Assembly Design > Assembly Design > Managing Large Assemblies > Shrinkwrap Models > To Create a Faceted Solid Exported Shrinkwrap Model
To Create a Faceted Solid Exported Shrinkwrap Model
1. Retrieve a part or an assembly (or a simplified representation of an assembly) as the source model.
2. Click File > Save As > Save a Copy. The Save a Copy dialog box opens. In the Type list box, click Shrinkwrap.
3. Enter a name for the Shrinkwrap model in the New File Name box, or accept the default name and click OK. The Create Shrinkwrap dialog box opens.
4. In the Creation Method area of the dialog box, select Faceted Solid.
The Quality, Special Handling, and Include Datum References areas of the dialog box are set in the same way as when a surface subset Shrinkwrap model is created.
5. In the Faceted solid options area of the dialog box, you can select Invert triangle pairs.
6. In the Output format area of the dialog box, specify one of the following output file formats:
Part (selected by default)—Creates a part with normal geometry.
LW part—Creates a lightweight part with faceted geometry.
STL—Creates an STL file.
VRML—Creates a VRML file.
The system automatically appends the extension .stl to STL file names and the extension .wrl to VRML file names. Select or clear Use default template (selected by default for Part and LW Part file formats; not available for STL or VRML file formats).
7. Click OK. The system computes faceted solid geometry to create a solid Shrinkwrap model, and saves the new part. The subset consists of faceted solid geometry from the source model, along with mass properties and additional geometry according to your specifications. The Create Shrinkwrap dialog box remains open and the source model remains in session as the current object.
8. Click Cancel.