Limit style tolerancing vs bilateral 3

[pugap]

We are in the process of writing drafting standards, and one of the debates is in the method of tolerancing. The majority of our old drawings had ± tolerancing, with some limit style tolerances. The group working on the standards is heading towards standardizing on limit style dimensioning only. The reasoning is that when you are inspecting a part, you only care if you are outside the limits, so the nominal does not matter. The debate comes on the question of design intent and the cad geometry. A part with a .4998+.0001-.0005 tolerance has a different design intent than a .4999/.4993 toleranced part.
Looking for feedback.

 

[looslib]

They can bothn be modeled to the nominal .4998 on UG and Pro/E, don't know about others. You just need to set your tolerances properly.


"Wildfires are dangerous, hard to control, and economically catastrophic."
"Fixed in the next release" should replace "Product First" as the PTC slogan.

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[pugap]

Agree, but the question is if someone sees a drawing with the part toleranced as .4999/.4993, how are they supposed to know to model it as .4998 (design intent) instead of .4996 (middle value)?

 

[TheTick]

I've had this argument before. I like bilateral tolerancing for the same reason: it shows the intent better.

However...
Most machinists/operators/inspectors do not care about your intent. They also don't care much for mental math and would prefer the easy way out.

The fact remains that if your part doesn't function over the entire range of the tolerances, then something is wrong.

 

[MadMango]

Star for TheTick, I agree.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[drawoh]

pugap,

Is it necessary to rigidly mandate this?

You should format the information for whoever is going to use it the most. That standard changes depending on production levels, inspection requirements, and the need for engineering to monitor the process.

JHG

 

[pugap]

That's the crux of the debate. The majority of the engineers are against the limit style, but the drive from the group developing the standards is to dimension prints to help manufacturing/inspection.

 

[ewh]

Is the drafting/design dept under the control of manufacturing or engineering? Everywhere I've worked, it was an engineering department. While consideration should be given to manufacturing methods, I feel that it is more important that the design be documented as engineered.

 

[ewh]

This seems to be boiling down to the same line of reasoning as thread1103-126443.

 

[ctopher]

I agree with Tick.
You can design for intent, but machinist will go for the nominal or mean. Years ago, our company standarized on limit dimensions. We create our models at nominal. All of our machinists and vendors understand it and makes it easier to import into CAM. I like bilateral in some cases, but we don't uses it unless a customer requires it ... it is rare.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)

FAQ559-1100
FAQ559-716

 

[MikeHalloran]

If the intent of the _document_ is to preserve or communicate the design intent, then nominal +/- deviation style dimensioning is appropriate.

If the intent of the _document_ is to show what dimensions are to be measured, and what limits the measurements must lie within, then limit style dimensioning is appropriate.

Yes, one of our customers maintains a separate set of inspection documents, with simplified geometry, and limits shown only for the dimensions to be measured, and with tabular space reserved for each item in a set of samples. A copy of that drawing becomes the inspection record for that lot.



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

 

[Tunalover]

Drawings are for delineating the REQUIREMENTS and should not be drawn to target any particular part of the organization (e.g. manufacturing, test, inspection). The number one role of the drawing is to emphasize function and to insure that the requirements are met. While it certainly doesn't hurt to think about downstream processes when doing drawings, understand that arithmetic and trig are part of the machinist's job; don't go out of your way to draft a drawing that minimizes how much work the machinist (or anyone else) has to do. If you let manufacturing have their way with drawings, they will turn them into step-by-step work instructions that will render them useful only to the organization who drew them (if you sent them to a contract assembler, for example, their hands would be tied into one specific way of doing things and they will quote accordingly!). Lastly, while keeping the drawings reasonably understandable, don't "dumb down" the drawing to suit the educational level of downstream users.

The same goes with unilateral vs. bilateral size tolerances. If a unilateral tolerance most clearly delineates the product function, then USE IT!




