4 Replies Latest reply on Dec 10, 2008 3:00 PM by John Lhuillier

    Tool Designers-transparent parts on drawings

    Mike Agan
      A co-worker found how to phantom the part while held in a fixture on a drawing.<br />This is the work around: On the drawings convert entities of the part edges, change to construction lines and hide the part in the assembly model<br /><br /><edit> (should appear under drawings heading)<br /><br />
        • Tool Designers-transparent parts on drawings
          Charles Culp
          You shouldn't need a work-around for this.

          In the drawing view, right click on the part. One of the options will be "Component Line Font..." Select that.

          un-check "use document defaults", and for "Visible Edges" select a line style of Phantom (or whatever you choose). After clicking OK the component should have edges that are phantom.
          • Tool Designers-transparent parts on drawings
            Charles Culp
            In that case, let me give you another option for a work-around. The benefit of this method is that it will be fully parametric. With "convert entities" changes to the model may not be reflected with changes in the drawing.

            Set all drawing views to "Shaded With Edges".

            Go to the model, set it to "Shaded With Edges". Right click on all "fixture" components, go to "Component Display", and chose "Hidden Lines Removed".
            Right click on all "part" components, go to "Component Display", and chose "Wireframe".

            Then,
            In the drawing view, right click on the part. One of the options will be "Component Line Font..." Select that.

            un-check "use document defaults", and for "Visible Edges" select a line style of Phantom (or whatever you choose). After clicking OK the component should have edges that are phantom.
            • Tool Designers-transparent parts on drawings
              John Lhuillier
              If you have a drawing that is a view of an assembly, the use ALT-POS-VIEW for showing the fixtured part in phantom. In your assembly create a configuration that would have just the parts you are fixturing visible and all others hidden and NOT SUPPRESSED. Then create your drawing view, then add this ALT-POS-VIEW and no workaround needed.

              You can also change the components you show in the alt pos view to their own layer if needed as well. To do this expand the alt pos view in the feature tree so you can see the featured parts. Then pick them in the tree and RMB on one of those you've picked. Then choose component line font from the pop up menu and choose the line features you want to change. Just use caution to check the tickbox for from selection or it will change everything to the line feature you've just chosen.

              You can also do this with Display states but you still need to have at least 2 configurations in order to create the ALT POS VIEW. Then you can change the ALT POS VIEW configuration back to the one that has your display state and then change the display state in the second step. I've added this as an enhancement request to allow ALT POS VIEWs to be created from just the display state so hopefully this process isn't as slow to do.