Tolerancing Dimensions for Custom Machinery Drawings 3

[curiousmechanical]

Hello Everyone,

I have a question about tolerancing methods used on drawings. I work at a custom machinery job shop where we fabricate parts/machines from outside customer's drawings and our own in-house drawings (created by yours truly). Because I deal with a lot of other people's drawings I see many ways to tolerance parts. The most common that I see are the following 3 methods:

1. People who tolerance their parts using the standard +.000/-.005, +.001/-.001, +.0000/-.0005,...etc. This method seems like they just go with their gut feeling and use multiples of .0005", .001", and .005".

2. Other people just put the nominal dimension on the print and specify the type of fit that they want with a mating part. ex. "0.250" Dia. THRU for Light Press Fit with Shaft A." The guys in the shop seem to like this method the best because it gives them the freedom to size things however they want (within reason) as long as the parts fit together properly.

3. Then I see other people who use very specific toleranced dimensions. They use the American Standard Fits Listed in the Machinery Handbook. ex. h7, s7, etc. I really like this style of dimensioning for two reasons.

a.) I like that I can give two parts to two different people and know that they will fit the way I want them to and the two people don't need to work together to obtain the desired fit between the parts. That just doesn't seem right to me. Although, it seems to be so common in the job shop atmosphere...

b.) Also, I really like using some kind of standard method of generating tolerances rather than going with my random gut feeling as in method #1. I like to be consistent. Although, because the tolerances are always oddball numbers, the guys in the shop always complain and ask me "where the heck did you come up with that tolerance?" I tried to explain that I was using "standard fits," but they seem to give me the common attitude such as: "You guys think all the answers are in those books" or "Books are not always right” or “You are over-tolerancing the parts.”

What is the proper way for me to be dimensioning my parts, in my specific atmosphere? I really don't want to use method two because it seems lazy. On the other hand, I don't want to use method three if it is not necessary or if everyone will think I am trying to just be fancy for the sake of being fancy.

Any suggestions?

Thanks everyone!

 

[Pressed]

When you launch prints of mating parts to the shop it will generally work out better if you detail them for their application. I have always uses the class of fits found in the back of my old drafting book and parts have always mated well.

I can't speak for every machinist but I haven't found one that knows how to apply the standardized class of fits. They can look up the chart values, but other than that it seems foreign to them. Machinist work with their hands and experiences, so the tolerances and fits will be from the school of hard knocks or in error. So if they designed tight mating parts, they would make one part first. Then match it to the next part. Problem is if the parts rotate or slide at high speed, they can seize or other.

Most drafters won't know unless they have been taught. Which is why you see all the standard numbers like +.001 or +.005 and the like. There are allot of people putting stuff on prints that never go downstream to see if what they designated is really working. Some engineers don't know because it wasn't taught or they didn't pay attention in class.

I remember the day they presented this. It wasn't to be on any test and classmates forgot it as fast as it was introduced. My initial reaction wasn't great either, it is odd at first.

To your question: If you choose the correct class of fit for the application then it can't be too fancy. It is a physical relationship of size and application. If you select the wrong class then the parts might: not fit, seize, be sloppy, not operate correctly, add cost. So it is design insurance, so to speak.

One other thing, the use of print call-outs ex. "h7" or "H6" can be interpreted wrong by someone downstream and you only find out when you receive the part. But it sure is easy for the designer to use those designations. If everybody is on-board with that system it is easy, especially when making changes to a large set of prints.

http://www.eng-tips.com/viewthread.cfm?qid=138270

If this post singles anybody, it wasn't intended to.

==========================================
Business Site

http://mech.e.tripod.com

------------------------------------------
Cycle Utopia.......

http://www.tailofthedragon.com

 

[ajack1]

We use the hole and shaft standards all the time. As stated the really strength is that if you call for a light drive fit for example that is what you get where ever the parts are made. If you leave it to the machinist some will make the hole tight some will make the shaft larger that is fine if everything is made in house and changeability is not a problem.

It also works for standard brought in parts, bushes, bearings etc, if the shop floor do not like seeing Dia30 H7 why not give them the actual values say 30.001-30.050? Not that they are the values for a 30H7.

 

[metalwillow]

The hard part........actually getting a machinist to follow
a drawing, especially if they are a veteran. But this is not always the case and some times you have to state your case.

As stated above it really depends on your application.
ie. if you in a high heat applicaton and your using
two different materials, one will expand at a different rate.

In my opinion you should use a method that
1 makes sense to you
2 makes sense for the application
3 the machinist can understand

 

[TheTick]

Tolerance scheme #3 shows that the designer put some thought into the drawing, and is more likely to be asking for exactly what he wants.

