Creating Loft and Loft Cut

You can create lofts by making transitions between profiles. A loft can be a base, boss, cut, or surface. You create a loft using two or more profiles. Only the first, last, or first and last profiles can be points. All sketch entities, including guide curves and profiles, can be contained in a single 3D sketch.

  1. From the section of the action bar, click Loft .
  2. Select the Sections faces, sketch regions, or sketch contours for the loft profile.
  3. Select the Guides .

    Each guide must intersect with all profiles. If three or more guides are defined, the intersection points between nonplanar profile and all guides must be coplanar.

  4. Select the Closing Points to specify a closing point on the closed sections whose closing point is not good enough to create a quality loft.
  5. Specify surface options.
    OptionDescription
    Solid. Creates a solid feature.
    Thin. Creates a feature with a constant wall thickness. To specify the wall thickness, drag the handle, or enter a value in the dialog box.

    When Thin is selected, you can define the wall thickness equally in both directions from the profile by clicking Midplane .



    		 Surface. Creates a feature with a wall thickness defined as zero.
  6. Specify merge options:
    OptionDescription
    Add Creates a feature that adds material.
    Cut Creates a feature that removes material.
    New Do not merge bodies.
  7. Specify segment options.
    OptionDescription
    Ratio. Profiles are mapped by curvilinear ratio.
    Tangency. Profiles are mapped by sharp points.
    Curvature. Profiles are mapped by curvature discontinuity.
    Vertices. Profiles are mapped by segments.
  8. Optional: Click Tangent Propagation to include all edges and faces tangent to your selection.
  9. Optional: Click Automerge to automatically find bodies to merge with the lofted body.
  10. Click .

 

See Also
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