In house tolerance standards

[MR Wolfdog]

I am the Machine Shop Supervisor in the "Engineering Department" at a major paint company. This is a very hands-on position as it is only me and two welders. When I first started there were only the default tolerances on the print that the CAD software put there. There are two Designers. One had no idea what a tolerance is and the other was taught in school that there is no place for fractions on a mechanical print. The department manager did not know what a tolerance is. I was getting prints for the mill and lathe that were dimentioned in fractions and band-saw and weld projects with 3 and 4 digit call-outs. (As a note I would like to say that this shop is strictly a support facility that caters to production, facilities, R&D and distribution.) Many projects are reverse-engineered, and some are semi-architectural, and others are in-house designed, tooling and fixturing. I requested a tolerance block call out as follows:
X/X = +/- 1/8 (to support welding projects)
.XX = +/- .02 (to allow the use of stock edges of material when application allows)
.XXX = +/- .005 (good all around machining tolerance)
.XXXX = +/- .0005 (bearings, dowls and other press fits)

I understand these are very general, but they cover most of the work done, and it is a good starting point. The idea was pretty well recieved except that the designer that went to school would not have any part of fractions on a print. We got a new manager and I gave him a quick lesson on benifit or use of a tolerance and won my case. Since then the designers have attended a GD&T course and the battle resurfaced. One of the issues screwing with my head is during the design process, I have been taught to use standard numbers in the design, these represent common fractions and wire sizes. Basicly, anything you will find on a fraction/decimal conversion chart. .75, .375, .188 etc. If I were to accept .X = +/- (.1/.2/.3 etc.) as a tolerance and a location, the only standard number that I would have to work with would be .5. Anything else would have to be rounded/assumed. A .25 target would be .3? I have several friends that work in heavy GD&T companys and they still retain the use of fractions for in-house fixturing. I have looked all over the internet for examples of what I would like, and I see many prints with a tolerance block simalar to what I want. I cannot find a GD&T example with a tolerance of .X or larger. Can I get some advice? If have to accept all decimal an all decimal format, metric would be a much better option. Thanks in advance ~ Mr Wolfdog

[Kelly_Bramble]

Welcome to Engineers Edge!

Well, you having thought about this in detail.... I'm tempted to just tell you to call me; however you did post this on the forum.

First, a little about me to qualify my answers...

I’m an old guy, 34 years engineering and design, mostly in aircraft, spacecraft and scientific hardware.
Last eleven years I have been a DFM and GD&T consultant and trainer – Google me
Authored four books on dimensioning and tolerancing (GD&T) and one book Design for Manufacturability.
You can feel free to buy one or all here --> http://www.engineersedge.com/catalog/index.php/cPath/21 --sorry about that folks....
Oh ya, I’m certified by ASME at a Senior GDTP – since 1997 and have an FAA Airframe and Powerplant Lic.. Educated too..

First, I agree that read-able tape measure increments (fractions) for tolerances and distances (Feature of Size) are a great choice for weldments. This is good practice from a DFM and dimensioning tolerancing point of view - works great.

The latest and greatest ASME Y14.5-2009 GD&T standard specifically says that that “US Customary linear units are the decimal inch”. But, it is understood that this is a general standard meant to cover the needs of many **********, so corporate standards are often utilized.

Often corporate dimensioning standards are **********s based on an existing standard (e.g., ASME, ISO) with additions or exceptions described. Typically, corporate **********s include four types of information:

• Choose an option when the standard offers several ways to specify a tolerance.
• Discourage the use of certain tolerancing specifications that may be too costly for the types of products produced in a corporation.
• Include a special dimensioning specification that is unique to the corporation.
• Clarify a concept, which is new or needs further explanation from the standard.

In other words – manufacturing and design need to get together and agree to what is in the best interest for your organization. Everyone should have a say – need keep competitive in this world.

