6 Replies Latest reply on Aug 5, 2010 1:26 PM by Scott McFadden

    Rhino to SolidWorks

    Dan Tegman
    Dan Tegman Aug 4, 2010 12:19 PM

      I have a latch assy. that was sent to me from a customer that was created in Rhino and he brought it into SW and it was sent to me. Now I need to separate the parts, which I have done. Now each part is STOCK part with no features. Is there away to have it behave like a SW part with features? I tried the feature recognition but it fails.

       

      thank you...

       

      Dan

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        • Re: Rhino to SolidWorks
          Jeff Mowry
          Jeff Mowry Aug 4, 2010 12:29 PM (in response to Dan Tegman)

          I haven't looked at the details of the parts you've got yet, but if Feature Recognition didn't work, you probably have more complex geometry in your parts.  If so, and if you need features, you'll likely have to rebuild each part in SolidWorks.

          • Re: Rhino to SolidWorks
            Scott McFadden
            Scott McFadden Aug 4, 2010 12:35 PM (in response to Dan Tegman)

            Dan,

            I agree that if feature works didn't work then your parts are more then just

            straight forward machine features.

            What I would suggest and I am only saying this because I am going to do this

            with my project is create a Solidworks drawing of each component with nothing

            but the greometry.  No centerlines, hidden lines or hatching.

            Insert this drawing onto a parts plane and use contour select to recreate your features.

              • Re: Rhino to SolidWorks
                Dan Tegman
                Dan Tegman Aug 5, 2010 12:18 PM (in response to Scott McFadden)

                Hi Scott,

                 

                So I create a drawing, do I need to put dims on it?

                I don't understand what you mean by " Insert drawing onto a parts plane and use contour select" ? Can you explain?

                 

                Dan

                  • Re: Rhino to SolidWorks
                    Scott McFadden
                    Scott McFadden Aug 5, 2010 1:26 PM (in response to Dan Tegman)

                    Dan,

                    I have been doing this all morning so it is very fresh in my mind.

                    Here it goes...

                    1.) Save the drawing as a DXF file or DWG file.

                     

                    2.) Start a new part so you have nothing more then axis and planes.

                     

                    3.) Select the plane you want the DWG or DXF on.

                     

                    4.) Then go to Insert>DXF/DWG

                    DWG.jpg

                    5.) Browse to where your file is

                     

                    6.)  "Next through this dialog DWG.jpg

                          unless you need to change something.

                     

                    7.)  Select "Yes" here  DWG.jpg

                     

                     

                    Then you will have your drawing on your plane with skect entities.  What I did from here was delete everything except the part I am trying to create.

                     

                    Good luck.  It is a little time consuming, but it is working for me.  I have created 2 parts already using this method starting from just a 2D drawing.

                • Re: Rhino to SolidWorks
                  Jerry Steiger
                  Jerry Steiger Aug 5, 2010 1:12 PM (in response to Dan Tegman)

                  Dan,

                   

                  You bought in the assembly as a part, so you have a multi-body part with eight bodies. FeatureWorks gives you an error message that the part contains overlapping solids. Otherwise, it looks like FeatureWorks should be able to do a good job on the parts as they are pretty basic. I would try reimporting the assembly as an assembly. You could also save each of the bodies as a part. Then try FeatureWorks on each part.

                   

                  Jerry Steiger

                   

                  Well, I just tried saving the latch body out as a separate part and FeatureWorks still fails. I was able to make it work by saving the body as a Parasolid file, importing the Parasolid file and running FeatureWorks on the new part. I suggest that you save all of the bodies out as Parasolid files and import them again. I'm not sure why this is necessary, but it probably has to do with the fact that the original saved body still has features for all of the other bodies, even though the bodies aren't there.

                   

                  Message was edited by: Jerry Steiger