6 Replies Latest reply on Jun 26, 2012 8:43 AM by Alina Mihai

    Trim a body with another body in assembly

    Alina Mihai

      Hi there,

       

      Please, please can anybody advice how will i be able to trim the tube from inside the sphear and fillet them together?

      I need to do it in that assembly because there are some other hidden parts which connect with those objects.

      I've been searching for something similar on the internet but couldn't find the answer

       

      Thank you, again.

        • Re: Trim a body with another body in assembly
          Deepak Gupta

          Edit the part you want to remove material from in context of the assembly (i.e. right click or click on the sphere and select edit component). And then go to Insert > Feature > Cavity option and select the tube as the tool for removing the material.

          • Re: Trim a body with another body in assembly
            John Burrill

            Alina, there are a number of ways that you can trim the tube to the sphere and I can think of two ways that you can do it at the assembly level.  The fillet is a problem because that can only be created at the part level (since it adds material to the model).  What I suggest, is editing the sphere in the context of the assembly and creating a 'join' feature with the tube part and then adding your fillets."  The tube part will still be in the assembly, but it will be hidden and it's goemetry will be merged with the sphere.  If the tube changes (or is moved), the joined geometry will udpate.  If the tube still has unconstrained degrees of freedom, that can make the part unpredictablein which case it might make more sense to insert the tube part directly into the spherical part (with the part open in its own window, select Insert==>Part from the menu and browse to the tube part).

            Now, to do the first part of what you asked about-trimming the tube to the sphere in the assembly, do the following

            open the assembly

            tube_trim1.png

            create a  sketch on a plane orthogonal to the tube

            select the silhouette edge of the sphere and do a 'convert entitites' to project it onto the sketch.  make the projected circle into a closed semi-circle profile using the line and trim tools.

            create an assembly revolve cut

            go to the 'Feature Scope' panel of the cut revolve propeperty manager and  deselect the 'autoselect' checkbox and populate the 'propogate feature to parts checkbox.  Pick the tube as the part affected by the assembly feature. 

            trim_inside_prp_mgr.PNG

            click OK

            tirmmed_outside.png

            If you're going to do the assembly this way, you'll need to create the fillets by creating revolved features or something similar

            fillet_revolves.PNG

            Will that work for you?

            • Re: Trim a body with another body in assembly
              Lenny Bucholz

              best way to do this would be to do a revolved boss, it will give you the whole thing in one sketch. your kind of making more work for yourself with the boolean type of operations.

               

              revolve.jpg

              • Re: Trim a body with another body in assembly
                Alina Mihai

                I managed! Thank you works works