25 Replies Latest reply on May 3, 2018 7:59 AM by Kevin Chandler

    Perpendicular GD&T on a Radius cut???

    Kevin Andrews

      I have a situation where I am having to produce a drawing for an additional machining step to be done after the original machining was done.

       

      In other words, someone screwed up and did not allow enough clearance for a couple of bolts in a cylinder head. Since there is already a drawing for the original machining operation, I am simply providing details for the additional machining to be done for clearance. This drawing will only be used for the previously machined parts. I will provide a revision drawing for the casting and machining going forward.

       

      Since the cylinder head is cast, there is draft added to the pull direction. The inside of the cylinder head (the cavity) does not get machined - just the mounting holes and the mating surfaces. This means that the inside walls of the head have draft on them as well (1° draft). Please refer to picture below:

       

      The plan is to have the machinist use a Ø3/8" end mill to do a plunge-cut in one corner and then mill over to the other corner. The depth of the plunge should be 0.357 from the finished, previously machined, surface [A]. The distance from the inside edge of the cavity is less than 3/16" (less than half the cutter Ø).

       

      This clearance cut MUST be perpendicular to the face of the finished surface [A]. When I am detailing the drawing, I am calling out the radii on the cuts because it is not showing as a hole. I am applying a perpendicularity GD&T with a tolerance diameter of Ø.016 in reference to datum A. However, this looks a little strange to me. Anyone else ever encounter a GD&T callout for axis perpendicularity with a diametrical tolerance?? See detail below:

       

      Does this look odd or improper to anyone else?

       

      Sorry for such a long description and question

        • Re: Perpendicular GD&T on a Radius cut???
          Ruben Rodolfo Balderrama

          Add some extra lines to define one limit....read the ASME Y14.5

          • Re: Perpendicular GD&T on a Radius cut???
            Kevin Chandler

            Hello,

             

            An aside: I don't know if this a final pass for these dims, but I suggest that one of them needs to be a reference:

            Also, I believe the diametral symbol isn't required for this situation.

            Remove that and your radii will be constrained between two parallel planes 0.016" apart that are square to A.

            Note that I said the "radii" because, as shown, the GD&T doesn't apply to the intermediate flat.

            (EDIT: By "radii", it's only the two R.188" ones. Might want to look into doing a profile for this.)

             

            Not sure what "ROUND SHARP CORNERS" gets you. R.125" will be as sharp as what a 3 place dim defaults to.

            But if you're looking for tangency, perhaps dim to the R.125 center marks.

             

            I hope this helps (I'm oh for one today: how to edit polygon, add sides/points, to crop view in .SLDDRW?  )

             

            Cheers,

             

            Kevin

              • Re: Perpendicular GD&T on a Radius cut???
                Kevin Andrews

                Yes, there is an inspection dimension relative to this section in another location of the drawing.

                 

                Have you ever been typing something, and someone will start talking to you, and then - all of a sudden - you realize that you have typed something that the person talking has just said?? Or - maybe you were thinking something specific, in your head, and wanting to put down something generic on paper - but instead put down the specific?

                 

                Now that I really have you going, "HUH?!?!?!"...When I was typing in "Round Sharp Corners", I was, literally, thinking of a 1/8" radius...and instinctively typed in "R.125" without even realizing that I had done it. Luckily, my co-engineer caught it and asked me about it as it went through "Engineering Check"

              • Re: Perpendicular GD&T on a Radius cut???
                Jason Edelman

                A few points I see;

                - the Diameter symbol after .016 is incorrect, diameter symbol is only referenced for cylindrical features

                - if intended to use a 3/8" tool (.375") the Radius should be over sized (.005-.010" or so) so the tool interpolates the radius

                - have the R.125 extend past cast surface and lead out of casting (those will never be tangent to casting face)

                 

                Question what is the critical nature of the flat (2.375") between Radius? Does that need to be perpendicular to Datum A also?

                • Re: Perpendicular GD&T on a Radius cut???
                  Dan Pihlaja

                  Does it matter if the radii are perpendicular, or just the flat face?

                   

                  Honestly, here are a couple of ways I would do it:

                   

                  OR

                   

                    • Re: Perpendicular GD&T on a Radius cut???
                      Kevin Andrews

                      While everyone has pointed out great information - Dan has given me the answer I was looking for. I do not need to put a perp tolerance on the radii - I need it on the face of the inset. Why I did not realize, nor think of, this earlier is beyond me...I will play the "blame game" and say it is attributed to the 3.5 hours of sleep last night.

                       

                      But I do have a question concerning the tolerance in the perp GD&T you show in your first example. Obviously, the "perp" symbol indicates that the face is to be 90° to A....so, what does the .016 refer to? This always throws me because I am thinking angular dimensions - but, in this case, it refers to a set of parallel planes, .016 apart, that this face can reside within - and, so long as no part of the face is outside of that box, it is within tolerance...

                       

                      Maybe I just answered my own question....verification would be appreciated.

