INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Jobs

Tolerance +/+ -/-

Tolerance +/+ -/-

(OP)
I have been using +/+ or -/- tolerances for a while now with no problems. For ex.: shaft 3" +.005/+.010, hub 3" -.005/-.010. Means shaft can be 3.005 to 3.010 and hub 2.995 to 2.990. This keeps my dimensions simple, clear and clean but tolerances drive the machining limits.

Lately somebody started questioning my sanity on this practice. Is this technique I use to GD&T standards?

William

RE: Tolerance +/+ -/-

It is a valid way to dimension. In the past I used this method a lot but after a couple of parts (from different shops) came in wrong with the explanation of "I thought that was a mistake and you really meant +/-..." I immediately went to using limit dimensions and haven't looked back. In my opinion it just leaves too much ambiguity to be worth it. That being said it doesn't go against either ISO or ANSI.

HTH,
Dan

Han primo incensus

RE: Tolerance +/+ -/-

Just point them to the standard fit tolerance callouts provided by ANSI B4.1 for an example of that exact method of tolerancing from an obvious authority. Keeping simple NOMINAL dimensions is often quite beneficial.

If you just use it as a way to make your nominals 'round numbers' and not actually to convey some information, then I could see it being insane. Otherwise, the ANSI B4.1 example is designed to infer specific information.

RE: Tolerance +/+ -/-

This should be an interesting debate.

My two cents: over the years in high-volume production environments with statistical process control and Six Sigma influences, I tended towards limit dimensions more than NOMINAL plus/minus (or any variation thereof). The reason: I wanted to make it easier for the Quality Engineer to set up controls and the Operator to verify features on my parts. More work for me once, less work for the people who have to do it all day every day. The feedback I received was that they appreciated my effort.

TygerDawg
Blue Technik LLC
Virtuoso Robotics Engineering
www.bluetechnik.com

RE: Tolerance +/+ -/-

Tell somebody to open a copy of Machinery's Handbook and show them the shaft tolerance section.

RE: Tolerance +/+ -/-

Back in the day, that was a perfectly acceptable and understood method. Nowadays, I'm not sure machinists are getting enough drafting, print reading, and GD&T skills taught before turning them loose in the shop. I would favor a 3.005/3.010 type of approach rather than calling out an essentially dead nominal number before the tolerance brackets. Expecting a machinist to look up his/her own standards or tolerance/fit charts would not be good practice, and even introducing it as an example may have unintended consequences. Occam's razor, give them exactly what is need to make the part, nothing more and nothing less.

It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.

RE: Tolerance +/+ -/-

(OP)
I do use nominal to convey design intent: 3" shaft for 3" hub and then fine tune it for machine shop with tolerances. Engineers look at nominal dimensions and machine shop looks at limits. I guess I worked too long for a place where machinists knew my quirky ways but now I have to outsource alot of parts hence there is not even Machinist handbook in-house.

I will change to "standard way" of doing things not to receive junk parts.
Glad I wasn't breaking any GD&T laws. Interesting fact: my GD&T professor was from Poland that's where this "European" way of dimensioning came from.

Thanks for all your input.
William

RE: Tolerance +/+ -/-

What you describe is not quirky, but standard practice.

What ornerynorsk says would seem to apply here.

Luckily, we either train machinists in-house, get them out of trade school, or a combination of both - but they have a good understanding of GD&T and it's typically a specific (hopefully required) class that focuses on that topic alone.

Dimensioning "Limits" might be a safe way to account for... the human factor... I suppose. I have done similar in other circumstances, but I hate deviating for the sake of 'dumbing it down'.

RE: Tolerance +/+ -/-

FeldmanWill,

I know that machinists like limit dimensions. If I am measuring something, I want to know the upper and lower limits. Nothing else matters.

If I am issuing DXFs or some other scale model, I want the fabricators to know what size I modeled the feature at. 40+0.1/+0.05 shows the model size, and my tolerances.

