hole sizing chart

[winpop123]

O.K. heres the dilemma. I'm trying to convince a bunch of knuckle heads that our tolerances aren’t "too tight". The situation is such that we are dealing with a bunch of fabricators that don't have outstanding quality and our internal model shop has only been at this location a year. To further complicate matters "our" primary area of expertise is in electronics. Where that leaves the Mechanical Design Group is a bunch of people commenting on designs that have no idea what they are talking about.

As an example a common part we would need fabricated may be an aluminum bracket out of 6061 with couple of #10 bolt holes in it (part may be anodized). Dealing with a real machine shop, a .221 hole with an appropriate positional tolerance would not be an issue. In our case it is to the point that the hole has to be wayyyy oversized to account for the poor positional tolerancing.

Back to the original question. Can someone supply documentation for a "standard size hole chart" or other documentation relating hole sizes to positional tolerances and machine capability. Heaven forbid anyone here would believe an engineer or the Machinery Handbook.

Thanks

 

[griffengm]

winpop123,
If they do not have faith in Machinery's then it is unlikely they will believe any other source you propose. When faced with a similar proplem we opted to go with short slots. This reduced the effects of bend allowances and kept the assemblers happy.

Griffy

 

[Airmack]

winpop123,

ASME Standard "B18.2.8 - 1999 Clearance Holes for Bolts Screws and Studs" may have what you need. This covers "close", "normal", and "loose fit" holes for bolt sizes from #0 to 1.5" and M1.6 to M100.

As for the chart relating the positional tolerance, you could do a simple tolerance analysis...

1. Determine the bolt size and obtain the MMC condition for the major dia. of the bolt.
2. Determine the hole size: close, normal, or loose fit. Obtain MMC condition from the ASME standard.
3. The difference between the MMC dia. values of the hole (smallest hole dia.) and the major diameter of the bolt (largest bolt major dia.) will give you the maximum diameter for which the center of your actual hole must lie, with respect to the nominal center, and still have parts mate.
4. Apply GD&T to the hole positional tolerance with respect to the MMC of the hole size. This will allow the fabricator to positionally deviate more for holes that are not MMC and still allow parts to mate. The MMC deviation should be the (value obtained in #3) / 2.


Pop into a spreadsheet the values for bolts and holes and you could have a custom chart to fit your needs, I think. This chart would show the 'best' you could do to accommodate poor positional tolerancing and still have standard bolts/holes mate.

Feel free to correct me if I've missed something.

 

[winpop123]

I'll check out the standard, sounds like what I'm looking for. Right now I'm looking for more of a political tool than an actual functional tool.

We can run the numbers as required depending on the hole size but trying to explain this methodolgy to folks that are clueless to GD&T is an exercise in futility. I just want something in writing that gives credance to our choices for hole sizes.

Thanks

 

[drawoh]

winpop123,

The Machinery's Handbook has tables showing recommended clearance holes.

I also have the Mechanical Design Handbook, edited by Harold A. Rothbart, McGraw Hill books. This contains a table showing clearance holes and the recommended "True Position" tolerances.

How do they bugger up hole positions? When I was in college, I worked with a fellow student on an assignment to measure hole positions on a part we had drilled on a drill press and on a milling machine. My partner was a machinist, so he did all the drilling. The drill press holes were more accurate than the milling machine holes. We should have repeated the test with me drilling, but it did not occur to us. I cannot find my results, so I forget what the numbers are. I have inspected holes here at work, and I find them located within a couple of thousands of an inch. The real issue here is possibly that your shop needs to meet some sort of standards.

Sheet metal shops locate features to +/-.015" from a bend. I would be machining 6061, not bending it.

ASME Y14.5M-1994 shows the math for relating hole sizes to positional tolerances. You can assign positional tolerances based on your incompetent fabricators, but at some point, your holes get too large.

JHG

 

[winpop123]

ASME B18.2.8 was exactly what I was looking for!! Its perfect for the point I'm trying to prove. Using one of our recent drawings as an example I'm able to show that we were "forced" to make bolt holes larger than the ASME standard and its not the design team thats off their rocker its the suppliers/machinist.

Thanks again

 

[Cockroach]

I can sense your frustration, I've dealt with many "knuckle heads", maybe they're interbred...deep, deep south wise!

Listen, you can also dimension relative distances and hold a tolerance, say +0.01/-0.00, from a common hole. This typically works if your hole are drill thru 1/32" over thread sizes. You can easily use absolute dimensioning from a common datum line, but you need to be sure that with mating positioning in the same fashion.

This is a common problem with mechanical prints. It doesn't surprise me, your solution to over drill hole sizes is a typical solution. You can also send those "knuckle heads" to look for a "plate stretcher", you may get a live bite on that one! There's always one in the crowd.

Kenneth J Hueston, PEng
Principal
Sturni-Hueston Engineering Inc
Edmonton, Alberta Canada

 

[Tunalover]

winpop123-
It sounded like you were looking for "standard" size tolerances on drilled or punched holes.

If you're looking for "standard" clearance holes there's no such thing unless you wish to commit to the "standard" positional tolerances that come with them.

In my book the word "standard" and the word "tolerance" don't belong in the same sentence.
\



Tunalover

 

[arto]

there's also the "projected tolerance zone" for when the fasteners pass through a thick plate or flange. [keeps the cL's straight enough for the parts to fit]