Help defining tolerance for true position radial holes

[john654321]

Working on a part that has radial holes in a cylindrical part. Hole location is (.014(M)/A/B(M)/C. C is not used on the part, A is the end of the part or the flat of the cylinder so that would be easy enough, B is actually the center of the part defined by one of the diameters of the part. The diameter for the B datum is not the same surface for the radial holes. I am trying to determine actual radial misalignment tolerance. There is no callout for angle tolerance specifically yet there is an angle location for the part.

The angles are all boxed. I understand MML just fine but I do not think I get any leadway on the MML because this is a threaded hole. .014 true position is a tight tolerance. Is there any other way to get more tolerance with this callout?

 

[john654321]

EDIT, C datum on one part is not used or called out. On one part it is an edge or plane but not one that drives the radial geometry.

 

[john654321]

Also, the angles that define the location for the holes are boxed.

 

[KENAT]

John, the 'boxed' basic angle combined with the presumed other dims is giving the theoretically perfect location. The position tol is then applied to this. That is why there isn't an angular tolerance as such, it's in the position tol.

Pos tol dia .014" is not that tight for a machined part, it's roughly equivalent to +-.005".

The MMC on B is giving you some more tolerance.

I suggest you post a sketch of the tolerancing scheme etc as a picture really can paint a 1000 words when it comes to this type of thing.

My original response:

http://files.engineering.com/getfil...7c3170&file=Help_with_GD&T_interpretation.mht

Posting guidelines faq731-376

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

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

 

[KENAT]

Oh, and what drafting standards are you working to, not sure on this one but sometimes it makes a difference.

Posting guidelines faq731-376

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

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

 

[KENAT]

MHT file won't upload properly so here's what I put before.

john, could I suggest you repost with a sketch over in forum1103: Drafting Standards, GD&T & Tolerance Analysis

It seems like there are errors either in the drawing or your interpretation or both.

When you say B is 'the center of the part' do you mean the datum feature is the outside cylinder and datum B is the centerline of this?

The B(M) is giving you some more tolerance. You're right that you don't get a lot from MMC with threaded holes except for certain types of gauging which I wont claim to fully understand.

http://www.tec-ease.com/tips/june-03.htm

Are you sure C isn't one of the holes or another feature to give you angular orientation.

The angles should all be boxed when used with position, they have to be basic.

.014 is not that tight of a tolerance, it's about +-.005 equivalent. I'd generally expect this to be able to be achieved with most threaded holes without too much difficulty on machined parts - though I'm not saying there arent exceptions.

Posting guidelines faq731-376

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

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

 

[john654321]

Unfortunately I cannot post any info on the part because it is aerospace and do not need any concerns over confidentiality. I think you are on the right track with the hole location but I am trying to figure if this is possibly a chordal length, or an arc length.

I realize .014 is not that tight but there are other factors playing in that will make holding that tolerance tougher.

One of the big questions is how MMC might play in on the B datum to add more tolerance. Possibly TIR?

 

[john654321]

OH, this is the ASME 14.5 standard

 

[KENAT]

I didn't say post the drawing, just post a simplified sketch with the relevant info.

For how B(M) may help you take a look at section 5.3.2.2.

5.3.5.2 is an example of radial slots which might help your chord/ard (I believe chord since you're worried about the centerline of the holes).

Fig 5-24 on has a pattern or radial holes but it's really a composite position example so might cause more confusion than is worth it.

Posting guidelines faq731-376

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

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

 

[KENAT]

Paragrahs above are ASME Y14.5M-1994, is that the year you're using?

Posting guidelines faq731-376

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

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

 

[Belanger]

Per 5.3.2.2 -- The M symbol on datum B is often confused with the M shown after the number. While that first M symbol may provide extra "bonus" tolerance on each individual hole, the M symbol after the B indicates that there may be allowable "slop" or shift around that datum feature. This could translate into extra tolerance for the holes, but NOT on an individual basis; rather, it allows the entire pattern to shift slightly. But it all depends on how datum feature B is manufactured.

You mentioned TIR. I don't think that would come into play at all with your callout. That's because TIR feels the actual surface, and will detect any form error. The GD&T that you mention will have no bearing on the form, so I would avoid the TIR business.

Kenat has lots of good info above, but I hope that helps too!

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