Designing to common or preferred decimal or fractional increments is a good DFM practice for about any thing engineered. This will allow manufacturing to use standard or stock sizes without additional processes, such as milling a thickness. However, in engineering and design we often get stuck using odd non-preferred sizes, etc. due to design constraints. Design should try really hard to use preferred sizes.

As far as rounding up or down to whole numbers this should be specified in your company standards and or on the engineering drawing and understood by both design and manufacturing. Rounding up from .25 to .30 could in some cases cause a fit and stacking problem at end-item assembly or weldment. No simple answer, just that everybody needs to be on the same page.

For a standard tolerance block, you can do anything that fits your applications there are no hard and absolute rules.

For example, you can have a tolerance for a linear distance and a tolerance that applies between two fractional sizes…

You might post what you think you want and we can go from there…

Ok, it’s late here and I got a grandparents breakfast tomorrow morning…

[jboggs]

First, thank you for your post. And please excuse the length of my response - but you've hit a nerve. This is a perfect example of the power of a forum like this - multiple points of view on a common question.

Like Kelly, I too come from a long manufacturing background. I've worked in many ********** including tires, paper, automotive glass, electronics, machine tools, truck components, powertrain, paint, steel mills, and have consulted in 100's of various applications.

We all end up with our own philosophies about questions like tolerancing. Here's my take on it: It's all driven by the end product. Unless you are bound by some broader corporate or industry standard (which you are not), this question should be approached from the point of view of what policies are most likely to produce the most useful finished product considering the skills and capabilities of the personnel involved.

Designers and engineers should treat the drawings they create as their "product", but it more accurately is just their contribution to the finished product. The drawing should fulfill its purpose of accurate communication completely and efficiently with minimum waste. Its "purpose" is NOT to impress everybody with how smart you are. That just causes confusion, resentment, and mistrust. Its purpose is to communicate ALL required information that will allow the downstream users (with their understanding and skill level) to accurately produce, inspect, and inventory the described part with no questions or confusion. The finished product is the goal here. The drawing is only one of many tools required to produce it. It a tool isn't working right, you change it.

On the specific question of dimensioning and tolerancing, in the absence of a corporate policy I follow my own philosophies. This all applies to imperial units (inches) only. I share your designer's hesitance to use fractions on a machine part drawing. My engineer's gut says that fractions belong on civil and architectural drawings, not on machined part drawings. That's one way you can tell when a civil engineer makes a machine part drawing. But I have learned and re-learned a very hard lesson over the years; there is an absolutely proper use of fractions on machined part drawings.

Most of the folks using your drawings are not going to be trained machinists. They are not going to know that 0.4375 is 7/16". And they certainly aren't going to know it if it is expressed in two decimal places as 0.44. But they do know how their tape measure is marked and how their drills are labeled - fractions. So, for minimum confusion when I am dimensioning screw clearance holes or weldment stock cut lengths I will use fractions. Obviously any machined surfaces require decimals.

My general default for linear dimensions is two decimal places, angular is no decimal places. The tolerance protocol that has worked best for me is:
Fractions = ± 1/32 (that's 1/16" total)
x.xx = ± .010
x.xxx = ± .005
Angle = ± 1/2°

For tighter tolerances (such as dowel position and size) I will use four places with explicit tolerances.

I think in inches and fractions, and express it in decimals. So, obviously .25 is 1/4". For fractions that require more than two decimal places, users must understand that .37 or .38 either one means .375 ± .010.

Generally, outside edges are dimensioned to two decimal places. For bolt patterns or other features that require more precision I use three places.

The varying capabilities of different machining processes (band saws and welding vs. milling and turning) explain why two separate drawings are often used for machined weldments. One for the technician doing the rough cuts, welding, and stress relieving, and one for the machinist creating the precise features.

One last thought: a designer that consistently fails to use various tolerance levels properly is either inexperienced and needs to learn or is just lazy (and needs to learn a more painful lesson).

To quote Forrest Gump: "That's all I have to say about that."

[RWOLFEJR]

Yep... what they said...

