Extrude feature or body

To begin, sketch or select a profile or region that represents the cross section of the extruded feature or body to create.

1. On the ribbon, click Model tab Create panel Extrude .
2. If there is only one profile in the sketch, it is selected automatically. If there are multiple profiles, click Profile, and then select the profile to extrude. Use Select Other to cycle through selectable geometry, and then click to select.

   If you select an open profile, select Match Shape, and then select the side to keep. Match Shape describes solutions that are defined through the extension of the open ends of the profile, and by the shape of the body. It is available only for open profiles in Parts.

   Note: For part features, you can use a shared sketch as a profile. In the browser, click the plus sign beside the feature that contains the sketch you want to use. Then right-click the sketch icon, and click Share Sketch. A sketch that you use in more than one feature is automatically shared.
3. If there are multiple bodies in the part file, click the Solids selector to choose the participating body.
4. In Output, click Solid or Surface. For base features , only Surface is available for open profiles. For assembly extrusions, only Solid is available.
5. In Operation, click Join , Cut , or Intersect with another feature. To create a solid body, click New solid . For assembly extrusions, only the Cut operation is available.
6. In the Extents drop-down list, select a method to terminate the extrusion. For base features, some methods are not available.
   • Direction (one direction), or Symmetric (extrude in two directions with half the total value) Enter the distance of the extrusion.
   • Asymmetric (extrude in two directions with different values) Enter a value for the positive distance. Enter a second value for the negative distance.
   • To Next Click the direction of the extrusion. Not available for assembly extrusions.
   • To Click a sketch point, work point, model vertex, work plane, or the End termination surface.
   • Between method Click the start and end termination surfaces.
     Note: For To and Between extents, if termination options are ambiguous, such as on a cylinder or irregular surface, click the More tab. Click Flip to specify direction. By default, the extrusion terminates on the maximum-distance surface. To terminate on the nearest-distance surface, click Minimum Solution.
   • All Click the direction of the extrusion, or to extrude equally in both directions.
7. On the More tab, enter a Taper angle, if necessary. In the graphics window, an arrow shows the taper direction. To apply a Taper angle to both directions, use the Distance-Distance option.

   Results preview on the model.

8. If appropriate, to place an iMate automatically on a closed loop (such as extruded cylinders, revolves, and holes), select Infer iMate.
9. Click OK.

Show Me How to Create an Extrusion