Metric Tolerances 1

[brakemeister]

I am trying to find a chart which relates the number of decimal places of a metric dimension to the, "Unless Otherwise Specified" tolerance.

In deference to the english system in which the number of decimal places does not specify the tolerance, the metric system does indicate the tolerance to be applied for the number of places.

Any leads would be greatly appreciated.

 

[Viktor]

No it does not. You should set these tolerances, for example: unspecified holes H11,shafts h12, others IT14/2. Viktor

http://viktorastakhov.tripod.com

 

[brakemeister]

I have seen such a chart. It is part of the documentation kept by journeymen machinists in europe. I was just hoping I could find a copy on the web.

The application I have is not a "fit" application but rather tolerances which reflect the capability of a manufacturing process.

 

[jimengr]

I think you are asking for DIN7168 "General tolerances for linear and angular dimensions and geometrical tolerances". This standard has 4 different degrees of accuracy for general tolerances. For example, the engineering drawing may specify DIN7168 m (for medium). For a linear dimension, the tolerance is then based on the length. For example, a linear dimension over 120mm up to 400mm the tolerance is +/- 0.5mm deviation. This doesn't cover dimensions that have tolerances for fits (H7 etc) or otherwise specified. It only applies for "parts produced by machining with cutting tools or metal-forming tools, provided there are no other standards for general tolerances for special manufacturing methods". This simply means that this standard doesn't apply to welded parts, burned or thermal cut parts (gas, plasma, or laser) and others as they have their own DIN standards for tolerances. Welding is DIN8570 and thermal cutting DIN2310 for example.

Finally, DIN7168 is obsolete and replaced by ISO2768 which is available on the ISO website. I would guess the others I mentioned are also replaced by ISO standards.

Hope this helps,
Jim

 

[GDTGUY]

The U.S. standard for indicating metric tolerances is ASME B4.3-1978, "General Tolerances for Metric Dimensioned Products". Like DIN7168, it also specifies metric tolerances based on dimension length. (However, I have not compared the values to see if they are the same as used in the DIN standard) It also offers several other methods for indicating general (or "block&quot tolerances on an engineering drawing including: decimal place indication, formulas based on International Tolerance Grades and direct reference to the ASME B4.3 standard itself.

GDT GUY

 

[pvdvyve]

Hay, in a lot of factories they use their own tolerances. I give you an example of a note of ours that is on each drawing.

ISO TOLERANCES, IF NOT INDICATED: MACHINE WORKED SURFACES
DIAMETRICAL DIMENSIONS JS13 -js13, LONGITUDINAL DIMENSIONS
JS14 - js14, OTHER SURFACES JS16 - js16.
Sometimes it's just noted:
overall tolerances:+/- 0,1mm
I'm workin' in a former American factory in Europe and I thought that workin' with those zero's after the comma was an English or American habit? I was never taught that in school over here!
Greetings
pvdvyve-Antwerp-Belgium-Europe Greetings from Belgium (Europe).