Make it easy for the folks using the drawing to understand what you're after.

Another little side note... Try to place dimensions at the same place on the drawings if you're making a lot of similar parts. Operators will get into a habit of looking at just the details involved in their particular machining operation. Make it easy and try to stay consistent with how you present the details on your print.

Also... We have a note on our tooling and part drawing tolerance block that says... "Tolerances Except Where Noted." Myself... I always tolerance every dimension right where I plop it on the print. If things get cozy I'll blow out a detail or section to dimension.

[MR Wolfdog]

Thank all of you for your very quick responses. I am on the same page. I have no need for fractions on prints for projects that will be run on my mills or lathe. My welders do primaraly 100 gallon stainless tanks, hand rails, sprinkler guards, and things like this. Their job is to band-saw or plasma cut to size, weld, then grind sexy. All of their measuring instruments are fractional. They are very good at delivering very functional projects. The person that wants this loose tolerance work dimensioned in decimals is from a metric part of the world and I understand his desire for a 10 base measuring system. But not with an inch. He is quoting ASME Y14.5M as justification for "all decimal" dimensioning, but no other aspects of GD&T. Goemetric Dimensioning is different than Distance Dimensioning and I do believe basic Distance Dimensioning is all that our shop requires. The department management does not want the conflict this is generating and does not want to side with either party. I need all of the professional input I can get. A possibility might be to hire a consultant to analize the scope of our projects and make a recomendation to the management.
Again thank each of you for your input.

[jboggs]

A couple things.
First, my symbology got screwed up in internet land, here's what I meant to say:
Fractions = +/- 1/32 (that's 1/16" total)
x.xx = +/- .010
x.xxx = +/- .005
Angle = +/- 1/2 degree

Second, sounds like you have a boss who doesn't have an opinion and doesn't understand the problem. Don't let personalities drive this thing. Maybe this will help. Many engineers mistakenly picture themselves as the "drivers" of the enterprise. After all, they are the ones that went to school. They are the "intelligent" ones, right? So, their word should be final. In my experience those guys will eventually find themselves on the outside and will blame everyone else. The most succesful engineers I know see what they do as a service. Engineering is a service organization. If there were no need for their help, they would not have a job. Yes, intelligence, mechanical insight, and technical inderstanding are critical to an engineer's performance. But they hold NO VALUE WHATSOEVER if he cannot communicate clearly and simply. The results are the same if he refuses to. Yes, ASME has recognized standards. So what? So does ISO, and ANSI, DIN, EU, and all the other alphabet soups out there. But what value is there in imposing those standards on your shop floor folks when all that is really needed is for the engineer to put himself in their shoes?

If those standards can't help your company get widgets out the door in the most efficient manner, they are useless. In my experience, unless you are in aviation, defense, NASA, or similar ********** your floor level technicians, the poor slobs who have to convert your drawings into a useful product, have not been trained in that stuff. And there is no need to if the engineer, who is supposedly sooooo intelligent will just think and communicate in terms they clearly understand.

You might want to try to communicate these thoughts to him or your management in slightly more tactical terms. Honestly, this whole question probably wouldn't have even come up if the designer and/or engineer were out on the shop floor working hand in hand with your guys to "git-r-dun". Now - there's a thought!

[jboggs]

I just got a clue - you said the person pushing the decimal dimensioning only was "from a metric part of the world". If that means this person grew up in a non-fractional environment, like Japan or Germany for example, that makes his position much more understandable. Remember I said I think in fractions? Well that's mainly because I grew up in the US. I learned about this when I worked for a company that was redrawing European drawings for American use. We had to use metric dimensioning exclusively. We adopted the terms "hard metric" and "soft metric". In "hard metric" the designer is thinking in millimeters from the beginning. In "soft metric" he thinks in fractional inches and just expresses it in millimeters. Hard metric drawings had a lot of even metric dimensions. Soft metric drawings were full of metric dimensions like 12.7, 19.1, 38.1, 50.8 (1/2", 3/4", 1.5", 2.0"). If your designer's brain isn't wired to automatically think in fractions, that could be a difficult transition for him/her. That might help explain their hesitance. Again, I think the more time this individual could spend on the shop floor working with your technicians the better.

