Tolerances on Mech Drawings 9

[Metalguy]

Many years ago when I took a HS course in mech. drawing, the correct way to show dimensional tolerances was to have the same number for the + and - eg., if you want something between 7 and 9 in. long you used 8+/- 1 (I can't figure out how to get the + directly above the - here).

But the foreign co. (Italian) I'm working at has a weird (to me) way of showing them. They'll use anything from 7 +2/-0 to 9 +0/-2. They've even used (I am NOT making this up!) something like 6 +1/+3!!! This is not a small company, but a fairly large but old manufacturer of BIG equipment.

Anyone seen anything like this before?

 

[ivymike]

yeah, I see it all the time. check out ANSI standard limits and fits for examples (machinery's handbook).

There are plenty of reasons why you would want to use unilateral tolerances, but most of them come down to ease of reading or ease of checking. If you have a hole that's specified as x -0/+tol, and a shaft that's specified as x -tol,+0, then you can easily see that they will have, at MMC, an exact match in size.

 

[MintJulep]

Warning! rant.mode = true

8 +1/-1 is not necessarily the same as 7 +2/-0, or 9 +0/-2.

The problem with tolerances is that nobody bothers to consider the root of the word. Tolerance comes from tolerate. The whole point is to define how much ERROR from the ideal case can be tolerated by the design.

I often hear "Well the parts don't go together right because there was an accumlation of manufacturing tolerances." WRONG! The purpose of actually thinking about, and correctly defining tolerances is to ensure that the inevitable manufacturing ERRORS will not result in parts that don't go together.

rant.mode = false

 

[boo1]

Tpically the number listed is the target number. The tolerance gives the acceptable range.

See ANSI 14.7 for correct notation.

 

[gearguru]

The way how your Italian company shows the tolerances is nothing unusual in "metric" countries.
This way of tolerancing makes it easier for the designer do define the min. clearance/interference.
Say we have a shaft 50mm dia and we want a bore locate on it with the min. clearance of 0.1mm and the machining total tolerance for both parts 0.05mm.
The "metric way" to dimension it would be:
Shaft dia 50 +0.0/-0.05
Bore dia 50 +0.15/+0.1
Locating smallest bore 50 +0.1) on largest shafts (50 +0) shows immediately the min. clearance.
The dia 50 in this example links the two parts together - it is usually called the "nominal" size for both of them.
This tolerancing style probably originated in the ISO system of fits( like 50H7/g6), what is used for decades and simplifies design, manufacturing and checking (if used properly).
Again - the main reason for doing it is to give to BOTH parts the same nominal size and using the tolerances define the fit. And for the ISO fits - there are standard tools, gages waiting for the smart user, it means less expensive tha the "special" gages/tools if no standard is used.

 

[jackk]

ditto the previous posts, especially gearguru. I'm surprised Metalguy didn't mention tolerance designations like H7/g6.

One problem though is how do you represent the geometry with a tolerance (such as 50 +0.15/+0.1) with a CAD/CAM system?

Most CAD designers would model a shaft with the nominal diameter of 50. But this would be out of tolerance if the NC programmer only used the CAD geometry.

 

[MikeHalloran]

The one thing they don't teach in mechanical drawing is, "What's a drawing FOR?".

A sketch can tell someone what you WANT.

A drawing tells someone what you WILL NOT ACCEPT.

;---

Asymmetrical tolerances are a shorthand way of saying that you'd prefer the feature be at the nominal location, but the design can tolerate (there's that word again) more varaition in one direction than another.

;---

Symbolic tolerance ranges are a shorthand way of dimensioning a joint for a particular fit, without going to the bother of calculating the numbers for every joint. It makes a lot of sense, though I never got used to it.

;---

I've gone to the trouble of trying to include tolerances in CAD geometry. It doesn't take a very complex part to drive you crazy, trying to figure out which line is the one you want to snap to, connect, etc. The closest I've come in practice is to model tapped holes as a cylinder of the tap drill diameter, and clearance holes at their nominal drill size.

As for modeling a feature where the desired size is not on the nominal, i.e., the tolerance range does not include the nominal, I'm not sure what to do. If you model the desired size, you have to override the dimension to show the nominal on a print, and if you model the nominal, the programmer has to work more carefully. Either way is likely to cause an error sometime. Modeling the nominal is slightly less likely to cause production of bad parts, but overriding dimensions carries risks of its own.

On the other hand, the number of times I've toleranced a part like that could be counted on the fingers of one hand, and it confused the hell out of everyone who saw the print. If you want to know when your part actually hits the shop, that's one way to do it; the phone will ring for sure.





Mike Halloran
NOT speaking for
DeAngelo Marine Exhaust Inc.
Ft. Lauderdale, FL, USA

 

[Metalguy]

Thanks for all the good responses. looks like the company is doing things correctly.

