Creating a Protected Feature

The Protected Feature command creates areas within the same body, and additional material cannot penetrate the protected areas. This is useful if you need to reserve space to add another features or for areas that must be kept open.

  1. Click Protected Feature in the Basic Features toolbar.

    Protected features can have different shapes. To know how to create any of them, refer to the Prism, Sweep, Revolve, Thick Surface or External Shape tasks in the Functional Modeling Part User's Guide. The Protected Feature dialog box that appears displays the Prism as the default shape to be created.



  2. Select the profile you want to extrude.



    Tip: If no profile is defined, clicking Sketcher enables you to sketch the profile you need.

  3. In the Limits tab, enter 20mm to define First length.

    Important: Refer to Prism or Sweep if you want to make the shape more complex, by setting parameters and options.

  4. Select the Thick check box that is available for the Prism, Sweep and Revolve shapes. This option enables you to add material to both sides of the profile.

    Following additional options display:



  5. Enter 5mm in the Inside Thickness field and click Preview.

    Thickness is added to the inside of the profile.

  6. Enter 2mm in the Outside Thickness field and click Preview.

    Thickness is added to the outside of the profile.

  7. In the Reference list, select Neutral Fiberto add material equally to both sides of the profile.

  8. Click Preview to see the result.

    The thickness you defined for Inside Thickness is evenly distributed: a thickness of 5mm has been added to each side of the profile.



  9. Click OK to confirm and create the protected feature.

    As a protected area, the protected feature is displayed in red. Protected Prism.X is added to the specification tree in the Solid Functional Set.X node.