9 Replies Latest reply on Jun 19, 2018 12:42 PM by Elisabeth Daley

    General profile tolerance and tolerance status

    Elisabeth Daley

      I've got a question about exactly how the General Profile Tolerance from 2018 interacts with other callouts when the Tolerance Status is calculated.  Say I've added the following DimXpert callouts, and a general profile tolerance:

      When the Show Tolerance status is on, the entire part is green, indicating that all of the tolerances are fully defined.  This is intuitive to me, because I initially assumed that the purpose of the general profile tolerance was to apply to every feature that wasn't fully defined by other more specific callouts.  However, I've been told that according to the GD&T standard, because the hole diameter has been added and there is a positional tolerance applied to it, the general profile tolerance should not be applied to the hole's diameter, and that in order to fully define it's size, it should be .53 +/- .005.

       

      Can anyone point me to clause in the standard that specifies this?  It seems like a fairly nuanced point, but has implications for whether we put a typical general profile tolerance block on our MBD drawing formats.  It would be nice not to have one, so as to minimize confusion about whether the GD&T general profile tolerance or the drawing format general tolerance applies.

        • Re: General profile tolerance and tolerance status
          S. Casale

          No matter of the feature, True Position requires a theoretically perfect dimension to locate it. This is the function of the basic dimension (boxed dimension). The M (Max material condition is additional allowable.  ASME Y.14-5 2009 1.3.64.

           

          The hole should be inspected with the plate measured from the Datum A then B then C. Per the order displayed in the control frame. Regardless of the size of the plate +.010 (.020 total) out or in, from the surfaces the Ø.53 hole axis should be within Ø.0197 projected from the front of the part thru the back for the part (rule number 1).

          • Re: General profile tolerance and tolerance status
            Dwight Livingston

            Elisabeth

             

            In ASME Y14 standards since Y14.5-2009, ASME uses the term "default tolerance" instead of "general tolerance". Even in Y14.5, they don't quite say "general tolerance" except in an aside and in the index, and instead refer to the "general tolerance block". In any case, a default tolerance (or a general tolerance) must be called out using the phrase "Unless Otherwise Specified" (see Y14.5-2009 2.1.1 (e) or

            Y14.100-2017 4.27.2 or  Y14.41-2012 1.3.10). In that case, the default tolerance does not apply where a different tolerance is applied in a figure.

             

            I do not have SW2018 and I have not used the "general profile tolerance" feature.  In the image you show, it appears to me to be non-standard and seems, as Dan says, ambiguous as to which tolerance applied. I'd say that, as shown in the image, it doesn't mean anything. If you add the phrase "UNLESS OTHERWISE SPECIFIED" to it, then it becomes a general note specifying a default tolerance and the local hole tolerance applies. I would group that general note with other general notes under the heading "NOTES", all in one plane if you are making a digital drawing.

             

            Dwight

             

             

            From ASME Y14.5-2009

             

            2.1.1 Application

            Tolerances may be expressed as follows:

            (a) as direct limits or as tolerance values applied directly to a dimension. See para. 2.2.

            (b) as a geometric tolerance, as described in Sections 5 through 9.

            (c) in a note or table referring to specific dimensions.

            (d) as specified in other documents referenced on the drawing for specific features or processes.

            (e) in a general tolerance block referring to all dimensions on a drawing for which tolerances are not otherwise specified.

             

             

            ASME Y14.41-2012

             

            1.3.10 Unless Otherwise Specified (UOS). The phrase “unless otherwise specified” or UOS is used to indicate a default requirement. The phrase is used when the default is a generally applied requirement and the exception can be clarified by providing a reference to another document or requirement.

             

            8.2.1 Notes Area Annotation Plane

            When general notes, flag notes, and special notations are placed in a model, they shall be placed on a single annotation plane or use a similar method. When displayed, these notes shall not rotate.

             

            8.2.2 General Notes

            General notes do not require associativity. General notes may include default tolerance(s) for the entire model.

             

             

            Y14.100-2017

             

            4.27.2 Commonly Used Words and Phrases

            The phrase “unless otherwise specified” or UOS shall be used to indicate a default requirement. The phrase is used when the default is a generally applied requirement and an exception may be provided by another document or requirement.