4 Replies Latest reply on Apr 3, 2015 3:43 PM by Pablo Jorge

    Origin problems after coping a file

    Pablo Jorge

      I have this piece, with the lateral ( red) and base plane (blue)... and the origin, no problem.

       

      However, when I edit the sketch, I see other origin, red, that avoid me to put relations.

       

      I have deleted all the relations and ad a new one, horizontal, but it is referred to the red origin not to the new one (blue)

       

       

      Of course I could draw it again, but I want to undestand what happens when I copy a file and give a new name.

        • Re: Origin problems after coping a file
          Jim Wilkinson

          Hi Pablo,

           

          Was the part that this part was copied form originally built in the context of an assembly? The origin of each sketch is derived from the face or plane that it was built off of, so my guess is this sketch was built off of the face or a plane of another part in an assembly, hence why the sketch origin does not align with the origin of the part itself. You can't easily make it align exactly with the part origin now after the fact and you are better off recreating the sketch.

           

          If this was not built in the context of the assembly, another way the sketch origin can become misaligned to the part origin is if you use either Tools, Sketch Tools, Modify or Tools, Sketch Tools, Align, Align Grid/Origin. Otherwise, I don't know how this could have been misaligned.

           

          I hope this helps,

          Jim

            • Re: Origin problems after coping a file
              Pablo Jorge

              Yes, is a part extracted from one assembly.

               

              My question is why it remember for ever its past?

               

              After broken all references and relations, HORIZONTAL should means HORIZONTAL.

               

              The question is how to do, when you copy a part from one assembly and you want to used in another different and not related assembly?

               

              Of course is easy to redraw a block, but imagine it was a complex piece.

                • Re: Origin problems after coping a file
                  Jim Wilkinson

                  Hi Pablo,

                   

                  As I noted, the sketch origin is derived from however it was originally created. It actually is very important for the sketch to remember its past, especially in complex models because if you have other downstream child features and you shift the sketch geometry of the first feature, all the other child features that are based off of the initial sketch would also shift. You could imagine that in a complex part that you may have some sketches defined based on the assembly faces, and others based on faces that relate to the part origin itself (off of the part reference planes). If you redefine the origin and orientation of sketches that are based off of the assembly faces, now they won't be properly positioned relative to the ones that were originally built relative to the sketch origin (since those would not shift while the ones made relative to the assembly would). You would very likely end up with very unexpected results and a lot of feature failures.

                   

                  I don't quite understand such a real world example where you would want to delete all of these types of relations, and then shift the sketch coordinate system and the geometry within the sketch, especially in a case where you have downstream child features (as you mention a complex model). But, it is technically possible by using the Tools, Sketch Tools, Align, Align Grid/Origin as mentioned earlier. However, to use this command you need vertices and edges to pick to do the alignment, so it can't be used in your attached example that has just one sketch.

                   

                  Thanks,

                  Jim