17 Replies Latest reply on Sep 22, 2016 7:49 AM by Kai Arne AA

    Using seleced body in drawing views

    Kai Arne AA

      I have a multiple sheet drawing of a weldment part.

      The main bulk of drawing views only contains selected bodies from a configuration.

       

      My question is if the drawing / drawing view communicates with the whole model configuration or only the bodies selected?

      The drawing file is just as big as the weldment part file (60MB) and i was hopeing making it lighter by making simplified configurations to select prefered bodies from.

      If that would help?

       

      If all my drawing views in 10+ sheets communicates with the main confiugration i can understand the drawing is running slow.

       

      I tried adding display states but it didn`t make mutch difference.

        • Re: Using seleced body in drawing views
          Glenn Schroeder

          To clarify, are you creating configurations or display states of the model just for showing selected bodies?  If so, there's your problem.  Use this button instead when inserting a drawing view (or you can use it on existing views).

           

           

          If you need configurations of your model for some other reason then we can try to address that.

          • Re: Using seleced body in drawing views
            Marshall Wilson

            I often split a multibody part into several Configurations (using the Keep/Delete body feature). This allows me to assign separate part numbers & part data to each body using custom properties. I have noticed though that it seems that file size - for a part at least - grows rather quickly once I start adding lots of new configurations. Haven't noticed how this affects Drawing file size though.

             

            Marshall

            • Re: Using seleced body in drawing views
              Paul Risley

              2 cents worth on multibody parts, configurations and multiple sheets on big weldments or structures equals huge load time/ file size on your drawings. Select the bodies you need as Glenn showed earlier. The more data stored in the weldment the harder the file gets to be to work with. Lets say you have 10 sheets to your drawing 5 configurtaions & 5 display states. Every time you open your drawing your weldment will have to re-build it's cut list 5 times and every sheet will have to update the 25 possible data paths it could be using per sheet. So imagine if you apply that across the board, I am good at math but this is huge re-build time for a drawing.

              1 or 2 configurations as needed, keep your display states to a minimum, if you need specific views set up construction planes as reference when inserting views. If you need specific parts only select insert/drawing view/ relative to model.By using this you can select the front and right planes to orientate your drawing.

                • Re: Using seleced body in drawing views
                  Kai Arne AA

                  Since i have lot of threaded patterns, drawing size reduced with 10MB afther changing from high quality to draft.

                  The model is quite optimized with only flat pattern as second configuration and one display state.

                   

                   

                  I have selected bodies through: model view - select part / configuration - select bodies.

                  I think it ends up simular to inserting view relative to model?

                    • Re: Using seleced body in drawing views
                      Glenn Schroeder

                      Kai Arne AA wrote:

                       

                      I have selected bodies through: model view - select part / configuration - select bodies.

                      I think it ends up simular to inserting view relative to model?

                      I know you asked Paul and not me, but I much prefer using the "Select Bodies" button I showed in my screenshot above over Relative View, for at least two reasons.

                       

                      1.  The bodies selected in the view are editable using the button.  Not with Relative View.

                      2.  Doesn't create a second drawing view, leaving the original, like Relative View does.

                        • Re: Using seleced body in drawing views
                          Paul Risley

                          Relative view was more for a specific plane of reference view if you are just using a traditional view it is not very useful for that. We have mitered and coped tubes creating complex angles out and sometimes we have to create planes to get a relative view. That is why I suggested that above the configuration option.

                           

                          Glenn you are correct whenever possible your option is the best and easiest to manage for drawings.

                      • Re: Using seleced body in drawing views
                        Kai Arne AA

                        Thanks for answers.

                         

                        It seems the model gets almost impossible to work with if i do alot of work on the drawing.

                        If i don`t involve the drawing and leave it checked in on server for some time, the model gets more cooperative.

                         

                        I am hoping using freeze bar will help when adding the part to assembly but i am not sure it works when using folders?

                        Hopefully issues in this older post are fixed?

                         

                        https://forum.solidworks.com/thread/87658?q=freeze bar