--
JHG

RE: Tolerance +/+ -/-

2
MIL-TFP-41 seems reasonable.

Ted

RE: Tolerance +/+ -/-

Interesting OP post, and interesting replies. I really can't add to the excellent replies.
but I will give my opinion.

over the years I have had the privilege of working in different working environments.
each are different and require different techniques.

what I have found out is it's what the Engineers, and skill workers are used to. and what they are taught.
notice I said skilled workers. the level of education and experience is as different from person to person.
general machining, sheet metal fabrication, metal fabrication in general, assembly, precision assembly, and on.

I have personally over the years have like the +/- from a nominal, it makes my job easier as a fabricator.
and easier to calculate stack ups.and as a general rule the process sketches are applied upper and lower dimensions. so no calculations for
the machinist or the fabricator. not all fabrication is completed right from the drawings.
there are changes that have to be made. for example tooling tolerance have to be held, stack up of dimensions have to be held.
plating allowances have to be held. distortion or grind stock or machining allowances have to be held. allowances for heat treat, and so at the end
all print dimensions are held. and it can get complicated.
just because a dimension has +/- .005 tolerance if any heat treating, grinding , machining in general that tolerance has to be choked.

but for designers the end results is all that matters.




so the final size can be held.

RE: Tolerance +/+ -/-

As a machinist, I was really good at giving people what they asked for, which they also paid for. If they wanted to pay me to march over to the book shelf and peruse the standards, well... it's their money.

RE: Tolerance +/+ -/-

(OP)

Quote (TheTick)

As a machinist, I was really good at giving people what they asked for, which they also paid for. If they wanted to pay me to march over to the book shelf and peruse the standards, well... it's their money.

That's why I always get 3 quotes. bigsmile

RE: Tolerance +/+ -/-

What book on the shelf would be needed to add or subtract a tolerance? I cited a book that has examples to support the OP's opinion on +/+ and -/- tolerancing.

I wonder what machinists do with profile tolerances or position tolerances applied to MMC boundaries. It could be too complicated. /s

It is interesting, the notion of how ranges are displayed supposedly affect the apparent ease of doing the job.

For a CNC programmer, they won't really like having to take limit dimensions and average them to find the center value. And it makes it harder to say that the given limits are +/- 3 sigma for a given process by just looking up previous process distributions, instead also requiring a calculation. Sure, if one has captive manufacturing and are buds with someone in QA it can make the relationship better, but it's not a universal truth.

On the other hand, one is faced with the problem of dealing with people who only half pay attention to what they are doing and need to have the dimensions ordered just so, in an effort that makes it so the machinist turning a hand crank on a cross feed will hit the first limit first and with enough time to wake up and notice that the other limit is now coming up and stop cranking.

I had one bunch decide that no intra-pattern dimensions could be allowed. All dimensions had to individually come from the edges of the parts, so that it was tedious to determine if two parts actually would assemble. Instead of comparing pattern values one had dozens of calculations to make; even one deviation between the two sets would result in garbage parts. Also ignore that this pattern was repeated multiple times, so a CNC sequence could be made once for all of them. But it sure made things easier for some hypothetical inspector.

RE: Tolerance +/+ -/-

3DDave,

What also concerns me is what the CNC programmer does with the scale model. Is Ø40.4/40.2 modeled at Ø40.3, or Ø40?

--
JHG

RE: Tolerance +/+ -/-

Quote (FeldmanWill)

That's why I always get 3 quotes. bigsmile
Now take that money you just saved and subtract it from the time you just spent on the phone railing about bad parts and waiting for rework.

RE: Tolerance +/+ -/-

The CNC programmer can program offsets from the nominal model. Offsetting is already required to change the tool path to adjust for variations between the idealized cutter and the cutter that is loaded into the machine. Anyone who blindly takes a CAD model as representing a machinable solution deserves to get what they get.

If there was a single all encompassing solution I'm sure it would have been selected already.

RE: Tolerance +/+ -/-

It is a constant issue. We all take great care in determining proper tolerances. Then, put a unilateral tolerance on something, a generous unilateral tolerance. Proceed to receive parts that are very close to nominal, but on the wrong side.sadeyes

There are no bonus points awarded for a part that measures closer to nominal.