                        • Re: Perpendicular GD&T on a Radius cut???
                          Dan Pihlaja

                          Yes, that is exactly the case.  Although in this situation, the perpendicularity tolerance should be less than the tolerance that you have placed on the dimension that defines the position of the face of the inset.   This is because perpendicularity does not control positon.   However, your +/- tolerances do (assuming you are using the ASME Y14.5M standard).  Your perpendicularity (man, that's a big word to type!) tolerance is something that resides within your +/- tolerances for that surface.

                          To explain further:

                          Regardless of the perpendicularity tolerance, if your +/- tolerance for the face of the inset was +/-.010", then you already gain a perpendicularity of .020, because with ASME Y14.5M standard, no portion of the entire surface is allowed to fall outside of the +/-.010" tolerance zone..   If you need this modified to be tighter with regards to perpendicularity, then you would add your perpendicularity callout.

                            • Re: Perpendicular GD&T on a Radius cut???
                              Kevin Andrews

                              "Perpendicularity" is not only a long/hard word to type, I find myself, somewhat, stuttering - or having to think about each syllable - when I say it.

                               

                              Thanks for the deeper clarification. I currently have the face at a +.031/-.000 from a set point on the body. Being that the location tolerance is 1/32", the 1/64" (.016) perp tolerance would still be "necessary" in order to ensure a truer (is that a word?) parallel face.

                            • Re: Perpendicular GD&T on a Radius cut???
                              Jason Edelman

                              I think what you are picking up on is the GD&T in Dans suggestions is half correct, Perpendicular .016 A is adequate, but the controlling dimension 0.188 is referencing a cast surface, the controlling dimension needs to be from machined feature, helpful if it is/can be the same as how the machinist is going to 'pick-up' orientate the parts when altered.

                                • Re: Perpendicular GD&T on a Radius cut???
                                  Christopher Culver

                                  I agree, and how it is intended to go together is critical in defining the tolerances. I would create a dimension/tolerance to that feature from another important machined feature that should also have associated tolerances.

                                    • Re: Perpendicular GD&T on a Radius cut???
                                      Kevin Andrews

                                      I am not dimensioning to any portion of the casting.

                                       

                                      This is an amendment, if you will, to an earlier machining drawing. We are sending these parts back to our machinist and supplying him with this new print. For reference purposes, I am only dimensioning the addition to the part and have referenced existing machined locations (from previous machining drawing) for location. If that makes sense.

                                    • Re: Perpendicular GD&T on a Radius cut???
                                      Dan Pihlaja

                                      Jason Edelman wrote:

                                       

                                      I think what you are picking up on is the GD&T in Dans suggestions is half correct, Perpendicular .016 A is adequate, but the controlling dimension 0.188 is referencing a cast surface, the controlling dimension needs to be from machined feature, helpful if it is/can be the same as how the machinist is going to 'pick-up' orientate the parts when altered.

                                      Agreed.  I didn't even think about the fact that it was a casted surface.   Yes, needs to go back to a datum of some sort.

                                    • Re: Perpendicular GD&T on a Radius cut???
                                      Kevin Chandler

                                      Kevin Andrews wrote:

                                       

                                      While everyone has pointed out great information - Dan has given me the answer I was looking for. I do not need to put a perp tolerance on the radii - I need it on the face of the inset. Why I did not realize, nor think of, this earlier is beyond me...I will play the "blame game" and say it is attributed to the 3.5 hours of sleep last night.

                                       

                                      But I do have a question concerning the tolerance in the perp GD&T you show in your first example. Obviously, the "perp" symbol indicates that the face is to be 90° to A....so, what does the .016 refer to? This always throws me because I am thinking angular dimensions - but, in this case, it refers to a set of parallel planes, .016 apart, that this face can reside within - and, so long as no part of the face is outside of that box, it is within tolerance...

                                       

                                      Maybe I just answered my own question....verification would be appreciated.

                                      What is your 3 place tolerance?

                                      If it's <= 0.008", then the perpendicularity or profile mentioned, doesn't have effect. GD&T isn't required.

                                      If your size tolerance is less than your form tolerance, size will restrain your profile, else the part is out of spec on a size violation.

                                  • Re: Perpendicular GD&T on a Radius cut???
                                    Mahir Abrahim

                                    Edit: Of course I see Dan Pihlaja's answer after I reply. His second method is exactly what I was suggesting.

                                     

                                    Kevin Andrews wrote:

                                     

                                    This clearance cut MUST be perpendicular to the face of the finished surface [A].

                                    Sounds like the entire cut is supposed to perpendicular, not just the radii. If that's the case, You're better off calling out a surface profile of .016 relative to datum ABC. That will make the entire surface +/- .008 relative to basic. Speaking of basic, if you do use surface profile, make EVERYTHING basic. That includes the 3 linear dims that Kevin Chandler boxed as well as the radius dimensions (both .188 and .125). To make it more clear, you can label the start/end points as X/Y and call out the surface profile X<=>Y. Lastly, for a non-cylindrical milled cut, you should really call out that .357 depth in a section instead of using a hole depth symbol. I know what is being communicated, but it's klugey.