minus minus tolerance 2

[bloodydecks]

Hello,

I need some help and hope someone can help us.

We recieved a drawing that has a diameter called out like with the tolerance set as minus minus.

-0.02
Ø4.2 -0.04

 

[DanStro]

What is it that you need help with?

 

[fsincox]

It is a not an uncommon style of tolerancing, what do you not understand about it? The math is not difficult.
Frank

 

[bloodydecks]

I don't understand what it meen's. would the tolerance range
be 4.18 to 4.16?

Thanks in advance.

 

[dingy2]

The math will give one a tolerance spec range and this type of tolerancing is used quite a bit in Europe. It still blows my mind though.

Dave D.

http://www.qmsi.ca

 

[bloodydecks]

I don’t understand the logic in specifying a dimension that way either. The only thing, I can think of is the 4.2 is the minimum bore diameter of mating part, hence the 4.18/4.16 tolerance range of the diameter.

 

[drawoh]

bloodydecks,

The required dimension is 4.16 to 4.18.

I know that +/+ and -/- tolerancing rattles people, but I like it. People want the CAD file to do CNC programming. It really helps if they know the diameter of the as-modeled feature, in your case Ø4.2.

JHG

 

[bloodydecks]

Thanks for your help in clarifying this for us. That is what I thought. first time I’ve seen a callout like that in my 22 years of manufacturing. I blame it on the global market place.

This place is great!!

 

[lifttrucks]

If your customer is using the Y14.5 standard-I don't believe this is an acceptable practice.

drawoh,

This practice was used in the past at my company, but has since been discontinued because of confusion in manufacturing. Bloodydecks is not the first person to question the meaning...

Why would anyone create a feature in a CAD model that is outside the tolerance limits? This can cause issues with CNC, interference detection, etc.

 

[DanStro]

My company uses it fairly often but I've gone to limit dimensioning because I've had too many vendors assume that I really must have meant +0.03/-0.01 instead of the +0.03/+0.01 on the drawing.

 

[ewh]

While I have seen it used in the past fairly often, it does not lend itself to CNC work where the machinist generally wants the model at nominal, which is never seen with +/+ or -/- tolerancing. We now try to model (and dimension) to WYSIWYG.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[BiPolarMoment]

I have argued this point both ways before. What I will say is that -/- tolerancing is fairly common just not called out explicitely. That is when using limits/fits (e.g. Ø4.2 H7/p6 which would be Ø4.2 -0.01/-0.022 on the shaft side to maintain clearance).

Personally I don't care that much, though it does appeal to me to have a round "nominal" as it does seem to confer a little bit of design intent. If you are willing to accept non-symmetric tolerances it's not a big mental leap to +/+ or -/-.

 

[BiPolarMoment]

Woops I was thinking one thing and typed another.

In my example H7/p6 for a 4.2mm diameter would net +0.012/+0.022 on the shaft diameter to ensure interference. (The hole would be 4.2 +0/+0.012)

 

[Belanger]

In the OP's example, 4.2 is the nominal. "Nominal" just means "name," right? It doesn't mean that that's the real size of the part -- which is why (I admit) it can be confusing.

But who ever said a 2 X 4 was 2" by 4"?

Here is another explanation:

http://gdtseminars.com/blog/2008/01/26/31/

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[ctopher]

This style of tolerancing is normal, although not common.

bloodydecks,
It has nothing to do with the "global market place".

Chris
SolidWorks 09 SP5.0
ctopher's home
SolidWorks Legion

 

[pmarc]

In ISO world this style of dimensioning is nothing weird. As J-P mentions on his blog it is commonly used when limits and fits are considered. For instance a shaft and a hole which are going to fit together have the same nominal diameter and by looking only at tolerances one can almost immediately say whether the fit is loose, transition or press.

There is a whole norm (ISO 286) that specifies:
- standard tolerances for certain ranges of nominal dimensions depending on the tolerance class,
- standard fundamental deviations from nominal dimensions which are later used in fit description,
- symbology for limits and fits marking.

Y14.5 standard indeed does not use -/- description for a tolerance, but actually gives an example of limits and fits indication. In 1994 edition fig. 2-3 depicts three methods for this. And in fact cases a & b are similar to the OP's dilemma - nominal dim. is 30 but the tolerance is -/-, only the indication on a drawing could be different.

 

[dgallup]

Depending on your CAD system, you can have asymmetric tolerances, including +/+ or -/- tolerances AND centered geometry for CNC programing. Pro/E will definitely do this, I think there are others too. In the OP's situation of 4.2-.02/-.04, if I set the dimension to regenerate at the middle of the tolerance, the geometry will measure 4.17 even though the dimension nominal is 4.2.

 

[SDETERS]

The place I see this type of dimensioning used is with seals. Usually the seal company specs a 15mm seal but to get the press and slip fits they call the seal od out for example 15 +0.1/+0.2. I would rather prefer limits makes things a little bit more clear to me.

 

[TheTick]

It's technically legal by some standards. I would never allow it on any of my drawings due to the confusion it might cause (OP's post is case in point). When I make a drawing, the goal is to get a good part. Making fabricators do extra math is counter to that goal.

 

[PeterStock]

Not to mention the odd vendor who makes the part to the cad model then looks at the drawing - opps. I can live (barely) with 15 +0.3/-0, but 15+0.1/+0.2 will not be released with my signature on it.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net