Threaded Hole Position Tolerance

[BfdDan]

I am a new engineer and am working on a project and am specifying the location of 3/4" ANSI Standard Hex bolts and need to know how to tolerance the position of the holes with respect to eachother, i.e. I have four bolts in a rectangular pattern. If anyone knows a good source for this type of information I would appreciate it.

Thanks,

Dan

 

[dimjim]

Basically, subtract the bolt hole diameter
from the minimum hole diameter and divide
by two. This would be the true position
tolerance on each set of holes. Normally
shops can do better than this and you might
want to tighten up the tolerance. This is
a general guideline.

 

[handleman]

This is usually built in to the standard fabrication tolerances. It's not common to call out a tolerance on the location of either tapped holes or their corresponding clearance holes for the bolt. The difference between the actual OD of the bolt and the ID of the clearance hole (usually a bit more than 0.78 for a 3/4 bolt) make up for anything but a gross hole positioning error by the fabricator. If you use standard taps and clearance hole drill sizes and end up with parts that won't assemble then you should probably look into getting your parts made elsewhere.

 

[lumenharold]

You might try:

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

or there might be an answer over at the GD&T forum:

http://www.eng-tips.com/threadminder.cfm?pid=1103

Harold
SW2007 SP2.0 OW2006 SP4.0

http://www.lumenflow.com

 

[dimjim]

If you are going to use simple dimensions
between the holes, .70 times the values
that I mentioned earlier would apply for
a rectangular tolerance. Then use 1/2
of that value for the plus and minus
tolerance value on the dimensions between holes
which would be a rectangular pattern
inside of a circular tolerance.
For example: if the holes were .78 and the
bolt .75 would give you a difference of
.030. True position tolerance would be
.015 and the give you a plus and minus
.0105 on the dimension between holes.

 

[winpop123]

I would specify hole size as .906 to .926, reference "Clearance Holes for Bolts, screws and Studs - ASME B18.2.8-1999.

Using bolt size at .75 - min hole at .906 you have .156 to play with. You could then allow +/- .060 positional tolerance and you would still have some margin.

All that being said it also really depends on your industry, who is making the parts on what kind of machines, or is it being drilled in the field etc. Hope this helps.

 

[ewh]

It definitely depends on the industry. I have come across very few hole patterns that were not positionally located, often simply for the "bonus" tolerance area provided, other times because location was critical.

 

[israelkk]

dimjim

"For example: if the holes were .78 and the
bolt .75 would give you a difference of
.030. True position tolerance would be
.015.."

This is true only if the holes positions are known with absolute accuracy. However, the holes too has positional errors that should be taken into account when specifying the bolts true position tolerances.

 

[KENAT]

If you want to do it properly (assuming you have 2 parts joined by these holes/screws) use positional tolerance as others above have explained.

If you want to half ass it (as is standard in many areas of industry) then use some of the other approaches given.

More seriously though what type of industry are you in, this will affect which option you take. Try and ask colleagues how your company normally deals with it (do they use GD & T or should they) or at least try and look at other drawings with similar features.

We prepared a table at my place based on information ( a chart) in machineries handbook but modified to suit our purposes.

Looking at our chart for 3/4", for what is termed Normal clearance then for 'floating fasteners' (ie both items just have clearance holes) suggested hole dia is .781 +.010 -.002 with positional tol of diameter .029.

We also have a close clearance for more precise applications. .760 (think it should be .766) +.010 -.002 with .014 pos tol.

I'd take a look at the GD&T forum.

 

[KENAT]

I am an idiot.

Looking at the title of your post you clearly state threaded hole.

As such assuming you can dimension the other part to suit you need to halve the positional tolerance I gave above.

If you only have control over the threaded item you need to do the calcs explained by others above.

http://www.draftingzone.com

may help.

 

[gfbotha]

Thinking about what tolerance to specify, also just keep in mind to accurately inspect such threaded hole positions is another real issue...

One way is an indirect method by screwing in bolts/studs with an unthreaded shaft. But if such studs are not perpendicular with the work, it will again lead to inaccurate measurements.

So, do not go too fine.

 

[stick1]

We call out the true position relative to the minor diameter. That way a standard gage pin can be used to represent the hole position. Just add "Minor Diameter" below the G,D & T feature control frame.

 

[BfdDan]

Thank you for all the responses, they have been helpful. Being new to this site I will provide a little more info on my line of work. I work for a small manufacturing company that rolls steel products. Our engineering dept consists of my self (grad. 2004) and on other 2005 graduate. Up until now, everything I designed has been built in house by our toolroom/maintainance dept. That makes it easy, I basically give them the concept, a few simple drawings and they get it done. That was the past year. Now I am starting to go to outside tool shops to manufacture my equipment. This is where the tolerancing became an issue of concern. I am sure I will use this site more and more in the near future!

Thanks again, Dan

 

[gfbotha]

Dan, it's completely optional but should you like, you could also go to Personal Profile and enter any personal info, interests or experience for others to see.

Cheers

 

[GBor]

Dan,

Get a copy of ANSI Y14.5M and/or an equivalent DoD specification. If you don't put ANY tolerance on the drawing, it doesn't mean that the fab shop can just put it wherever they want...there are standard tolerances.

I teach a class on CAD drawings, but I'm also an engineering consultant. The unfortunate reality is that tolerances are specified however people feel like it most of the time...few follow the "right" procedures. James Earle has an 11th edition of his book Engineering Design Graphics that has a great chapter on tolerances (chapter 21). It may be worth a purchase...

For your hole positional tolerances, you have a symbol (looks like the cross hairs through a scope), a tolerance, an indication of whether you are using "maximum material condition", "least material condition" or something regardless of feature size, you may use a datum plane or two for reference and that would have to be indicated, but all of this is only if it falls outside of the standard tolerances. You need to specify which standard you are following...the fab shop will have to know the standard.

My 2 cents...

Garland

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group

 

[KENAT]

Definitely get ASME Y14.5 (assuming you're in the US). Looking at that and some of the resources mentioned you should be able to get a pretty good grasp of positional tolerancing and how to specify it. For some of the other GD&T you'll probably need some training of some kind. You're unfortunate in that it doesn't seem you have any more experienced guys to learn from at your employer.

If you don't put ANY tolerance on the drawing, it doesn't mean that the fab shop can just put it wherever they want...there are standard tolerances.

GBor this isn't my understanding. While certain sections of industry have their standard tols I don't think that would apply here. Even if you reference 14.5 that doesn't actually give any tolerance values. As a minimum you need to either reference a spec which does gove tolerance values or have a 'block' tolerance on the drawing.

 

[GBor]

My bad, KENAT, I didn't mean to imply that there is some universally accepted tolerancing or even some industry accepted unspoken rule, but no tolerances on a drawing technically means no latitude for error. Obviously, this is a physical impossibility in the real world, but it does give a QA Right of Refusal if something isn't built properly.

 

[KENAT]

I think I understand you now, I thought one of us was loosing it for a minute though.