Tolerancing style

[metalonis]

I thought this might have been discussed before in this forum but I couldn’t find the thread.

Under which circumstances are limits vs ± vs +x/-y tolerances used or more desirable?

 

[4zengineering]

I use a z +x/-y when I feel like z measuring z would best suit the function of the part, or when hard tooling that establishes z is going to be built.

When I put the tolerance that way, I suppose it identifies it to our toolmaker as needing to be that number without being too restrictive, and he usually builds the tool right at z.

If I went somewhere else, or we had a different tool maker, I'm sure our little "gentleman's agreement" might not work, but that seems to work for us right now.

 

[fcsuper]

I only use +x/-y when I have tolerance zone that is not centered on the nominal. Otherwise, I just use ±.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[metalonis]

But not limits? Some of our designers prefer limits, others prefer +/- or ±.

 

[KENAT]

I assume you mean Limit Dimensioning per section 2.2 of ASME Y14.5M.

In the UK where I worked we normally did limits, e.g. .995 to 1.005. Here in the States the place I work mostly uses +- e.g. 1.000+-.005.

I'm not sure there's any widely accepted method of determining which to use. +- Dimensioning is perhaps better for manufacturing, as it gives them a nominal/mean to aim for without calculation. Limits is perhaps better for inspection since it's obvious if a measurement is more or less than the limits without calculation.

However, the calculation is so trivial I'm not sure it's much of an argument, but I suppose for every calc there's a chance of a mistake.

Now as regards non symmetric +- dimensions, the most obvious example I can think of is typically drill tolerances. Depending on size these will be +.005 -.001 or similar, essentially the nominal size of drill tends to produce an oversize hole. This Tolerancing method is to allow easy selection of standard size tools while allowing for the fact that the hole will be oversized. The same idea may be extrapolated to other processes etc, perhaps some types of semi stock dimensions or the like.

I know some people use non symmetric to imply they'd rather be at one end of the range than the other. For instance if they'd like to have a .5 dimension but if push comes to shove they'd accept up to .51 then they'll dimension it .50 +.01 -.00 rather than .505 +-.005 with the hope that most of the parts will end up nearer .5 than .51. However, to the best of my knowledge this idea of preferring one end of the tolerance zone is not supported by the standard, if the entire tolerance range is acceptable then it's acceptable, if not then a tighter tolerance should be specified.


KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

What is Engineering anyway: faq1088-1484

 

[metalonis]

Yes, I did mean Limit Dimensioning per section 2.2 of ASME Y14.5M.
Guess the debate here will go on.

Thanks all for your insights.

 

[dgallup]

Usually it's determined by some sort of company standard.

In general, I like to keep all dimensions nominal with symmetrical +/- tolerances. I only use asymmetric tolerances when it is absolutely necessary such as the ISO system of press fits. I think asymmetric tolerances are way overused. Most manufacturing process these days are going to try to be mean centered to keep their Cpk high.

The places that I have seen that prefer limit dimensions have production operators making manual measurements. With limit dimensions the operator does not have to make any calculations to see if the part is in limits. As a design engineer I hate them as I have to constantly calculate the nominal. But I make fewer calculation mistakes than the operators so I understand the reasoning.

 

[SDETERS]

I like to use +.005/-.001 type dimensions when I want close fitting parts to be targeted to the Design intent. Like a rod in a bore. Other than that I like to use limits.

Some people argue here it is all the same if you use (1.003/.997) or 1.000+.003/-.003 or .998+.005/-.001. I would like to think if I use +.005/-.001 they are targeting to the .998 dim I have on the print and not the 1.000 average of the tolerance.

 

[KENAT]

SDETERS that's exactly the case I was trying to illustrate and to the best of my knowledge it's not backed up by any standard or the like. I'm sure many operators just calculate the mean and aim for that.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

What is Engineering anyway: faq1088-1484

 

[drawoh]

metalonis,

For me, it all depends on the end user, the functionalty of the drawing, and the information I want to show off.

In CAD, if your dimension is Z±x or Z+x/-y, presumably, you modeled to dimension Z. Often, someone needs to know this. The Z dimension is your nominal design intent.

I know that machinists on a lathe like to see limit dimensions. This is probably more convenient to inspectors too.