RE: Tolerance +/+ -/-

It's entirely possible to model with a nominal dimension, a unilateral tolerance and have the geometry fall in the middle on the allowable range. I do it all the time both for CNC programing and for finite element analysis work. You just have to know how to correctly use your software. I don't care if you use ASME or ISO, the correct way to call out fits between a bore and a shaft is with unilateral tolerances. Ignorance on the part of suppliers is no excuse, get competent suppliers. At minimum, if they don't understand or question your drawing they should contact you and ask questions. If they make assumptions and start cutting chips then it's entirely on them to eat the scrap.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

RE: Tolerance +/+ -/-

" the correct way to call out fits between a bore and a shaft is with unilateral tolerances. Ignorance on the part of suppliers is no excuse, get competent suppliers. At minimum, if they don't understand or question your drawing they should contact you and ask questions. If they make assumptions and start cutting chips then it's entirely on them to eat the scrap."

remember all this is a discussion, don't let it get personnel.

if you analyze the about statement the supplier is force to work within the the tolerance given , regardless of opinions. period. as far as I am concern, I don't work to modelling. I work to drawing dimensions.,
end results would be try to hold the nominal of the tolerance. process engineers , Machinist , fabricators are going to hold the nominal of the tolerance. regardless. it is a mute argument otherwise.

RE: Tolerance +/+ -/-

To be fair, you should work to whatever your customer dictates. Most of ours tell us that the model rules when conflicts occur. A couple dictate that the models are reference-only and the drawing is law. The latter makes more sense, but the former is more reliable in some companies - especially those where the engineers are whipping things out very fast, to get quick turnaround on parts, and their drawings are more prone to errors than the model they invested most of their time in.

I also don't think @dgallup's comment was 'personal' or even wrong. Asymmetric tolerance zones is a basic, basic, rudimentary tool of drawing standards, going back a century. I have in my hand, right now, a copy of Machinery's Handbook published in 1919, and on page 880, there are tables titled "Allowances for Difference Classes of Fits (Newell Engineering Co.)" which shows alphabetic classes similar to our ANSI alphanumeric schemes today. The tables dictate "Standard Holes" tolerances at various diametric ranges, as well as tolerances for "Forced Fits, Driving Fits, Push Fits, Running Fits" and formulas for deriving your own.

98 years since it was published as a standard, necessary fact of manufacturing knowledge. No excuses from any relevant supplier that claims competence.


/edit/
punctuation correction

RE: Tolerance +/+ -/-

JNieman

I did not mean to point the finger at dgallup, I meant that as in general, my apologies to dgallap.

now I have worked with drawing that were designed before my time and many others here.
there was no GD&T, no standard for Gear Standards, it was what that standard was at the time.
in house standards. regardless I have to follow the print. it is the part of the contract we agreed to.

Currently there are a slew of standards we have to follow. if that is what you have to follow then it is what it is.
now if the model is considered a basic, then some where it has to be given tolerances, purchase order, an email, a contract
I think this is bad business , but it is regardless of what I think , it is what is contracted by customer and supplier.

I believe this trend to work to models is bad because I like data written down on paper. I can see programing cnc code from a model, then if it
conflicts with the drawing correct one or the other.
Concurrent Engineering is an essential part. and it is ashamed it does not happen more often.

But you are correct it is what ever customer and supplier agree to.
My points of view is what has worked for me, it may not work for others.

let me state a again maybe I was not clear, regardless of our point of view.
what ever type of tolerance is applied. suppliers, machinist , fabricators, have to hit between the tolerance , period.
if that was agreed to.



RE: Tolerance +/+ -/-

Of course manufacturing is going to try to mean center their product within the tolerance. I was merely saying there is no conflict between having a nominal dimension with unilateral tolerances and the model geometry in the middle of the tolerance zone so if it is used downstream for other purposes such as CNC programing or FEA it is representative of the desired end result. And as JNeiman stated, class of fit systems with unilateral tolerances have been around nearly as long as engineering and drawings.

I can quite easily create a drawing with the OP's shaft 3" +.005/+.010 and actual geometry at 3.0075".

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

RE: Tolerance +/+ -/-

Quote (dgallup)

I can quite easily create a drawing with the OP's shaft 3" +.005/+.010 and actual geometry at 3.0075".