When I was a machinist, I didn't give people what they wanted. I gave them what they asked for on the print. If they asked for what they wanted, then everyone was happy.

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[deanc]

TheTick

I agree with each part of your post. I use the last one often.

 

[eromlignod]

You have to take into account how badly you really need that tolerance, how much you want to pay for it, how thoroughly you want to confuse the machinist (and anyone else who has to figure out your intent when reading your drawing) and what the capabilities are of the machine shop. You need to familiarize yourself not only with what fit is appropriate for a given application, but how this degree of accuracy is going to be accomplished in the shop.

If all you want is a slip fit for a dowel pin on a mating part, then you should be careful that you're not calling out a ridiculous tolerance or finish that requires meticulous boring, honing and lapping, etc. You are the engineer and you must know ahead of time just how he's going to produce that part...that's your job. Specifying a fit based solely on tables and statistical charts alone is naïve and can cost you a lot of unnecessary time and money on a project.

If you put "0.500 +.005/-.000", he's probably going to use a .501" reamer and be done. If you use a tolerance of +.002/-.000 then he's probably going to use that same reamer. Tightening the tolerance didn't technically do much for you in this case.

Don
Kansas City

 

[ewh]

I agree with the others. Ask for what you need. I oten use your method 2 for inseparable assemblies, usually tooling. As long as , for example, a pin is the correct size, located as specified, and has an interference fit, I will let the fabricator determine the hole tolerances. For something like a slip fit, however, I will specify the tolerances allowable, as this will effect other calculations. After all, inspecting hole size tolerances on a press fit is pretty difficult after the fact.

 

[handleman]

I work in a custom machinery setting as well. One important thing to remember is that any part may need to be replaced, modified, remade, etc in the future. Any "fit" that has to be matched up with some other part in the shop is a bad idea in that context.

 

[wes616]

Remember when you do prototype work you don't actually have to worry about the fits regarding replacable compontents the same way you would if you were in a volume manufacturing environment. Many of these standard fits and tolerances are derivitive of such manufacturing environments where statistics rule the roost. In prototype work it is better to use common sense to make the fit than statistics.

There is a big difference between steve down in the shop drilling the hole for a light press fit than there is when it's 6 guys working 3 shifts drilling the same hole in five parts a minute.

Wes C.
------------------------------
No trees were killed in the sending of this message, but a large number of electrons were terribly inconvenienced.

 

[Tmoose]

A maker of fancy automatic drawbars for machine tools includes a hunk of the ISO hole/shaft table in the corner of the drawing that is dimensioned using 27 mm H6 etc.

I thought, and think, that is one good solution.

http://www.ame.com/images/hskmanual.pdf

 

[drawoh]

curiousmechanical,

The standard tolerances from the ANSI handbook are weird because they are called out in inches, and they are based on the ISO standard, which is metric. I am sure they are also based on a lot of practical hacking around in machine shops. Limits and fits are a wheel you do not have to re-invent.

Your Machinery's Handbook has charts showing you the ANSI fits, the ISO fits and tolerances, and tables showing what fabrication process is required to achieve any given tolerance class. There is an additional table showing what surface finish can be achieved by various processes. I recommend that you bookmark the pages.

I like your method 3. Using the standard ANSI fits means that you can design new stuff, drastically resized from the old stuff, apply the same fit class and get the same performance. If your tolerance values look non-standard, it indicates that you thought about them. This tells the fabricator that he had better achieve them.

JHG

 

[KENAT]

1. Done correctly it isn't gut feeling. Tolerance should be driven by function while supporting manufacturability as much as possible. These values are arrived through a combination of experience, calculation, investigation... Sadly in practice you're correct that alot of people just throw down numbers or, sometimes worse, leave the default CAD setting for number of decimal places on dimensions and hence invoke the relevant title block tolerance, without even thinking.

Like ajack in the case of push fits etc I will typically use the standards you give in option 3 to find the values but convert them to +- type tolerances on the drawing as in the US this seems what machine shops are used to, in the UK I did a similar thing but showed the tolerances as upper and lower limit as this was the customary way of showing tolerances.

2. I do not like this way. You don't have control over the end product, essentially you're leaving it to someone else to do your job as the designer and your drawing does not fully, unambiguously define the part. For instance If you have dissimilar metals with different thermal coefficients then what was an interference fit in the shop could be a transition or slip fit in it's application (this was based on a real example). As for using this method on prototypes, beside the problem I already stated prototype drawings have a habit of turning into production drawings with little more than a change of rev at most. Sure the prototype hand built by skilled fitters worked great, the 1000 made by semi/unskilled staff have pins falling out or parts deforming due to the force required to push the pin in etc. Only time I might do this would be on some kind of one off production tooling like the example ewh gives.

