Tolerance +/+ -/- 8

[FeldmanWill]

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

 

[DanStro]

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

 

[JNieman]

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.

 

[tygerdawg]

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

http://www.bluetechnik.com

 

[3DDave]

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

 

[ornerynorsk]

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.

 

[FeldmanWill]

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

 

[JNieman]

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'.

 

[drawoh]

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

 

[hydtools]

MIL-TFP-41 seems reasonable.

Ted

 

[mfgenggear]

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.

 

[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.

 

[FeldmanWill]

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.

 

[3DDave]

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.

 

[drawoh]

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

 

[TheTick]

That's why I always get 3 quotes.

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.

 

[3DDave]

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.

 

[Nescius]

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.

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

 

[dgallup]

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.

 

[mfgenggear]

" 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.