 

[drawoh]

Metalguy,

My copy of Engineering Drawing by Thomas E. French, McGraw Hill, published 1941, shows +/+ tolerances. They describe the practise as acceptable, but not as clear as limit tolerancing. They discourage making the workman do arithmetic. That makes the practise legal here in North America at least back to WWII.

With CAD, there are several ways to model something to scale and apply dimensions and tolerances. The nominal dimension, max and min allowance format makes clear what someone did. If you are working on someone else's drawings, you could get a nasty surprise.

JHG

 

[gearguru]

Using the tolerances as metalguy asked about means, that the people using the drawings are properly trained. Unfortunately the US colleges do very little (if anything at all) to improve the situation.
For the CAD representation: in our company the models are always created using the mean dimensions (average between the upper and lower limits) even if they are dimensioned different way. This helps if the models are used for rapid prototyping or castings etc. Again - the drafter has to be trained how to calculate the mean dimension. In case of confusion - and ISO fits are confusing for most of them -they ask your truly...

 

[gearguru]

For those of you who need to "decode" some ISO metric fits withot looking in a book, here is the web address of the Fit Calculator. I mentioned it before, now I found the address.
Enjoy!

http://www.tecnologix.net/en/tools/passungsrechner/passungsrechner_v05.html

 

[spiritditch]

A useful site for ISO metric fits calculation was

http://www.tecnologix.com/en/tools/fset_.html

but the site closed down a while back.

Does anyone know any other similar sites out there?

 

[diamondjim]

I do not know if you are talking
about acad or not, but for some
reason in order to get the plus
sign to appear, I would enter
1.00000001 for the plus tolerance
and 1 for the minus tolerance.
Then it would show the plus and
minus in the tolerance in the
dimension.

 

[drawoh]

tchettle,

ISO fits are explained in the Machinery's Handbook. The ANSI fits are based on ISO tolerance values, and are also based on the Machinery's Handbook.

There ought to be a macro button on this site that automatically generates the reply "Refer to the Machinery's Handbook!".

JHG

 

[unclesyd]

I don't have Acad but in some cad programs you can enter Alt 241 and get the ±.

 

[Cockroach]

UncleSyd, in AutoCad (any version) the command stroke on the keyboard is simply %%P. Back in the day, AutoCad Version 8, keystroke entries where the norm. I guess it just got built into the code somehow.

There are a ton of them, %%C for the diameter symbol, %%D for degrees, the list goes on.

I gotta admit, I never heard or seen +/+.

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

 

[Tunalover]

I heard someone say that the drawing needs to minimize how much arithmetic the fabricator has to do. NO! That is part of the fabricator's job and it is expected that he will have to do it.

An engineering drawing exists for depicicting the end-item; if a dimensioning and tolerancing style emphasizes the end-item's functional requirements while requiring the machinist to do some calculations then that's OK.

The drawing is an ENGINEERING tool that is used for inspection and for clearly protraying the end-item's functional requirements.

To be fair, though, the draftsman should never go out of his way to make a drawing that requires the machinist to figure things out!




Tunalover

 

[ctopher]

I agree tunalover!

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
ctopher's home site

FAQ559-1100
FAQ559-716

 

[drawoh]

tunalover,

I was quoting my 1941 drafting book. I collect old books, especially engineering and history.

The book actually is correct in the context of their discussion. If I am working on a drafting board, the clearest way to express a tolerance is to show limits...

1.253/1.251 DIA

This is as clear an instruction as you can send to a fabricator, and it meets engineering requirements.

In my next paragraph, I was somewhat vague, but the point is that with CAD, we use the scale drawing/model, and there are several ways of causing the display above. This could be nasty if your job is to model and dimension the mating part.

1.250 +.003/+.001 DIA shows the real diameter of the scale model. It shows that I applied the ANSI fits and/or the ISO tolerances entirely with the dimensioning tool's tolerance feature. At the preliminary phase of the design, I even use the ISO tolerance codes because they are independant of the dimension. I have not the nerve to send these out to the fabricator.

I tend to change diameters to limit dimensions when I finalize the drawings. The toleranced dimensions are used mostly by the fabricators and inspectors. Engineers can get at my CAD model.

JHG

 

[Cockroach]

Typicall DrawOh, CAD models are drawing to maximum material. In other words, given 1.253/1.251 as an outer diameter, I would draw a line at 1.253 diameter. Conversely, given 1.251/1.253 as an inner diameter, the line would be drawn at 1.251 diameter.

There is nothing wrong with reporting 1.253/1.251, just as 1.252 dia +/-0.001, 1.251 dia +0.002/-0.000 or 1.253 dia +0.000/-0.002. Depending on the circumstances of the design, the designer would make a consideration on what is theoretically needed to what is practically possible. This in itself takes years of experience, although I have seen enough raw talent to have faith in the practice of engineering, as a skill and an art.

CAD drawings should show maximum material. That way if buddy is having a bad day on the machine and overshoots the lower number, he has an upper target to meet knowing the piece is not dysfunctional. Should he violate the limit, then I expect a visitor.

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