Concerning tolerance for linear masurement

[Tartof]

Hi,

The question is presented in the picture below

Kindly
Paul

 

[drawoh]

Tartof,

You have not specified a standard.

ASME Y14.5 specifies that any measurement between the two surfaces lies between the specified tolerances. Any geometry that allows that, is legal. Watch out for the angle tolerances on your drawing title block. According to ASME Y14.5, this is what controls the perpendularity of your sides.

I understand ISO is different.

JHG

 

[btrueblood]

As drawoh says, any geometry. One could take a pair of calipers, and apply the measurement at any point within the 400x400 area and if it measures within tolerance, then ok. Again, using ASME Y14 definitions.

 

[dgallup]

ISO 8015: Technical drawings - Fundamental tolerancing principle will give you a totally different result. According to it the definition of a linear tolerance only controls the actual local size (2 point measurement) of a feature. If you want to control form you need geometrical tolerances or invoke the envelope requirement.

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

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.

 

[Tartof]

Sorry, i thought this was same for all standards. I am using the ISO standard. What i am concerned about is if the measurement given in the picture with the tolerance, also includes Flatness.If it is based on cross sections then it does not include flatness.

btrueblood
My intepretation of what you said when you mentioned calipers is that you imply that it is govern by cross sections because the caliper does not cover the entire surface?

You used the word points, which is even more limiting then cross sections.

 

[CheckerHater]

The answer is "Yes"

 

[fsincox]

I think the ASME standard now only controls "directly opposed- features of size" not "any geometry". That is what we all thought it covered, before the 1994 version. In the simple example here it would be covered, true.
Frank

 

[CheckerHater]

You can add Envelope requirement to your dimension:

20+/-0.5(E) (It's "E" in circle)

Then it will include flatness.

 

[Tartof]

So when manufactued the detajl could look as in the picture i have attached?

Do anyone know in what section in ISO 8015 i can read about this?

 

[Tartof]

Sorry forgot to insert the link

 

[pmarc]

In ISO 8015:1985 you can read chapters 4 and 5.

However there is newest version of this document issued this year and the independency principle is described in clause 5.5.

 

[CheckerHater]

You may be out of luck if your print invokes ISO 2768-2.

Also, ISO 1101 (if specified)automatically invokes 2768.

Boy, I love where this is heading!

 

[Tartof]

The reason i ask this is that i want my drawings to be correct we do not need to go in to the detajls. Here in Europe most drawings refer to ISO 2768-2 in the drawing header.

So ISO 2768-2 is a subsection to ISO 8015 or how does that work?

 

[CheckerHater]

There is a pair of standards, ISO2768-1 dealing with untoleranced dimensions, and 2768-02 dealing with unspecified geometrical tolerances.

They are causing some controversy and are not universally loved on this forum.

You can take a quick look at this picture:

http://www.globalspec.com/reference/43769/203279/chapter-16-general-geometrical-tolerances

It shows "invisible" GD&T implied by referencing 2768.

 

[pmarc]

ISO 2768-2 is a separate standard. It defines general tolerances for some of geometric controls. And the flatness is amongst those controls.

It means that if you refer to 2768-2 on a drawing the flatness is limited even that nothing else beside single dimension is shown on a print like in your example. According to the standard the intent of this is practice "to simplify drawing indication"...

Another important thing which is very often overlooked is that ISO 2768 (parts 1 & 2) are dedicated for parts "that are produced by metal removal or parts that are formed from sheet metal". This means that if your part is for instance a plastic plate formed in an injection molding process, refering to ISO 2768 is not a best choice.

 

[fsincox]

ISO and ASME are not the same!
ISO 2768-2 will specify default controls for things like flatness, if it is being invoked on the drawing properly (say"-mK", or such)?
Frank

 

[Tartof]

This makes me wonder, because i have seen drawings who only refer to ISO 2768-2 and not ISO 8015. Does that mean that the drawing don't have a standard?

 

[CheckerHater]

Quote:

"In any event, general geometrical tolerances in accordance with this part of ISO 2768 should be used when the fundamental tolerancinf principle in accordance with ISO 8015 is used and indicated in the drawing"

 

[pmarc]

That is right. Whenever a drawing refers to 2768-2 it also has to refer to 8015, otherwise the standard indication is incomplete.

 

[ak762]

Could someone clarify how to correct interpret meaning "length of the shorter side" in ISO 2768-1 general tolerance for angular dimensions.
if angle "d" was defined which shortest side will be use A or B?