Tolerances of ISO 2768 cumulative or not?

[fsincox]

Does anyone here know if ISO 2768 tolerances are to be treated as cumulative or are they non-cumulative (as say, a basic profile without datum references).
Ken had a thread awhile back on a discussion he had with a German engineer who clamed they were non-cumlative. I like Ken had always assumed they would be cumulative between the non-dimensioned features. Does anyone out there know? Can you reference why and where this is stated?
Thanks,
Frank

 

[pmarc]

Frank,
Can you clarify what do you mean by "cummulative" or "non-cummulative" ISO tolerances?
I was not able to find Kenat's thread on this and I have to admit I am lost a little bit on this.

 

[fsincox]

pmarc,
Thanks, You seem to have some experiance working with ISO?
Sorry, it may be my teminology.
Non-cumulative, I believe would be like a part defined with all basic dimensions and an all around profile tolerance. I believe any (2) arbitrary opposed sufaces would be required to be within +/- 1/2 the profile tolerance zone. This inspite of the dimensioning scheme shown on the drawing.
Cumulative, our normal method where the non-specified or implied dimensions will cumulate a tolerance stack-up.

 

[pmarc]

Frank,
I'd like to help but I can really find a link between your issue and general tolerances (linear or geometrical) according to ISO 2768. I must have a blackout or something :-[

 

[fsincox]

pmarc,
Sorry, I am not explaining it well.
I am asking if someone knows when you reference the general tolerances under ISO 2768 are they only to be applied to the dimensions as shown on the drawing or do they also apply to the nonspecified, implied dimensions?
If (2) holes are dimensioned in the same direction from a common surface with 200mm and 220mm dimensions, does the implied 20mm tolerance between holes themselves apply as if it was directly specified under the 20mm tolerance? I am assuming, for argument sake, the tolerance band for 200mm & 220mm is much greater than that for 20mm, I don't have it in front of me now.
I would not have assumed that the tighter tolerance of the 20mm would apply, but I have heard claims that some believe it would and I would like to know if it is specified, I assume it must be, somewhere.
Any clearer?
Thanks, for trying to help.
Frank

 

[powerhound]

I'm looking at 2768-1 right now and I see no indication that tolerances are non-cumulative. I don't think the tolerances apply to unspecified dimensions. That just wouldn't make sense. In the case you present, both the 200 and 220mm dimension have their own tolerance and the spacing between the holes is not relevant. If it were, then there should be a 200mm and a 20mm dimension between the holes. I glanced through 2768-2 and saw no mention of tolerance non-accumulation.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[fsincox]

powerhound,
Thanks, I would agree with you and KENAT's original assesment.

pmarc,
Original thread, sorry Ken.

thread1103-196260

 

[fsincox]

My old copy (1989) says: "This part of ISO 2768 only applies for the following dimensions which do not have an individual tolerance indication:
a) linear dimensions (e.g. external sizes, internal sizes, step sizes, diameters, radii, distances, external radii and chamfer heights for broken edges)"

It seems primarily directed at the dimensions not the features so I would think it is dimensionally dependent.
Frank

 

[pmarc]

Frank,

Now I got your point
I can only agree with you, powerhound, Kenat and everyone else who was involved in this and the other (Kenat's) thread.

However a short comment:
For location of holes ISO 5458:1998 "Positional Tolerancing" recommends position tolerance together with basic (theoretically exact dimensions, TED) dimensions from datum reference frame instead of coordinate dimensioning. If in your and Kenat's examples dimensioning was done in proper way (according to the standard), there would be no issue at all, because basic dimensions are non-cumulative and there is a clear instruction from which datum point, line or plane they are locating part's features.

 

[fsincox]

pmarc,
Interesting point, I will look for that one.
Frank

 

[fcsuper]

Without seeing the ISO standard, I would have to still assume that tolerances of linear dimensions accumulate, since the only common way to have non-cumulative tolerances is to apply GD&T to BASIC dims.

Matt Lorono, CSWP
Lorono's SolidWorks Resources & SolidWorks Legion
Follow me on Twitter

 

[KENAT]

WRT my original thread the consensus of the US rep for the German company was that tolerances are cumulative.

On my parts, they didn't reference the second part of iso2768 for geometric controls and definitely didn't have basic dims.

So arguably they weren't using 2768 as intended by the folks that wrote it.

However, it seems a fairly typical way of using it based on other German & ISO drawings I've seen that reference 2768.

