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Saving New In-Context Components

You can specify the default behavior for saving new in-context components as:

  • External files (same as in SolidWorks 2007 and earlier)
  • Virtual components (same as in SolidWorks 2008 and 2009)

A new option in System Options - Assemblies sets the default behavior:

Save new components to external files
If selected, prompts you to name and save new in-context components to external files. If cleared, saves new in-context components in the assembly file as virtual components.

To save new in-context components in external files:

  1. Open install_dir/samples/whatsnew/assemblies/virtual/flanges.sldasm.
  2. Click Tools > Options and click Assemblies.
  3. Select Save new components to external files.
  4. Click OK.
  5. Click Insert > Component > New Part.

    The Save As dialog box appears so you can save the new part to an external file.

  6. In the dialog box, for File name, type gasket1 and click Save.

    Now you select a face on which to position the new part.

  7. Select the face of the three-bolt flange.



    The new part, gasket1, appears in the FeatureManager design tree. Editing focus changes to the new part and a sketch opens on the selected face.

  8. Use Convert Entities to create sketch entities that reference the edges of the flange, bolt holes, and center hole.



  9. Close the sketch.
  10. Extrude the sketch to a depth of 10 to create the part.
  11. Click in the Confirmation Corner to return editing focus to the assembly.

    After completing the above example, if you want to change the default behavior back to saving as virtual components, return to System Options - Assemblies and clear Save new components to external files.



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