3. Is a reasonable way. In mainland Europe and maybe Japan this seems standard. Trouble is in the UK & US many machinists etc wont fully understand it. Also when done on shaft basis (I think that's the right way round) with common shaft sizes standard tools should be available to support this, although this may be more applicable to the metric world.

So suggestion 4:

4. Use the values given by the standards but express them in +- or limits form. This way the machinist understands what is required of him and you have the benefit of using values that have been established by people with more experience than certainly I have.

Does your company invoke any drawing standards, eg ASME Y14.100/14.5 etc If so by my interpretation this would probably preclude option 2 (ASME Y14.5-1994 1.4a-d).


KENAT, probably the least qualified checker you'll ever meet...

 

[curiousmechanical]

First of all, thank you everyone for the wonderful feedback!

It's such an eye opener to hear other people's points of view. I'm glad to see that most people support using standard fits and tolerancing parts properly. I think the best defense I read was the idea of interchangeability, especially when a replacement part is needed. That will help me defend myself out in the shop! On the other hand, I am glad someone mentioned that it is naive to try to use a table for everything. Not everything is so cut and dry. I sometimes need to be reminded of that. At my company, we also do a lot of work that is simply an in-house one-off project that will never occur again in the future. In those cases, I could be more relaxed on my tolerancing I suppose.

At my company, they would probably be more than happy to only release hand sketches on napkins if they could. Luckily for me, they can't do that with more complicated projects. I am fairly new to engineering. Therefore, I am still trying to hone my designing skills to be the best engineer I can possibly be. Concerning my drafting efforts, I just want to do the things the correct/best way.

Is there a more detailed reference for tolerancing standards other than the machinery handbook? I'm sure there are specialized ones for GDT, but is there a reference with a usefulness equivalent to the machinery's handbook?

Thanks again everyone!

 

[hydtools]

Tolerances should be determined by the person who will be the bad guy if the design does not work. My opinion is the designer is responsible for the tolerancing. The designer is also responsible to understand manufacturing prosesses and how capable they are of holding tolerances. Talk to the machinists to learn what it takes to hold tolerances.

You may note tolerance class on a drawing but I recommend also stating the tolerances. Don't depend on someone looking up a reference. You already looked it up, write it on the drawing.

Title block tolerances were agreed to by both product design and manufacturing. These were default tolerances if none were specified. Otherwise, dimensions were toleranced. Including stating tolerances greater than title block tolerances (that will get you some shop questions).

Ted

 

[KENAT]

If you're in the US then ASME Y14.5M-1994 Specifies Dimensioning & Tolerancing, it is THE industry tolerancing standard for mechanical drawings.

Whether you/your company choose to invoke it is another matter.

It does not only cover GD&T, it also defines a lot of the basic rules, Section 2 is titled "General Tolerancing and Related Principles".

However it doesn't have the table of fits in it but references ANSI B4.2.

Other countries have different, broadly equivalent, standards BS8888 in the UK which in turn references an ISO as I recall. Note that there are some differences between them.

There is a forum on this site that specifically deals with tolerancing and GDT:

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

KENAT, probably the least qualified checker you'll ever meet...

 

[curiousmechanical]

Do you think ASME Y14.5M-1994 is a necessary resource for an engineer to have? Or, does it just provide some general information and guidelines (basically...how thorough is it?)? Also, I checked in to B4.2. That seems to be the guide to Preferred Metric Limits and Fits. Do you know of a guide for ANSI fits (I am in the U.S.)? Or, is that included in the ASME Y14.5M-1994?

Thank you!

 

[ajack1]

This is a useful reference; unfortunately to the best of my knowledge full standards cost money.

http://www.roymech.co.uk/Useful_Tables/ISO_Tolerances/ISO_LIMITS.htm

 

[KENAT]

If you are serious about creating high quality drawings that conform to accepted industry practices then yes, 14.5 is almost a must. At least half of it does deal with GD&T which you don't seem to concerned about but it also sets down a lot of other conventions etc.

It doesn't have a table of limits and fits and the only one it references (unless I'm missing something) is B4.2.

I don't know of an inch version of this. Obviously you can divide by 25.4 and perhaps add a decimal place if need be but, if you're coming off an inch size shaft in the first place this probably wont then match the 'standard' tools.

KENAT, probably the least qualified checker you'll ever meet...

 

[hydtools]

Just to be clear, ASME Y14.5 does not tell you what tolerances to use. It is a guide to create uniformity in the stating and interpretation of tolerances. You should also consider other ASME Y14 standards for engineering drawings.

Inch version of fits standard is ANSI B4.1-1967(R87) according to my Mark's 10th edition.

Ted