GD&T Basics and True Position Conversion Charts

[rhmeng]

I have two mating parts, Part A and Part B. Lets for example look at the #1 tapped features (circled red part A). To calculate out the diametrical positional tolerance, I took the thru hole of Part B (.081) subtracted the OD of the #1 screw (.073) and divided by 2 -> (.081 - .073)/2 = .004. I used .004 for both the tapped feature and the thru hole. My understanding is that now, the tapped feature has a a diametrical tolerance of .004, so the center is able to move in any direction by .002" (the radius in the positive and negative direction).

I was talking to a machine shop who told me thats not true, and that you divide the diametrical tolerance by the number of datums so you only get (.004)/(3 datums) = .0013" in each direction. He also told me I should get a true position conversion chart to help me out. I googled this for a while and could not find anything relevant.

Does this sounds familiar to anyone? I thought i knew what was going on when it came to tolerancing holes/virtual condition/ etc, but maybe not. Thanks in advance.

 

[pmarc]

I was talking to a machine shop who told me thats not true, and that you divide the diametrical tolerance by the number of datums so you only get (.004)/(3 datums) = .0013" in each direction.

That is the most absurd GD&T-related thing I have heard for a long time. The number of datums has nothing to do with the available amount of geometric tolerance specified in a feature control frame.

Looks like the positional tolerance values circled in red were calculated using fixed fastener formula as given in Appendix B.4 of Y14.5 standard. One thing to remember is that this formula works well if projected positional tolerance zone is defined for the component with tapped holes. Since that is not the case for part A, the positional tolerances (or at least one them) should be further tightened to assure that the parts will always assemble. A formula given in Appendix B.5 could be used for that purpose.

 

[CheckerHater]

Very little can be added to what pmarc has already said.

It is possible not to split available tolerance exactly in half (.004 and .004) but to make one of the tolerances tighter (.003 and .005 for example).
This is usually done to accommodate shop capabilities, etc.

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[KENAT]

Your machine shop is not using any method I'm familiar with.

For fixed fastener case subtracting max major dia of fastener from minimum diameter of hole gives you the position tolerance budget to share between the threaded & clearance hole - which appears to be what you did. ASME Y14.5M-1994 has this equation as an annex, B4 from memory or around there.

(BTW, often times it may not be the best use of this tolerance budget to split it equally. May be beneficial to give a bit more of the budget to the threaded holes and less to the clearance due to the relative ease of locating those features during manufacture.)

I'm trying to think if they are trying to 'square the circle' or some such but not sure it's that as it would give +-.014 in X & Y for your case.

Posting guidelines faq731-376

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

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

 

[rhmeng]

@pmarc, CheckerHater, KENAT
Yea I was a little confused with what he was saying also, but it was said in such a "matter of factly I have been doing this since you have been born" tone that I thought I was wrong. I will bring it up again and see if I misunderstood, but thats what he told me. I often do unevenly split tolerances however thanks for the tip, i will update as necessary thanks for all the input.

 

[KENAT]

Technically pmarc is correct about the projection aspect.

However, 'worst case' tolerance analysis tends to be a little conservative so for relatively thin parts I don't normally oversize the holes or add projection. However, if the parts are thicker, or the tolerances tighter or.... I will add it.

Note - This is on low volume stuff I currently deal with in a commercial setting, I might do differently for true high volume or govt work....

Posting guidelines faq731-376

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

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

 

[mkcski]

This may have been overlooked and is not directly related to the question; I note that both FCF's on Part A have the same sequence of datums. This invokes Simultaneous Requirement conventions per Y14.5-1994, para 5.3.6.1, i.e. all (8) features are a single pattern.

 

[rhmeng]

This may have been overlooked and is not directly related to the question; I note that both FCF's on Part A have the same sequence of datums. This invokes Simultaneous Requirement conventions per Y14.5-1994, para 5.3.6.1, i.e. all (8) features are a single pattern.

I looked up this Simultaneous Requirements, and I am not exactly sure how it is relevant or how to apply it in this situation. The Datums themselves on Part A do not have geometric tolerances or requirements applied to them, so I dont know if that matters or not?

 

[CheckerHater]

All 8 features cannot form a sigle pattern, because they belong to 2 different parts

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[mkcski]

CH:

I agree completely. But I was taking about the two patterns on part A only, one of which is NOT circled.