(Maybe it's analogous to the over dependence on block tols in the US, but at least with the block tols I know what I means for sure - even if it's wrong wrt function.)

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[Dazza421]

Im going to step in here because Im having this discussion at work currently.
If 2 holes are dimensioned as 200 and 220 from an edge, The manufacturer can only assume that the 2 holes have a relationship to the edge which is paramount to the correct proformance of the part. ie the 2 holes locate different fixtures correctly relative to the edge. Applying a general tolerance of +/-1mm the 2 holes may be 18mm to 22mm apart.
If those same holes are dimensioned as 200 and 20mm, the manufacturer can assume that the 2 holes hole an individual fixture or 2 fixtures having a functional relationship between them. Applying the same tol. the 2 holes may be 19 to 21mm apart.
However I donot accept tolerance stack. Just because the first hole is 1mm over dim, the second has a tolerance applied to the theorically correct position. therefore the distance between the holes maybe 18mm (first at 121, 2nd at 120+19) This effectivly reduces the 1mm tol to 0.5mm.
Dont we weave a tangled web!
Dazza

 

[powerhound]

Dazza,

I'm going to respectfully disagree with you. If I understood your post correctly, you are saying that if the first hole was called out at 200mm from the edge and the second hole 20mm from the first hole, that the second hole should really be held to 220mm from the edge instead of 20mm from the first hole. Is that what you meant to say?

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[fsincox]

It seems to me it should be very easy for someone who actually uses this to explain to us. It is such a fundamental issue on every drawing that incoporates it. If the ISO has not laid this out somewhere or is not at least is dealing with this issue it will amaze me. I can understand there is differences in opinion as there is many time with ASME issues.
Thanks,
Frank

 

[fcsuper]

ISO 129 5.1 Chain Dimensioning

"Chaings of single dimensions should be used only where the possible accumulation of tolerance does not impinge on the functional requirements of the part."



Matt Lorono, CSWP
Lorono's SolidWorks Resources & SolidWorks Legion
Follow me on Twitter

 

[fsincox]

Matt,
Thank you, for your input. It certainly does seem to indicate they are aware of the basic issue itself. Do you work with many of these drawings?
Frank

 

[fcsuper]

Not in my past. I was a ANSI/ASME guy. Now that I'm work as the Product Definition Specialist on drawings for SolidWorks, I am quickly learning ISO based standards.

In general, the recommended way to avoid accumulated tolerances is to use GD&T. I actually wrote an article about that awhile ago (before I took my new job here at SW). The article has ASME underpinnings, but the same rules are fairly universal, unless someone can find a specific statement in a specific standard to the contrary:

http://www.fcsuper.com/swblog/?p=2440

Matt Lorono, CSWP
Product Definition Specialist, DS SolidWorks Corp
Personal sites:
Lorono's SolidWorks Resources & SolidWorks Legion

 

[mikestl]

It's been a few weeks since the last post on this discussion but let me correct something (and give my opinion at the same time).

I think Dazza was the closest to explaining the intracacy here but I need to correct him/her. ISO2768 has a sliding tolerance based on the size of the dimension. For a medium tolerance class per the ISO, dimensions over 6mm but up to 30 mm have a tolerance of +/- .2mm. Dimensions above 120 but up 400 have a tolerance of +/- .5mm.

Therefore, the 200 dimension would have a tolerance of +/- .5mm. The 20mm dimension would have a tolerance of +/- .2mm.

Therefore if the drafter wanted the distance of the holes from the edge to be critical, he would have both holes dimensioned from the edge of the part (i.e. 200 +/- .5mm and 220 +/- .5mm).

If he felt the spacing between the holes were critical he would dimension the first hole at 200 +/- .5mm then the second dimension would be 20 +/- .2mm.

Therefore I feel that the drafter decides the tolerance stackup. Nothing else.

 

[fsincox]

Based on our discussions in another thread: thread1103-305454
I went back and reviewed my copy of ISO 2768-2. It shows an example drawing (B.2) with a “this-means this” implied by the referencing of general tolerances ISO 2768-mH on an example part. The dimensions are shown with the normal implied +/- tolerances on the dimensions so I still believe this must accumulate if you are interested in the distance between (2) features not directly dimensioned. Say the end of the pin and the start of the taper both listed as +/-0.3mm the distance between the (2) should be 22.5mm+/-0.6mm.
Frank