3 Replies Latest reply on Apr 17, 2014 1:22 PM by Matthew Lorono

    Undimensioned features tolerance

    Ethan Zalkus

      I was recently presented with a problem involving tolerances for undimensioned features on a drawing. We have a note on all drawings stating that the parts are controlled by the Solidworks database and that the 3D model takes precedence over the drawing and a box in the title block stating "Unless otherwise specified..." with a basic tolerance of .XX is +/- 0.25. So we have this part that was not fully dimensioned on the DWG, and the MFG. used the 3D to pull a dimension off of. The measurement taken was 16.50. I would think they should hold to the +/-0.25 that is stated on the DWG sheet, am I wrong to assume this? Is there any "standard" that would cover a situation like this?

        • Re: Undimensioned features tolerance
          Christopher Estelow

          I think ASME Y14.41-2003 is what you are looking for.  Here is a brief overview of what it is for.  It is specified in cases where the drawing and the 3d model are used.

           

          Chris

          • Re: Undimensioned features tolerance
            Roland Schwarz

            This is an abhorrent practice.  It can be misinterpreted in so many ways.  ±.25 from what?  Can two holes that are .5 apart have the same tolerance as those 200 apart?

             

            At the very least, specify datums from which to measure.  Using a blanket GDT surface profile callout with specific datums is much less confusin (though still likely to cause trouble).

            • Re: Undimensioned features tolerance
              Matthew Lorono

              Applying a general tolerance to solid models is a practice of growing popularity.  Simple +/- tolerances don't work for the reason stated by Roland.   Where is the tolerance applied from? Your part is basically undefined.

               

              There are currently three options to fully define a part from the solid model (as of ASME Y14.5-2009):

               

              1.  Add all dimensions in the model space that would've been added to a drawing (full PMI - ASME Y14.41-2012 covers requirements for this).

              2a.  Declare the model as Basic, and apply one Profile feature control frame to all surfaces referencing stated A, B and C datums.

              2b.  Declare the model as Basic, and apply one Profile feature control frame with ALL OVER modifier. I talked about this here some time ago: http://www.fcsuper.com/swblog/?p=213

               

              The safest bet is #1, but time savings isn't quite as good as #2a or #2b. 

               

              #2a is fairly clean, but relies on knowing what is A, B, and C datum on every part.  (Three datums are not always required/available, nor is it always possible to apply these to design intent.)

               

              #2b is cleanest and most consistent, but you'll have to work out with your vendors on how you will judge their final products directly against a solid model on a computer screen.  3D scanners are getting much more accurate these days, but the better ones are still pretty costly.  You can use the same methods as you do for #2a (CMM or OC), but some dissemination of data will have to occur for undimensioned features.

               

              Edit:  These are all Model Based Definition methods (that is, defining the product from the model)

               

              Message was edited by: Matthew Lorono