Yes, but it sure is easier to modify a tolerance on a drawing if you don't have to adjust the model to do so. Also, downstream features in the part file may be inadvertently changed.

RE: Tolerance +/+ -/-

An other point from modeling is how is it verify by the inspection department? In our case we are AS9100 certified. First Article is required.full in house detail inspection plan is required.

RE: Tolerance +/+ -/-

The model size does not matter to the CMM. It will use the values it automatically pulls from the PMI value or from what the CMM programmer inputs, which includes the unilateral tolerance. It will create an upper and lower boundary for that feature, and it will measure the feature and spit out the actual value. It will never say "Hey, it's not modeled at an acceptable size" and fail a part. It doesn't care if it's modeled at 3.0000" with the acceptable range being 3.0005-3.0015".

RE: Tolerance +/+ -/-

"Of course manufacturing is going to try to mean center their product within the tolerance."

When the Gen 1 Chevy small block V8 was in it's heyday the production folks got the process to the point they could machine the decks consistently to the "high" side. The time saved, reduce tool wear, or whatever meant the number of blocks machined per day increased, and THAT was their goal.

RE: Tolerance +/+ -/-

Tmoose makes an excellent point. We constantly have a back and forth between engineering and our floor personnel on a similar topic. They tend to run our product to the stock safe side of the tolerance so that if something goes wrong, we have material left to rework them (i.e. running and outer diameter to the high side of the tolerance). This helps avoid scrap but also introduces unnecessary rework compared to us running at the mean of the tolerance.

Aidan McAllister
Metallurgical Engineer

RE: Tolerance +/+ -/-

Tmoose - That would explain why all those Chevies were so slow, with all their decks machined to the high side they were all down on compression.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

RE: Tolerance +/+ -/-

A star for you dgallup! That's one my Mopar buddies haven't thought of yet.

It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.

RE: Tolerance +/+ -/-

there is more than just dimensional attributes , there is heat treat requirements, non destructive requirements, thread requirements, plating and coating requirements, some close tolerance attributes have close surface finish, shot peen, radii, milled surfaces, turned surfaces, case hardness requirements, it just depends on the products. there is a million different requirements for different parts and assemblies.

RE: Tolerance +/+ -/-

Quote (mfgenggear)

there is more than just dimensional attributes , there is heat treat requirements, non destructive requirements, thread requirements, plating and coating requirements, some close tolerance attributes have close surface finish, shot peen, radii, milled surfaces, turned surfaces, case hardness requirements, it just depends on the products. there is a million different requirements for different parts and assemblies.

That should all be rendered moot on the manufacturing drawing. The person making the part shouldn't require knowledge of the behavior of steels during heat treatment, anodization growth of aluminum, or other such processes when making the part. Ideally, the manufacturing drawing should tell them what to manufacture the part to before the process, and call out the process to perform such that the result is satisfactory.

I can see the case for some things being left to the manufacturer when the process is very common, such as anodizing, and just calling out what the hole size should be /after/ anodizing, letting them figure out the in-between, but even that has its risks. This is what, I assume, @TheTick referred to when saying that the more specs you call out, the higher the price of the product. Instead of placing the knowledge, which you already have, and putting it on paper, you're instead requiring your suppliers or manufacturers to retrace your steps, and hoping they arrive at the same conclusion. This increases costs and can result in delivery delays while RFIs are processed. Sometimes the specs may cost money, that you're requiring them to get, which means you're either going to have to tell them over the phone/email what to do, hope they have it or they'll build that cost into the quote.

Ideally, the print has all the requirements for the part to satisfy the designer's intentions. Unless your supplier is also in some in-between "design-build" arrangement where you can rely on them to fill the gaps. In that case, you're likely dealing with a supplier who will not balk at, or misunderstand, unilateral tolerances.

RE: Tolerance +/+ -/-

At this point I'm turning to the idea that engineers should make the parts and just get rid of the machinists. That way there's no need to even spend the time making drawings in the first place. What use is the expertise of a manufacturer if their hands need to be held every step of the way, and they are likely to make the parts wrong anyway?

Fortunately this discussion is mostly about the engineering drawing, which is an entirely different thing than the manufacturing process drawing.

