAT, probably the least qualified checker you'll ever meet...

 

[GBor]

Are you asking about how to QA this dimension? If so, 50 points on a CMM is overkill...3 will generally do; 4 is better. The CMM should give you nominal diameter and error.

 

[GTFiji]

The drawing standard is ASME Y14.5M-1994.

If I use a CMM and average a "number" of points the program reports a best fit diameter as the answer. In this case, assume I take 25 hits and the CMM calculates 79.95mms. In tolerence (80.0 +/-0.15 mms)!

I can then take calipers and measure a "high" and a "low" around the diameter and at a given section I measure 79.80!

Does this part meet the drawing tolerance????

 

[drawoh]

GTFiji,

If any dimension across your part reads 79.8, it does not meet specification.

How thorough do you want to be, and what errors do you anticipate? This problem is complicated because you have a diameter error and a positioning error, both of which will be visible to the CMM. If the diameter matters to you more than the position, perhaps you should fabricate a go-no[ ]go gauge.

I would think that the three point measurement suggested above, would be a good way for a CMM to test the position of an accurate, round diameter. Just like a series of calipre measurements, three or four point measurement can fail to detect a non-round form.

With 50[ ]points, you can plot them, and superimpose the maximum and minimum circles on them. I am sure there is a way to do this in 2D[ ]CAD. How much effort are you willing to go to?

JHG

 

[powerhound]

Using the average diameter will not give you a best fit scenario. ASME uses material boundaries to determine fits whereas ISO uses averages to determine whether or not the part is good; which is useless as far as I'm concerned. The only size pin that will fit into a hole is a pin with the same diameter as the smallest calculated dimension. The average size serves no purpose. While 50 hits may be excessive, it will give you a better idea of what the actual size of the smallest circumscribed cylinder is than 3 or 4 hits will.

If you work at a machine shop, have someone turn a pin that is 79.85 on one end and 80.15 on the other. This will be a quick GO/NOGO gauge that will work.

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[drawoh]

powerhound,

I think the correct go-no[ ]go gauge would be a barrel Ø79.85, with a pair of small ears at one end to measure Ø80.15. You would have to try the no[ ]go gauge at multiple angles, all of which should not allow the gauge.

A no[ ]go gauge tests only one feature at a time.

JHG

 

[GTFiji]

Thanks for the responses. I am going to try and ask my question in another way to try and better explain my issue!

The diameter I am dealing with is an outside diameter. The inspection method was to take hits around the O.D. with a CMM and then the program does a best fit of all the data and gives me an answer. Although my answer is in tolerance due to the best fit method I know that my round plastic pipe is really egg shaped. If I measure with calipers in one direction I can find an area where the diameter is too small (under the bottom edge of tolerance).

My question is am I in spec. based on the callout and measurement technique (best fit of points)? My feeling is that my technique is correct based on the callout and I report it in tolerance. If I want to control the "egg shape" then I need to add a roundness callout.

OR

I am really simply out of tolerance because the caliper method in one place only IS applicable to this callout.

 

[KENAT]

Take a look at section 2.7 Limits of Size in 14.5. Within the limits of the tolerance you have some control on 'egg shape' with ANSI dimensioning. With ISO you'd need the extra control as I understand it.

Powerhound & drawoh are better at this than I but the fact you measure below the min diameter at one point would make the part out of spec as I understand it.


KENAT, probably the least qualified checker you'll ever meet...

 

[drawoh]

GTFiji,

ASME Y14.5M-1994 Individual Feature of Size (Rule[ ]#1.) Where only a tolerance of size is specififed, the limits of size of an individual feature prescribe the extent to which variations in its geometric form, as well as size, are allowed.

Basically, you have two concentric circles Ø79.85 and Ø80.15. The outline of your part must be within these. If you can measure a diameter outside of these with a calipre, your part does not conform.

It sounds to me like best fit method does not describe an out-of-round shape effectively.

JHG

 

[axym]

It's amazing how complicated a "simple" thing like diameter can get, when form error rears its ugly head.

As was mentioned earlier, ASME Y14.5M-1994 has something called Rule #1 (a.k.a. the envelope rule, a.k.a. perfect form at MMC) as the default for size tolerances like diameter. There are two requirements that have to be met. One is that the feature must fit through an imaginary boundary of MMC size. The other is that the "actual local sizes" must all be within the specified limits. For the pipe OD example, you would need a precision bore of diameter 80.15 mm, at least as long as the part, to verify the boundary requirement and a mic or calipers for the local size requirement.

The "best fit" size that the CMM gives you is based on a least squares fit algorithm. It's kind of an average diameter, that unfortunately doesn't match either of the two requirements! The Minimum Circumscribed Cylinder algorithm, if available, would be the one to use for the boundary requirement on an OD. For the local size requirement, you would have to take a series of opposed point measurements and verify that they are all within the proper range.

A consequence of Rule #1 is that there is an indirect form control. If the feature passes both the boundary requirement and the local size requirement, all of its form characteristics will be controlled to a value equal to the size tolerance. For the diameter tolerance of 80 +/- 0.15 mm, the size tolerance is 0.30 mm. So the circularity, cylindricity, surface element straightness, and derived median line straightness all get controlled to a worst case of 0.30 mm. So the size tolerance indirectly controls how much out of round or egg shape condition the feature can have. There can be an additional circularity tolerance to refine it further, but there doesn't have to be.

If one of the caliper measurements came out smaller than the lower size limit, the feature is nonconforming.



Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[GTFiji]

Axym,

Home run! You answered my question precisely!

Not the answer I wanted to hear but great info!