12 Replies Latest reply on Sep 9, 2014 3:42 PM by Timothy Bratton

    How to create drawing dimensions of this part

    Fred Vraj

      Hi everybody,

      I have been trying to create a part drawing ( attached ) for my machinists but I am not able to fine the right way.

      I need him to see the center of the large face cut out as well as all the radius values. He needs to set his center point to mill the cut out.

      The OD of the green pipe is 63.5 mm and the bend of the green pipe is R75 mm ( center line of the pipe. )

      I am attaching the joint.

      I do appreciate all your  help....

      Thank you very much

        • Re: How to create drawing dimensions of this part
          Jan Forkovic

          Hi,

          hard to dimensioning and machined this surface. Intersection area is part of the torus. This will be a task for 3D milling machine I think better way is drill cylinder hole to pipe and ball joint to weld to this hole.

            • Re: How to create drawing dimensions of this part
              Fred Vraj

              Hi Jan,

              thank you very much for your input.

              I do agree that hole in the pipe would be the way to go however i got to go the hard way unfortunately. I think you are right about the milling part. I have not figured out how to dimension this part yet. I will see if I get any more replies otherwise I might have to manufacture this part manually and see how it fits. I hope I will not have to do 100 of them:-)

              • Re: How to create drawing dimensions of this part
                Fred Vraj

                Hi Jan,

                I have just checked your EDITED PART and it would be much easier...Yes.

                I will still wait if I get more replies anyway. It is very good to see people writing inputs so we can all learn something new.

                I like it! It makes us all better which is the main reason of this forum:-) Thank you so much!!!!

              • Re: How to create drawing dimensions of this part
                Jamil Snead

                Here's what I came up with. I don't know how easy it is to interpret, though. Note that the initial view is perpendicular to the plane that the pipe curve lies on.

                partdwg.PNG

                  • Re: How to create drawing dimensions of this part
                    Fred Vraj

                    Hi Jamil,

                    I thought doing simillar...look below..

                    I was trying to give to our CNC guy his CENTER POINT for the TOOL PATH.

                    I am actually CNC programmer and operator ( Milling, Turning , CNC Centers )

                    but we dont do steel  at my current place ( only ALLU ) so I need to send it out on stronger CNC.

                    MACHINE PARTS.JPG

                      • Re: How to create drawing dimensions of this part
                        Lenny Bucholz

                        any good cnc guy only needs the part file for SW or an export of a step, parasolid or iges, the drawing is just for reference.

                         

                        the cam program will cut it just fine.... do this everyday for 20 yrs.

                          • Re: How to create drawing dimensions of this part
                            Fred Vraj

                            I agree but that really heavily depends on what equipment they have. If they do use CAM program, they rely on numbers and calculation only.

                            I have been using GibbsCam myself  for many many many years but again, it is not connected to theirs machines so I can not post it over.

                            ( POST FILE WOULD NOT BE CORRECT )

                            Unfortunately there are many businesses without CAM even these days.

                            But I agree Lenny and I do appreciate your help !!! Thank you

                          • Re: How to create drawing dimensions of this part
                            Jamil Snead

                            Knowing what the part geometry is I can understand your drawing, but I'm not sure it would be entirely clear to someone who doesn't have the model. Firstly, I don't think that line in the top view is actually intersecting the center of the sweep. In my example section A-A was going through the arc center, and it is not in the same place as your 22 degree line. Also, the arc in the bottom view is sort of misleading, because the path is not actually normal to that view, so the actual path viewed from that angle would be an ellipse. To get a view where the arc is actually a circle you'd need a view coming off at the 22 degrees, which is why I did the Section View A-A. Lastly, you are missing the radius of the cut profile 31.75 mm (the radius of the green pipe). I have Section B-B to show this dimension (1.250 in).

                        • Re: How to create drawing dimensions of this part
                          John Blotnick

                          Apparently its the pipe that attaches to the green pipe that needs machining.  If the machine shop has the ability to roll its own pipe, might it be simpler to put a slice in the pipe drawing, do a flat pattern, roll it and weld the seam?  The next piece - the adapter - if not a store bought can be machined separately and welded in.

                           

                          John

                          • Re: How to create drawing dimensions of this part
                            Timothy Bratton

                            Tough one dimensioning the compound radius, do you not have #D Model capable CNC programming?

                             

                            If i were to attempt to dimension this I would need the centerline of the path of the green part it is being welded to, and then dimension that in relationship to the ball and then provide the radius size according to that path.

                             

                            Considering we use the 3D model for programming I would simply NOTE: "Machine to Model" and move on.

                             

                            I think you will find they will require fixturing for this weld job, and the final piece they actually weld on for the "ball joint" will not look exactuly like your model.  It will need scalopped for welding, and probably need to be releived.  Basically the cut through the ball joint related to the frame would need to have a gap, not be a perfect mate, as in reality it will never be perfect it will either interfere or have clearance.

                             

                            You may be beating your head against the wall on something that should be of no concern, i would suggest getting with those who will be machining and welding and find out what they feel they need from you.