[MR Wolfdog]

I could understand if it were just hesitance. But, this person is very animated and mad if/when he doesnt the get standards in a 100% decimal format. When the new manager sided with me (after meetings of course). this guy would not speak to me for at least a month. And now he goes to a GD&T course, comes back and "proposes" basing our drawings "primarily on ASME Y.14.5M standards". No mention of geometric symbology though... go figure. This is a little 3 person fab shop with me, the machinist and two pretty good welders. Heck, we don't need tolerances. I know enough about my projects to know a press fit from an outer edge and where a datum should go. The welders do their best and that is GREAT! I just don't want to get parts for the mill and lathe in fractions and band saw / weld projects dimensioned with 3 and 4 digits. I understand what a metric background could put in the head, but we are not metric. I also contacted the instructer at the GD&T class they the drafters took and he also confirmed that fractions are OK for loose tolerance items. This designer quoted the instructor as advising that "Fractional dimensions are usually used where tolerances are looser. However, the same can be achieved using decimals, and not be in violation established standards." The only problem I have with that is if a " loose tolerance " is called out .X - and it is dimensioned likewise, my only choices are .1, .2, .3, etc. These are not standard numbers used in design work. Only .5 and .0, what will the designer use if the customer of a project wants something 17-3/4? Does he call-out 17.8? Just wrong in my opinion.
Thanks to everyone for your input.

[MR Wolfdog]

that should say 100 percent decimal format. I don't know what happened.

[jboggs]

I feel your pain friend. One thing I have learned over the decades is that if people who continue to piss everyone off are not ushered to the door, just be patient. They will eventually find their own way there.

You should ask the decision maker on this question what business you are in. If you are in the paint business, drawings are just one of many means to that end. If you are in the drawing business, paint is an accidental by-product. ALL of the most strictly controlled engineering methods are just tools, just like a hammer. The job to be performed determines the tool to be used. If you want to cut off stock to some rough length you could use a multi-million dollar precision water jet, but you don't. You don't because there is no good business reason to do so. The same logic applies to fractions on drawings. If using fractions enhances accurate communication (which in your case it does) they should be used where appropriate. If using decimals for rough low-precision callouts does not enhance accurate communications (like the example of 17.8 for 17-3/4) they should not be used. I, for one, NEVER EVER use a single place decimal for that very reason.

By similar reasoning what advantage does it gain your business to adopt, implement, and enforce some drafting standards designed for businesses that are orders of magnitude larger than yours? How many people actually use your drawings anyway? Hundreds? Thousands? What purpose do they serve beyond just basic fabrication? Are they government records? Are they patent or legal documents? Is there some contractual requirement involved? No, all they do is communicate to your few guys in the shop how to convert the designer's thoughts into a functional part. As I understand it, that is their sole function in your business of making paint.

[PIYUSH PATEL]

I received drawing from my customer, In that drawing All liner Dimensions are in Inch and (mm).

My Query is that, Tolerance table incorporated in drawing have two type of tolerances.

1. Decimals(±0.05) & 2.Fraction(±1/64).

Which tolerance to be used?

Thanks in advance.

[jboggs]

The tolerance block probably applies to the inch dimensions, not the mm dims. Inch dimensions can be expressed in decimals or fractions. Are the inch dimensions in decimals or fractions?

[Kelly_Bramble]

I received drawing from my customer, In that drawing All liner Dimensions are in Inch and (mm).

My Query is that, Tolerance table incorporated in drawing have two type of tolerances.

1. Decimals(±0.05) & 2.Fraction(±1/64).

Which tolerance to be used?

Thanks in advance.

Can you post a picture of the tolerance table and any associated note defining how to interpret dimensions and tolerances on the drawing?