18 Replies Latest reply on Aug 4, 2012 12:21 AM by John Burrill

    gdt tol block question

    Scott Cole

      i have a note on a drawing wich says "face of fitting must be perpendicular to axis of thread within plus or minus 0 deg 10', how do i put that into a tol box?

        • Re: gdt tol block question
          Harold Brunt

          First question that pops into my mind is how in the heck did that get inspected? If it is getting inspected, that will be a clue as to how the control frame should be constructed. If not then the fitting face should be defined as a datum surface. Then you can assign a positional callout to the thread to the global datums and further define the position with either an angle or positional callout to the flange datum. personally I would use the positional since it is the easiest to measure. You will need to calculate what the positional error would be relative to the reference surface for 0deg 10' for the thread depth.

          • Re: gdt tol block question
            Scott Cole

            how do i put the drawing into this post?

            • Re: gdt tol block question
              Scott Cole

              here is the part i am talking about

                • Re: gdt tol block question
                  Tony Cantrell

                  in the tolerance frame, hold the "Alt" button and type in 241 using the key pad for the ± and 248 for the ° symbols.

                  go here for a list https://forum.solidworks.com/docs/DOC-1205

                  • Re: gdt tol block question
                    Harold Brunt

                    I can appreciate your frustration if you are simply updating the print to GD&T because I can't believe that part was ever inspected to those dimensions. Here's what I am talking about: 0 deg 10' = .166 deg; take the tangent and multiply by the width of the surface of the flange (about .5") and that's .0015". Plus or minus .0015" as measured from a threaded surface. Consider the surface area on the flange with the chamfers and slots. Then consider how are you goung the establish the dimension of the thread? Center line, minor, major or pitch diameter? And that's a standard thread callout too so not much to work with.


                    I don't want to come off as though I'm ambushing you here just that those tolerances are not realistic and you have an opportunity to fix it. If you want to let it ride, assuming this is a mostly turned part my suggestions are:

                    • Make the flange surface datum 'B'
                    • Add a Datum 'C' using one of the flats
                    • Add a Positional callout from the across the CL from flat to flat to establish the postion
                    • Change the Concentricity callouts to Positional (easier to inspect) unless this part spins
                    • Calculate the the max allowable error for Datum 'B' (the flange) and the thread so that the Perpendicularity callout is referenced to Datum 'A' (easier to measure) and use a positional callout for the thread


                    You won't be using a plus or minus anything in a GD&T control frame if you take my suggestions or not and it will be expressed in inches (in your case).


                    Hope I'm not coming off as too harsh. Not my intent at all.....

                  • Re: gdt tol block question
                    John Burrill

                    Scott, GD&T works differently from plus-minus tolerancing-especially with respect to angles.

                    The upshot is that it doesn't tolerance angled features with allowances for deviation in degrees.

                    In your case, you define the tolerance as the space between two planes perpendicular to Datum A that youre surface has to land inside.


                    The entirety of GD&T is based on these theoretical volumes that say where the feature has to be when it's inspected so specifying ± degrees is not supported.  If you need to tolerance the face that way, use a regular angular dimension.

                    Also, Datum B isn't really serviing much of a purpose.  You've already qualified the counterbore.  Finally, concentricity doesn't do what you think it does.   Concentricity is for defining the center of rotation of an irregular form like an extruded prism.  It's rarely used correctly. If this part is stationary in it's application, use position with a diameter symbol.  If the part rotates or acts as an idler or cam, use runnout.

                    finally, if you're going to be designing using GD&T and not just applying notes other engineers give you you should by a book on Y14.5 and ideally: take a class.  The standards books are sold by ASME and they're expensive.  IHS Drawing Requirements Manual 9.0 combines several standards into one book.  TechEase offers pretty good training. 

                    Good luck.