×
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!
  • Students Click Here

*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.

Students Click Here

Jobs

minus minus tolerance
2

minus minus tolerance

minus minus tolerance

(OP)
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
 

RE: minus minus tolerance

What is it that you need help with?

RE: minus minus tolerance

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

RE: minus minus tolerance

(OP)

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

Thanks in advance.

RE: minus minus tolerance

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.
www.qmsi.ca

RE: minus minus tolerance

(OP)
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.

RE: minus minus tolerance

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

RE: minus minus tolerance

(OP)
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!!

 

RE: minus minus tolerance

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.

RE: minus minus tolerance

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.


 

RE: minus minus tolerance

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." - Robert Hunter
 

RE: minus minus tolerance

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 -/-.

RE: minus minus tolerance

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)

RE: minus minus tolerance

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"?  smile

Here is another explanation:
http://gdtseminars.com/blog/2008/01/26/31/

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

RE: minus minus tolerance

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

RE: minus minus tolerance

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.  
 

RE: minus minus tolerance

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.   

RE: minus minus tolerance

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.

 

RE: minus minus tolerance

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.

RE: minus minus tolerance

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
www.infotechpr.net

RE: minus minus tolerance

2
The +/+ and -/- are typically used with fitting cylindrical parts to one another using the following types:

• RC = Running or Sliding Clearance Fit
• LC = Locational Clearance Fit
• LT = Transition Clearance or Interference Fit
• LN = Locational Interference Fit
• FN = Force or Shrink Fit

see also:
ASME B4.1 - 1967 Preferred Limits and Fits for Cylindrical Parts
ASME B4.2 - 1978 Preferred Metric Limits and Fits

the purpose of ISO 286-1/2 and ASME B4.2 is one for using a system of common tools, production methods, and gages. This is the description taken from the ASME B4.2 catalog:

"This standard describes the ISO system of limits and fits for mating parts as it is approved for general engineering usage in the United States of America. It establishes: (1) the designation symbols used to define specific dimensional limits on drawings, material stock, related tools, gages,
etc., (2) the preferred basic sizes (first and second choices), (3) the preferred tolerance zones (first, second and third choices), (4) the preferred limits and fits for sizes (first choice only) up to and including 500 millimeters, and (5) definitions of related terms."


for example, say we want a Ø45mm shaft/bearing assembly that requires a good positional fit but also needs to slide for assembling and for allowing movement during operation.  Now from our preferred fit tables (ISO/ASME) we find that an RC3 fit (H7/f6) is a common choice for such function and should also prove economical for our manufacturing.

on the drawing, we can easily show this as:

Hole     Ø45 H7
Shaft     Ø45 f6

now you are asked by the inexperienced shop, what is H7/f6?  so you add the tolerances:

Hole     Ø45 H7 (+0.025/+0)
Shaft     Ø45 f6 (-0.025/-0.041)

well, there is that nasty +/+, -/- again which nobody seems to like, so we can nominalize it to give:

Hole    Ø45.0125 +/-0.0125
Shaft    Ø44.967 +/-0.008

I think, it should prove quite easy to find tooling and gages (common) for a Ø45H7/f6 connection, but I would think that one should expect a few blank looks and likely additional costs if they inquired about a drill bit/reaming set and gaging for a Ø45.0125 +/-0.0125 hole and a roller burnishing tool and gaging for a Ø44.967 +/-0.008 shaft.

RE: minus minus tolerance

pmarc,

Quote
"There is a whole norm (ISO 286) that specifies:
- standard tolerances for certain ranges of nominal dimensions depending on the tolerance class"

That's not correct IMHO,
ISO 286 is only used for tolerancing shaft fits, nothing more.

Din-ISO 2768 (part 1) specifies tolerances for certain ranges of nominal dimensions (not ISO 286).

And as others have stated, it is fairly common practice in Europe.

RE: minus minus tolerance

321GO,

You are right - this was my mistake.    

RE: minus minus tolerance

321GO - DIN/ISO 286 is used for all fits, not just shafts.
DIN/ISO combines the former DIN specifications completely:
DIN 7150 T1 = ISO tol. and fits for length dim. 1 to 500mm
DIN 7151 = ISO Basic tol. for length dim. 1 to 500mm
DIN 7152 = Creation of tol. fields 1 to 500mm.
DIN 7160 = ISO - deviations for O.D. (shaft) 1 to 500mm.
DIN 7161 = ISO - deviations for I.D. (bore) 1 to 500mm.

DIN/ISO 286 replaces the following DIN specs in part:
DIN 7172 T1, T2, T3 and DIN 7182 T1.  

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