Perpendicularity of a flange surface to a bore ID datum

[dstokesag]

I have a very large flange part that has a 0.05mm perpendicularity callout to Datum -A- which is an ID bore diameter that is also very large and only about 21mm in depth. We setup a CMM program to inspect the part and depending on how many inspection points we put on this surface we can get whatever reading we want (Mitutoyo CMM is not equipped with a scanning head). So have a few questions here:
What is the proper number of inspection points and programming method (have PCDMIS software) for checking perpendicularity on a point style head CMM type machine for this type of check?
How do you set up the axis of Datum -A- if it is so short in land to ensure you have the true axis of Datum -A- established to take a good reading of the surface (again what is proper number of inspection points etc.)?
What would be the proper inspection method using a surface plate and indicator to do this open plate layout check and calculate the perpendicularity instead of using a CMM?

Thanks,
DS

 

[Belanger]

Not sure about programming PCDMIS, but to answer your last question about manual inspection ... An easy way might be to mount datum feature A (the ID) on an internal chuck or expanding mandrel such that it can rotate. Then rig a dial indicator to be exactly 90º to the axis of rotation. As the part rotates, move the dial indicator along that flange surface in any and all directions, and the total indicator deviation shall not exceed 0.05.
What I've described is called total runout, but it's identical to perpendicularity for the flat surface, if I'm picturing your requirement correctly.

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

 

[ModulusCT]

I agree with belanger. Rotating part however is not entirely necessary. You could just move the indicator manually yourself. The idea that you must cover the entire surface (or nearly so) is correct.

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

 

[pmarc]

What is the proper number of inspection points and programming method?

The most obvious answer is - the more points the better, but I don't think this is the one you are looking for.
I am pretty sure different companies have different policies and take different approaches. In the attachment below you can find an excerpt from "CMM Measurement Strategies" guide by National Physical Laboratory. They, for example, refer to BS7172:1989. They even have special formulas for calculating how many measurements planes and how many point in a particular measurement plane should be considered when probing a cylinder.

http://files.engineering.com/getfil...f-86dc-63caf12be9d4&file=cmm_cylinder_NPL.png

If we are talking about IDs, from theory standpoint the datum axis should be the axis of a maximum cylinder than can be inscribed within the probed contour. If the ID is primary datum feature, this maximum inscribed cylinder is unrelated to any datum. If the ID is secondary or tertiary datum feature, the maximum inscribed cylinder must be oriented and/or located relative to higher precedence datums.

How do you set up the axis of Datum -A- if it is so short in land to ensure you have the true axis of Datum -A- established to take a good reading of the surface (again what is proper number of inspection points etc.)?

This is great question. In 99% of cases I have experienced, such short features (short comparing to the size of part) do not really function as primary datum features. In other words, they do not orient part sufficiently to be named primary datum feature in any geometric callout. Moreover these features do not produce repeatable datums.

Without knowing all the details of the part (its mating relationships in the assembly) it is hard to give good answer, but perhaps it is the face of the flange that should serve as primary datum feature, and the ID should be controlled relative to datum plane derived from that face (through perpendicularity callout). Then the inspection should go quite smoothly.

As for optional inspection methods, what J-P (Belanger) suggested will work provided that the part can be repeatably fixed in the chuck or mandrel. Due to short length of the ID this may be difficult to satisfy, that is why usually in such cases, when runout is verified, a planar feature (perpendicular to the datum axis) is defined as primary datum feature, and the cylinder becomes secondary datum feature. This stabilizes the part and enables repeatable measurements.

 

[greenimi]

Pmarc,
Quote: “If the ID is primary datum feature, this maximum inscribed cylinder is unrelated to any datum.”

Is the maximum inscribed cylinder above the same with unrelated actual mating envelope?
IS there any difference between them?


And one more question: IF perpendicularity is called at MMC then how the bonus is calculated? (something like the difference between the actual mating envelope or the maximum inscribed cylinder –IF they are the same-- and the MMC size, my best guess)

Thank you

 

[pmarc]

greenimi,

1. There is no difference between the maximum inscribed cylinder and the unrelated actual mating envelope of internal feature of size.