RE: Tolerance +/+ -/-

In most situations the engineering drawings are the manufacturing drawings, and provide the data for the CAM.
Our drawings cannot be drawn with a square corner and then have a note added for break, the exact break must be drawn. And this means that our drawings must be exactly in mid-range of dimensions (or where we want the nominal to be).
I can see calling a part '3" shaft' and the size being 3.005-3.010, but I would never use +/+ tol. Just too much chance of errors.

= = = = = = = = = = = = = = = = = = = =
P.E. Metallurgy, Plymouth Tube

RE: Tolerance +/+ -/-

On your custom cold drawn shapes, is the initial draw size required on the engineering drawing? How about the original billet size? Without those, how does manufacturing proceed?

I will agree, if manufacturing doesn't pay attention to the drawing there is a good chance for errors.

RE: Tolerance +/+ -/-

Quote (mfgenggear)
there is more than just dimensional attributes , there is heat treat requirements, non destructive requirements, thread requirements, plating and coating requirements, some close tolerance attributes have close surface finish, shot peen, radii, milled surfaces, turned surfaces, case hardness requirements, it just depends on the products. there is a million different requirements for different parts and assemblies.


Quote: That should all be rendered moot on the manufacturing drawing. The person making the part shouldn't require knowledge of the behavior of steels during heat treatment, anodization growth of aluminum, or other such processes when making the part. Ideally, the manufacturing drawing should tell them what to manufacture the part to before the process, and call out the process to perform such that the result is satisfactory. wrong every try to make gears that are case hardened. ever heard of a machine called a Gleason Quench Press, a good engineer will put down the final print requirements that's it.
a company we will call it Company A, decided to make there own Case Harden gears. now let be know it takes years of experience to do so.) they ended scraping out $13 millions of parts because they did not quite have the knowledge. and experience personnel to process parts correctly, Machine parts correctly, because of carburizing issues, gear cutting and gear grinding. because they were not trained properly.

I can see the case for some things being left to the manufacturer when the process is very common, such as anodizing, and just calling out what the hole size should be /after/ anodizing, letting them figure out the in-between, but even that has its risks. This is what, I assume, @ TheTick referred to when saying that the more specs you call out, the higher the price of the product. Instead of placing the knowledge, which you already have, and putting it on paper, you're instead requiring your suppliers or manufacturers to retrace your steps, and hoping they arrive at the same conclusion. This increases costs and can result in delivery delays while RFIs are processed. Sometimes the specs may cost money, that you're requiring them to get, which means you're either going to have to tell them over the phone/email what to do, hope they have it or they'll build that cost into the quote.

Ideally, the print has all the requirements for the part to satisfy the designer's intentions. Unless your supplier is also in some in-between "design-build" arrangement where you can rely on them to fill the gaps. In that case, you're likely dealing with a supplier who will not balk at, or misunderstand, unilateral tolerances.

Hmmmmm OK we don't agree sorry. but after working in Aircraft, Space, and Commercial Industries. this has always been the this way.
It is a team effort between Design & stress Engineers, Manufacturing Engineers, Quality Engineers, Lead Machinist, Lead Sheet Metal Fabricators, Lead Assembly Mechanics.
Many times it was the model shop figuring how to manufacturing parts then relaying that information to the engineer. (ever heard of a master plaster) before there were computers), or Engineers designing a part that had to be built so all the errors for assembly, or static, dynamic testing had to be verified. There no one in this world that can do it all. and if they can they are a dam genius. just think of all the type of machines, and the type fabrication that has has to be done out there. space vehicles, different types of aircraft, gear boxes, and on. ( there a million people working together on these projects)
clean room procedures, plating procedures, like mention before , castings and forgings have to be fabricated, bar stock has to be made, sheet metal has to be manufactured and all of it has to meet or exceed the specification requirements. then on the engineering side there are stress and strain, loads, cycle times, can the equipment or vehicles or the ship set bird carry the loads. which is beyond the scope of the OP post. and is now hijack. sorry about that.
Many Times it the guy on floor that finds errors from print designs. and ask hey is that correct?
tolerance how you think is correct and be done with it.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources


Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close