I need help with threaded/clearance positional tolerance. 2

[preecher]

I have a threaded hole and a clearance hole in two parts that are to be bolted together. The clearance hole diameter is roughly .031" larger than the bolt nominal diameter. I've told the designer he should use Ø.010mmc tp for the clearance hole and Ø0.020mmc tp for the threaded hole, thinking that the threaded hole would be more difficult to hold tighter than the clearance hole and that measuring the threaded hole is more difficult. However, the designer is also being told (by another) to reverse those tolerances. I don't want to cause problems, so I want to know if there is an manufacturing rule of thumb or standard that would indicate which way the tolerance imbalance should fall.

 

[EngineerTex]

When you state "Ø0.010mmc tp", are you meaning:

a) The location of the theoretical centerline of the hole is within 0.010 inches of true position?
or
b) The hole diameter wall resides within an annulus where the minimum material condition (mmc) is nominal diameter + 0.010 inches and the maximum material condition (MMC) is the nominal diameter?

I could be missing something, but I don't think either of these will work. The true position of the holes is such that the edge of the clearance hole is 0.0155" away from the (theoretical) "edge" of the threaded hole (0.031/2). If the clearance hole is moved in the +x direction a distance of 0.010" and the threaded hole is moved in the -x direction a distance of 0.020, you have an issue of a clearance hole which partially obstructs your threaded hole, yet each falls within tolerance.

Engineering is not the science behind building. It is the science behind not building.

 

[lumenharold]

Perhaps a GD&T calculator would be helpful:

http://www.engineersedge.com/calculators/fixed_fastener_pop.htm

Harold
SW2010 SP1.0 OPW2010 SP1.0 Win XP Pro 2002 SP3
Dell 690, Xeon 5160 @3.00GHz, 3.25GB RAM
nVidia Quadro FX4600

http://www.lumenflow.com

 

[ewh]

EngineerTex,
I have to disagree. While you halved your TP tolerance, you neglected to halve your offsets. The scheme will work as originally presented.
I agree with preecher that it would be preferable to use the larger TP on the threaded hole, as more effort is required to fabricate it than would be a simple clearance hole.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[ewh]

For a more thorough analysis, try posting the question here --> forum1103

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[KENAT]

When possible giving the thread some extra position tolerance is better as there are more steps in making a threaded hole so more tolerance build up, and they're unable to take advantage of MMC (except for certain fixed gage situations).

I can't think of any applications of simple hole patterns where I'd put less tolerance on the threaded holes than the clearance ones but there may be some functional logic not apparent in your post.

I posted a calculator over in GD&T thread1103-221602 (4 Sep 08 3:26 version) based on appendix B of ASME Y14.5M-1994, not sure you need it though.

Posting guidelines faq731-376

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

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

 

[drawoh]

preecherm,

I am not aware that threaded holes are harder to locate than through holes. I am not a machinist, so I could be wrong.

I question your use of MMC on your tapped hole. Specifying MMC tells the fabricator that if their hole is oversized, they can open up the positional tolerance, accordingly. Tapped holes are accurate, and screws are self-centreing. The "bonus" tolerance does not exist. This has been discussed at some length in the dimensioning and tolerancing forum.

The major diameter of your tapped hole plus the positional tolerance of your tapped hole, equals the minimum acceptable diameter of your clearance hole located exactly at true position. You can call this value up with a positional tolerance of zero at MMC. The plus tolerance of your hole diameter should be generous. At the very least, add the tightest positional tolerance your fabricator can achieve, to the tightest plus tolerance your fabricator can achieve on the hole. You will not be getting the minimum diameter. I like to do this on my drawings.

If your feature size is accurate compared to your positional tolerance, MMC does not provide your fabricator an opportunity to save you money. If you can specify MMC, you can tighten up the positional tolerance.

JHG

 

[mfgenggear]

I concur with Drawoh.
with today’s CNC equipment threaded holes can readily be machined. yes the time & material is higher. but the accuracy of cnc equipment is there.
the Inspector should use threaded pins to locate
the position of tapped holes using a CMM. no MMC should be RFS.

To my opinion the threaded holes should be as tight as the
clearance hole, Because it sets the position of the threaded fasteners. just my personnel opinion.
Reason is that the fastener will be at a projected height
so there is potential the fasteners will be slightly skewed.

MfgEngGear

 

[KENAT]

So my justification for giving a bit more tol to the threaded hole when possible...

Creating the threaded hole is typically a multi step process. First you have to drill a tap hole - which simplistically I'd assume has similar process capability as the mating clearance hole from a tolerance point of view.

You then have to tap the hole, while the tap will follow the hole it may wonder a little bit - or so I've come to understand.

Finally when you come to inspect the hole you can't generally take advantage of the MMC like you can on the typical clearance hole.

MfgEngGear makes a good point about the projected height of the fasteners that go in the holes, however I'd hope the OP has taken care of this either by over sizing the clearance hole accordingly (ASME Y14.5M-1994 annex B shows how to do this), using a projected tolerance, or maybe just accepting the risk and using up some of the generally over conservative 'worst case' tolerance budget.

Obviously a lot will depend on what your tolerance is. The OP tolerances aren't that tight - hitting dia .010 pos with a threaded hole shouldn't be much of a cost driver. Also I don't know what the OP's tolerance on the clearance hole diameter. However, without knowing more I might suggest a rule of thumb 60%-40% split in favor of the threaded hole, so maybe .018 for the thread and the rest on the clearance.

Or, if your machine shop quotes the all to familiar "+-.005 tolerance for holes tighter will cost you" then throw .014 on the clearance hole and the rest on the threaded hole just to keep them happy;-).

Posting guidelines faq731-376

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

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