10 Replies Latest reply on Jul 23, 2013 5:22 PM by John Burrill

    Geo-Tolerance vs Default Drawing Tolerance

    David Clough

      I have a question about Geo-Tolerancing.  When showing a geo-tolerances in a drawing, does that negate, for those specific dimensions, the default standard tolerances shown in the title block.    In other words, when you specify a tolerance (not geo-tolerance) in a drawing, then the drawing tolerances are being over-ridden.  Does this also apply with geo-tolerances?  Our QA is adding using both, meaning that our sheet tolerance is +/-.005 AND adding another +/-.002 for geo-tolerance yielding an overall +/-.007.  I feel this is incorrect, that the sheet tolerance is omitted since there is another tolerance shown; whether standard sheet tolerance or geo-tolerance.  Any thoughts??  Thanks,  David

        • Re: Geo-Tolerance vs Default Drawing Tolerance
          Mike Agan

          I would say ,yes, it does negate the default tolerances.

           

          edit: I believe our "default" says unless otherwise specified

          • Re: Geo-Tolerance vs Default Drawing Tolerance
            Josh Brady

            Dunno if you need this to be a "pile on QA" thread, but I concur with Mike.  Now that you know this about your QA person, every single thing that's ever been inspected by them is now suspect.

            • Re: Geo-Tolerance vs Default Drawing Tolerance
              Paul Marsman

              most definately should not be adding the two tolerances together.  The block tolerance is as Mike says "Unless Otherwise Specified" and you are specifying otherwise!

              • Re: Geo-Tolerance vs Default Drawing Tolerance
                Matthew Lorono

                To add to Josh's comment, I would question is the individual knows how to read (not interpret) the Feature Control Frames and how they apply to the part.  For example, a positional tolerance with a diameter symbol has a completely different shape for its tolerance zone than a +/- tolerance, and these two cannot be measured using the same methods.

                • Re: Geo-Tolerance vs Default Drawing Tolerance
                  David Clough

                  Thanks everyone.  Most of our drawings have the tolerances shown, without utilizing geo-tolenancing.  Looking at one of our older drawings, though, is where this question came up.  Thanks for clarifying and expounding on this for me.

                  • Re: Geo-Tolerance vs Default Drawing Tolerance
                    John Burrill

                    You can use block tolerances in conjunction with GD&T for features of size.

                    For example, you can say that a boss is Ø.500 and has a cylindricity tolerances of .002.  If you have a block tolerance of ±.005 then you can have a .495-.505 boss but it can only taper .002

                    Now for something like true position of a hole, you can use a block tolerance for the size of the hole and incorporate that into the size of the tolerance zone (effectively expanding the positional tolerance for the center when the hole is bigger than minimum size) but true position is based on a theoretically precise location-usally called out with basic dimensions so you can't say that a hole is 2.500±.005 from an edge with a true position tolerance of Ø.014 with respect to a datum reference frame.

                    With profile tolerances, all dimensions going into the definition have to be basic with respect to the datum reference frame

                    I would say that if your QA person is having a hard time interpreting GD&T it's worth the time and resources to make sure they're fully trained and not simply left to come up with their own meanings.

                    That's how people wind up using concentricity.

                    • Re: Geo-Tolerance vs Default Drawing Tolerance
                      David Clough

                      So in my case, the problem we have is, drawing default tolerance is +/-.005.  The part is a shaft, that is cut .003 off of centerline X .320 deep.  So with just that being said, we can cut between .008 of one side of CL, and .002 on the other.  The geo-tol added to the original drawing is:      'profile of a surface' / .002 / and the datum is the OD of the part.  So the way I would read this is that the cut path, can not deviate more than +/-.001 (.002 total).  The question is, does the +/-.005 still apply?  If so, does the path deviation HAVE to fall with-in the +/-.005?  All of this is basically for my future knowledge, because before I started here, the drawing was revised, and there is no longer any GD&T on our drawings.  Thanks

                        • Re: Geo-Tolerance vs Default Drawing Tolerance
                          Paul Marsman

                          David,

                            Can you post the before and after drawings in question (or a mock-up of it)?  It would just make answering your question for sure correctly much easier than assuming we have deciphered your paragraph properly.  Picture worth a thousand... you know

                           

                            Without that, I would say based on what you have said that the profile tolerance of .002 is the only tolerance that is require to position the off center cut (including the .320 deep dimension)  The block tolerance of .005 is ignored for all details of the cut because the profile defines the tolerance required.

                           

                            Really, block tolerances are just a way to say: "if I don't specify a tolerance, use this"

                           

                          Paul

                        • Re: Geo-Tolerance vs Default Drawing Tolerance
                          David Clough

                          OK, here's a snap shot of it... dimensions in question is .003 @ Detail B.

                           

                          Hopefully this helps.

                           

                          Retainer Snapshot.JPG

                            • Re: Geo-Tolerance vs Default Drawing Tolerance
                              John Burrill

                              Yeah, they're not using Profile correctly there.  No wonder your QA guy is getting confused.

                              When you use profile, you have to show someone how to get to the nominal surface from the datums.  I'll ignore the unconstrained translation for the moment  The .003 dimension should be basic and the CL should be located with a basic angular dimension to the Datum B slot.

                              Then, in the stack-up, you could have that surface .001-.005 off that theoretical centerplane