Extrude PropertyManager

Set the PropertyManager options based on the type of extrude feature.

From

Sets the starting condition for the extrude feature.

• Sketch Plane. Starts the extrude from the plane on which the sketch is located.

• Surface/Face/Plane. Starts the extrude from one of these entities. Select a valid entity for Surface/Face/Plane . The entity can be planar or non-planar. Planar entities do not have to be parallel to the sketch plane. The sketch must be fully contained within the boundaries of the non-planar surface or face. The sketch follows the shape of the non-planar entity at the starting surface or face.

• Vertex. Starts the extrude from the vertex you select for Vertex .

• Offset. Starts the extrude on an plane that is offset from the current sketch plane. Set the offset distance in Enter Offset Value.

Direction 1

• End Condition. Determines how the feature extends. Set the end condition type . If necessary, click Reverse Direction to extend the feature in the opposite direction from that shown in the preview.

• • Blind. Set the Depth .

  • Through All. Extends the feature from the sketch plane through all existing geometry.

  • Up to Vertex. Select a vertex in the graphics area for Vertex .

  • Up to Surface. Select a face or plane to extend to in the graphics area for Face/Plane . Double-click a surface to change the End Condition to Up to Surface, with the selected surface as the termination surface. If the sketch that you extrude extends outside of the selected face or surface body, Up To Surface can do some automatic extension of one analytic face to terminate the extrusion.

  • Offset From Surface. Select a face or plane in the graphics area for Face/Plane , and enter the Offset Distance . Select Translate surface to make the end of the extrusion a translation of the reference surface, rather than a true offset. If necessary, select Reverse offset to offset in the opposite direction.

  • Up To Body. Select the body to extrude to in the graphics area for Solid/Surface Body . You can use Up To Body when making extrusions in an assembly to extend the sketch up to the selected body. Up To Body is also useful with mold parts, if the body you extrude to has an uneven surface.

  • Mid Plane. Set the Depth .

• Direction of Extrusion . Select a direction vector in the graphics area to extrude the sketch in a direction other than normal to sketch profile.

• Flip side to cut (Extruded cuts only). Removes all material from the outside of the profile. By default, material is removed from the inside of the profile.

• Normal cut (Sheet metal cut extrudes only). Ensures that the cut is created normal to the sheet metal thickness for folded sheet metal parts.

• Merge result (Boss/Base extrudes only). Merges resultant body into an existing body if possible. If not selected, the feature creates a distinct solid body.

• Link to Thickness (Sheet metal parts only). Automatically links the depth of an extruded boss to the thickness of the base feature.

• Draft On/Off . Adds draft to the extruded feature. Set the Draft Angle. Select Draft outward if necessary.

Direction 2

Set these options to extrude in both directions from the sketch plane. The options are the same as Direction 1.

Thin Feature

Use the Thin Feature options to control the extrude thickness (not the Depth ). A Thin Feature base can be used as a basis for a sheet metal part.

• Type. Sets the type of thin feature extrude.

• • One-Direction. Sets the extrude Thickness in one direction (outward) from the sketch.

  • Mid-Plane. Sets the extrude Thickness equally in both directions from the sketch.

  • Two-Direction. Allows you to set different extrude thicknesses for Direction 1 Thickness and Direction 2 Thickness .

• Auto-fillet corners (Open sketches only). Creates a round at each edge where lines meet at an angle.

• Fillet Radius (Available if Auto-fillet corners is selected). Sets the inside radius of the round.

• Cap ends. Covers (caps) the end of the thin feature extrude, creating a hollow part. You must also specify the Cap Thickness . This options is available only for the first extruded body in a model.

• • Cap Thickness . Sets the thickness of the thin feature cap, from the end of the extrude towards the sketch plane.

Selected Contours

• Selected Contours . Allows you to use a partial sketch to create extrude features. Select sketch contours and model edges in the graphics area.
  
  of cut extrude using selected contours

Feature Scope

Specifies which bodies or components you want the feature to affect.

• For multibody parts, available if you select Geometry pattern under Options. See Feature Scope in Multibody Parts.

• For assemblies, see Feature Scope in Assemblies.