Tunalover

 

[Heckler]

A

for your answer tunalover. Typical when our designs require multiple setups or special processes our manufacturing engineers will do "operational drawings" which list only the features for that specific operation or specific piece of equipment. And this gets down to the nuts and bolts of a manufacturing engineer affectively and efficently using the equipment. When the QA/QC department does a complete first article they are required (AS9000) to produce documentation detailing ever feature on that part....this is where they like to use limit dimensions verses +/-....I don't blame then because some of our complex castings can have 300 machined features.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 3.1 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[ajack1]

Surely a lot depends on how parts are to be measured. If all parts are inspected it probably makes little difference, if however only a certain number say one in a hundred are and the company uses SPC or CAP then by not making your desired size the mean, what you are actually trying to achieve as the optimum could fall outside of the control limits.

I do find some of the comments odd about let the machinist sort out the trig, surely everyone should aim to make the next guys job as easy as possible, for example items are dimensioned you do not have to add up half a dozen dimensions and then subtract two to find a size.

We do seem to be becoming an “It is easier if someone else does it” culture.

 

[pugap]

ajack1: Interesting point on the SPC. I don't think anyone has looked at it from this standpoint. Looking at the bell curve (in my example) of a .4998 +.0001/-.0005 design nominal part has a different meaning than the data using a .4996±.0003 nominal value part. Right?

 

[ajack1]

Certainly as I understand it pugap, however I am sure others are far more knowledgeable on the subject than me.

My understanding is as a rule of thumb you aim for 7/10ths of the limit, where if you are piercing or drilling for example you go towards top limit as tool “dulling” brings the part towards mean. If you are turning for example you go towards bottom limit as in this case “dulling” makes the shaft larger and towards mean.

You then have a control limit so all parts are around mean. I do realise there is more to it than that but like I say rule of thumb.

 

[TechDavid]

As ajack1 noted, tooling wear can be a good reason to use bilateral tolerance so that you can specify a target to increase effective life of the components.

If, for example, you have a core pin on an injection molding tool that you know will wear quickly, you'll want to target the size near maximum so that as it wears, you'll get more useable molding cycles from the core. If you set your target as the mean of the spec limits, you'll make it easier to build the core, but you lose life cycles.

 

[EngJW]

My first on-the-job teacher taught me to use the nominal or design-intent dimension, and then put a plus tolerance if a bore and a ninus tolerance if a shaft. The machinist would shoot for the intended dimension knowing that he had some room if he missed it.

I still like this system but everywhere else I worked at they used limits, probably for the reasons stated by Mr. Tick.

Often times there is confusion of what the nominal dimension is. For example, if a length is 5.000 minus .002, some drafters and checkers use 4.999 as the nominal and you can go into a cad layout and find the part drawn as 4.999 instead of 5.000.

Another thing they do, and I think it is an ANSI standard, is to put the largest number on top if it is a limit dimension. If it is a bore, the top number is not the one you want to shoot for. I suppose it makes sense to most people, though.

 

[pugap]

EngJW - Your perspective was felt by the majority here, so we're going back to predominantly ± tolerancing. It became too much hassle when it came to the cad drawings and having something drawn to scale - just like your example. We may still have some limit dimensions, but we'll use them where it makes sense as opposed to being the default tolerance method for all dimensions.

 

[drawoh]

pugap,

.4998+.0001/-.0005 = .4996±.0003 = .4999/.4993 = .5000-.0001/-.0007, exactly.

The fabricated part must not exceed .4999" diameter and must not fall below .4993" diameter. The shop's job is to accomplish this somehow. Nothing in the above formats indicate anything about how the shop is to achieve the tolerance. If the fabrication process drifts, the fabricator will set it towards the end of the dimension range that provides maximum production between setups. If the fabricator likes to show off and can achieve the tolerance easily, they will fabricate as close to MMC as they can.

Statistics have nothing whatsover to do with this. As per ASME Y14.5M-1994, you can indicate statistical tolerancing and allow the dimension to open up a little, accordingly. If you do not do this, the part must fall between .4999 and .4993. All of the dimension formats above are unambiguous.

JHG