JHG

 

[CheckerRon]

We work to a company standard (manufacturing driven) that insists on "target" dimensions, meaning nominal, with an equal ± on unequal +x/-y tolerance. Both unilateral and limit dimensions are prohibited by our DRM.
This drives some people nuts, particularly when working with standard fits and matching to unilateral dimensions from purchased components. We thus convert limit and unilateral dimensions to "target" dimensions with an equal (or unequal if an odd number) tolerance.
The only advantage I see is that it prompts you think about your tolerance, and not just copy something.

 

[PeterStock]

I tend to use limit dimensions (i.e. .999-1.005). I prefer not to use 1.000+.005-.001 as the cad model will measure 1.000. Alot of time the vendor takes the model to make the part. If the nominal is close to the limit or worse yet at the limit (i.e. 1.000+.005-0) there is a good chance a bad part can be made. I prefer that a vendor not have to change a model to insure he creates a good part.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

 

[drawoh]

PeterStock,

RC4 fit on a 2-1/8" diameter...

Shaft (f7): Ø2.125 -.0012/-.0024 = Ø2.1238/2.1226

Hole (H8): Ø2.125 + .0018/0 = Ø2.2168/2.2150

Note how the limit dimension does not show that the shaft diameter is outside the limit dimension values. If you explicitly show the as-modeled diameter, there is an opportunity for someone, including you, to sanitize the model for fabrication.

The jobbing machine shops I deal with read drawings carefully. In my one and only experience with a rapid prototyper, I do not think they even looked at my drawings. The next time I do rapid prototyping, I will change my CAD procedures.

JHG

 

[metalonis]

So far I haven't heard any totally compelling arguments either way, but I tend to agree with PeterStock. Dimensioning to the reality of the finished part just makes sense to me.

 

[CheckerRon]

One of the big reasons we use nominal or "target" dimensions is to get our designers to build nominalized CAD part models (as Peter was mentioning), especially to facilitate CAD assemblies. This is why we avoid unilateral and limit dimensions.
We do very little MBD, so all tolerances are covered on the drawings. I except to see that changing, however.
Inspectors I've worked with prefer limit dimensions, and I can see machinists particularly lathe operators preferring unilateral dimensions.

 

[NomLaser]

In a design world, you would want to show design intent and keep that history. Example is the shaft/hole fit. In this case you would have your shaft size with double negative tolerances. Sadly, you will, more times that not, get back a part out of tolerance because they will use the CAD data or think you made a mistake with double negative tolerances (I have had both happen to me).

So what we as designers have to realize is that there are other people that will be making our parts. They may or may not take the time to double check their inputted values into their calculator or just simply make a mistake. Whatever happens, the designer should be responsible for ensuring that the parts are toleranced for manufacturability. So if that means using limits or (a)symmetrical tolerancing then it should be done.

So what I'm saying is that the parts should be toleranced in a way that makes it easiest to manufacture but it should also hold up to the intended design intent.

 

[HGMorgan]

Drawoh - take a look at your numbers, transposed the 1 2 on the hole tolerance

Group - make it nominal in the model and dwg, and use +/- tol, that is easier for everybody except the up front designer. People get hung up on the 2 1/8 dia being nominal, and in this case, it isn't.

Drawoh's example would be:
Shaft 2.1232 +/- .0006
Hole 2.1259 +/- .0009

Easy to read that the shaft is going to go in the hole. Easy to make to model and/or dwg, easy to inspect.

 

[MotorVib]

I also tend to use limit dimensions. It limits the chance of errors reading drawings. People should be able to read drawings but they still have problems reading drawings.

Chris

"In this house, we obey the laws of thermodynamics." Homer Simpson

 

[drawoh]

HGMorgan,

Oh well. For once, I did not do the calculations in my head. I used a calculator. Bad typing made up for it.

The problem with the Ø2-1/8" is that I normally model to nominal size, then apply tolerances. In SolidWorks, I can set tolerances to the ISO tolerance codes used by the ANSI tolerances. If, half way through the design, I want to change from RC4 to RC5, I go to the fabrication drawings and change the ISO tolerance codes. The model is Ø2.125".

The jobbing shops I go to seem to get this right, so I assume they are reading my drawings. As noted above, if I need rapid prototypes or castings, I intend to wind up with everything modeled at median size, with ±[ ]tolerances.

JHG

 

[CheckerRon]

There ye be, HG (Morgan). I agree with you completely