4 Replies Latest reply on Dec 8, 2018 11:04 AM by David Matula

    Is it possible to copy/trace an elipsed edge of a part and make it a sketch in another

    Angie Dirks

      I have a circular part that had to be cut at an angle. I need to make a mating part to the edge which is now an ellipse. Can I trace or copy the edge of the ellipse to place as a sketch on the mating piece that needs to be cut out?

        • Re: Is it possible to copy/trace an elipsed edge of a part and make it a sketch in another
          Dan Golthing

          yes.  position the two parts in an assembly where you want them.  edit the part "in context" that is in the assembly.  go into the sketch command and convert entities. 

           

          If I'm understanding your question correctly.

           

          This then has a relationship from one part to the other, which is called "in context"  In Context relations can cause problems down the road if you aren't careful.

          • Re: Is it possible to copy/trace an elipsed edge of a part and make it a sketch in another
            Solid Air

            To answer your question how asked.

             

            First create a sketch on face of the angled surface,

             

             

            Next select the outside edge

             

             

            Then covert entities

             

             

            Exit the sketch, then highlight it in the feature manager tree and from the edit menu select copy.

             

             

            Then in your mating piece, select the surface you want to cut the ellipse on.

             

             

            And now from the edit menu select paste

             

             

            And you ellipse has been copied.

             

             

            Of course you will need to edit the sketch to fully define it and place it where it should be on the part.

             

            However, what happens if the angle changes?

             

            Instead of copying the sketch, I would create a construction sketch on you mating part that mimics the first part

             

             

            I would then use that sketch to create a second sketch of the ellipse making the major diameter coincident to the end points of the angled line and dimensioning the minor diameter.

             

             

            If you plan to make an assembly using both parts then Dan Golthing's suggestion will get you a parametric link which will automatically change if the angle changes.

             

            There are other ways (ex. weldment) to do this also.

            • Re: Is it possible to copy/trace an elipsed edge of a part and make it a sketch in another
              David Matula

              simple answers is yes it is possible.  now see ya later.

              what you have to do is do some assembly part editing, use the convert edges tool in the sketch and create some incontext features by doing so.

              This is so much fun especially when you open an assembly created 5 versions ago and some of the assembly features are all showing errors cause these kind of features have lost planes, or some other kind of reference.  90% of the time it is an easy fix till you come across a model that was not done with any kind of standards, or rational thought and then you end up spending about an hour to a week trying to figure out how to fix all the problems.  Some times it is just easier to blow it all away and make it right.