Create centerline loft

Create a loft with a centerline.

1. On the ribbon, click 3D Model tab Create panel Loft .
2. On the Curves tab, specify the sections to loft. In Sections, click, and then to blend the shapes, select the sections in sequence. If you select multiple sections on any plane, they must intersect.
   Note: If more than one loop is in a sketch, first select the sketch, and then select the curve or loop.
3. To select a centerline guide curve, right-click, and choose Centerline, or in the dialog box, click Centerline. Select a 2D or 3D curve to use as the centerline. The centerline holds the loft shape between sections normal to the centerline.
4. If the part contains more than one solid body, click the Solids selector and choose the participating body.
5. In Output, select solid or surface.
6. To join the beginning and ending sections of the loft, select Closed Loop.
7. To merge loft faces without a seam, select Merge Tangent Faces.
8. In Operation, click Join, Cut, Intersect or new solid .
   Note: The selected sketch or edge highlights in the graphics area.
9. On the Transition tab, Automatic Mapping is selected by default. If appropriate to modify automatically created point sets, or to add or delete points, clear the checkbox .
   • To modify, add, or delete, click the point set row.
   • A default map point calculates for each section sketch. To specify a unitless value (zero represents one end of the line; one represents the other end. Decimal values represent positions between ends), click position.
   Note: The selected point set or map point highlights in the graphics area.
10. To create the loft, click OK .

Show Me how to create a loft with a centerline