Create a part or a virtual part in an assembly

1. On the ribbon, click Assemble tab Component panel Create .
2. To create a virtual component: Select the Virtual option. Some dialog box options are disabled. You enter the component name and default BOM structure only. Select the BOM Structure for the virtual component from the Default BOM Structure list.
   Note: A virtual component is a component that requires no modeling of geometry and no file.

   To create a component:

3. In the dialog box, enter information about the file and its location:
   • Under New File Name, enter a name. If you do not enter one, a default name is created.
   • Specify the template to use for the new part.
   • Under New File Location, browse to a folder whose path is specified in the assembly project.

     If you specify a folder not included in the project, Autodesk Inventor sometimes does not find the file the next time you open the assembly.

   • Select the default BOM structure.
     Note: You can override the structure to be Reference at the component instance level.
   • Select the check box to place a mate constraint between the sketch plane and the selected face or plane in the assembly. Clear the check box if you do not want to create the automatic constraint.
4. Specify how to position the new sketch plane of the part. Choose one:
   • Select a component face or work plane on which to sketch.
   • Click in empty space to create the part with the same orientation and origin as the target assembly.
   • Click the origin point of the target assembly or any occurrence of a component. This action orients the new part to the rotation and translation of the selection.

   If appropriate, use Project Geometry to project geometry from the part to the new part sketch.

1. To reorient the view of the sketch, click View tab Navigate panel View Face .
2. Use the commands on the Sketch tab to create a sketch on a selected face or plane.
3. Select Extrude, Revolve, Loft, or Sweep to create a feature using the new sketch.
4. Continue to select faces on which to sketch and add new features as needed.

When the part is complete, click Return or double-click the top-level assembly in the browser to reactivate the assembly environment.

Note: If you project geometry from an assembly part, you can make the new part associative. Select Tools tab Options panel Application Options Assembly tab, and then select the check box called Enable Associative Edge/Loop Geometry Projection During In-Place Modeling. Sketches that include projected geometry are shown in the browser as Reference symbols nested under a Sketch symbol.

Note on templates

When you create a part-in-place, you can browse to the template you want to use. If you enter a file name with a different extension than the template, the file name is displayed in red.

When you click Browse to New File Location:

• If the template changes (enter a file name with extension, select a template from list, or browse to a template location), the current template selection filters the file dialog box.

  If you enter a name with an extension different from the template, the template extension is appended to the name and displayed in file name control.

• If the template is the default, both the part and assembly filter the dialog box. When you enter a name with a valid extension, the template updates.