2. Yes, you are correct. When perpendicularity is called out at MMC, bonus tolerance is the difference between size of UAME and the MMC size of a FOS (if we think about internal FOS).

 

[dstokesag]

Okay additional question now. The flange face has typical profile or flatness error of the surface. This error increases the perpendicularly error the more points you add when checking the face. So am I correct in statin that you cannot subtract your profile or flatness error from your perpendicularity measurement or can you?

 

[pmarc]

If I understand your question properly, the answer is following:
By default you cannot subtract form error (profile, flatness) from orientation error (perpendicularity). There is a way to override this - by using tangent plane modifier (T in a circle) after tolerance value in the perpendicularity feature control frame - but as far as I see this is not the kind of callout you are dealing with.

If you have access to Y14.5 standard, check out fig. 6-18 in 2009 version, or fig. 6-43 in 1994 version.

 

[dstokesag]

Thank you pmarc for this clarrification and that is what I thought. I opened your attachment for the number of points for a feature with the calculation and have a question in the example. What is "N"? I see the radius as "r" and the height of the cylinder "h" but don't know where they are getting "N" from. Please explain and do you have an example like the cylinder for calculating the number of points for a plane or do people typically just use the 9 (Approximately three lines of three)?

 

[pmarc]

It looks like they selected N=30 (total number of points) just like that.

There is one more thing I did not show in that attachment:
Note: It is beneficial for the number of points to alternate between odd and even on the circles, viz., in Figure 23 above seven points on the first circle, eight on the second, seven on the third, etc. This choice will enable any lobing effect on the circular cross section to be detected.

Below you can find 2 more pages from the very same document where probing strategy for planes is described:

http://files.engineering.com/getfil...44f7-9791-9520ead18952&file=cmm_plane_NPL.png

 

[dstokesag]

Please explain what you mean by they selected N=30 just like that?
Also my part is a circular flange not a square plane (OD is 406mm and ID is 311.61mm so the width of the flange is 47.195mm) The flange has 16 10.5mmdiameter holes on a 387.35mm bolt hole pattern). So the square plane number of points sheet won't work for me. Is there some other number of points sheets that tells you on a flange surface the number of points you can send me?

Thanks,
DS

 

[pmarc]

By "just like that" I meant they did not explain why they selected 30 and not 40 or 10 for example (at least I could not find such info).

Also, this document does not offer anything when it comes to circular surfaces, but does it really have to? The message is following - to achieve more or less uniform distribution of points, divide inspected surface into smaller fields (more or less similar in size and shape) and place at least one point in each field. I think this is doable also in your case, but of course the fields won't be square or rectangular (see another attachment).

http://files.engineering.com/getfil...db1-8cb9-24229f0eb8fb&file=flange_probing.png

 

[dstokesag]

Okay this is great but I still don't know what big N is to figure out what it is for my part to do the cylinder. Any other ideas as to where I can find that?

 

[MikeHalloran]

3xx mm is not 'very large' in some circles.
Nevertheless, a very short bore like that is a terrible primary datum. I am assuming you are not the design authority and cannot change the drawing, so..

The old school way to use that bore as a primary datum is to machine a tight-fitting plug to push into it, and spin that plug on a stem or face machined into it in the same setup.
... while bitching continuously about the designer's skill set, of course.

I am not aware of any property or technique associated with a CMM that can make consistent measurements easier or faster, given such an unfortunate dimensioning scheme.




Mike Halloran
Pembroke Pines, FL, USA

 

[3DDave]

Pick increasing values for N until the variation in the result is smaller than some amount. As long as you don't move the part on the CMM you can just keep adding points and determining the axis, avoiding starting all over. If it's a manually positioned CMM there's going to be a lot of effort.

21* (.05/406) is the amount of axis variation that would entirely consume the perpendicularity tolerance. You'd want to lose no more than 5% -> about .0001 to repeatability error or less. Confirm this with the drawing in hand.

If it is hard to determine if the part passes, then that's unfortunate for the part function in the next assembly as it will likely not act properly there any better than in inspection.

 

[jflongwell]

Why is the axis primary? Make the flange primary with a control applied (flatness, profile), and the axis secondary. The tolerance zone for the flange would essentially be equivalent.