Extrude PropertyManager

To open this PropertyManager:

  1. Create a sketch.
  2. Click one of the extrude tools:
    Extruded Boss/Base on the Features toolbar, or click Insert > Boss/Base > Extrude
    Extruded Cut on the Features toolbar, or click Insert > Cut > Extrude
    Extruded Surface on the Surfaces toolbar, or click Insert > Surface > Extrude

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 nonplanar. Planar entities do not need to be parallel to the sketch plane. The sketch must be fully contained within the boundaries of the nonplanar surface or face. The sketch follows the shape of the nonplanar entity at the starting surface or face.
Extrude feature  
Nonplanar starting surface
Sketch entity

You can create boss, cut, and surface extrudes from any size surface, face, or plane. The surface or face must be planar.
   
Vertex Starts the extrude from the vertex you select for Vertex .
Offset Starts the extrude on a plane that is offset from the current sketch plane. Set the offset distance in Enter Offset Value.

Direction 1

Some fields that accept numeric input allow you to create an equation by entering = (equal sign) and selecting global variables, functions, and file properties from a list. See Direct Input of Equations in PropertyManagers.
  Direction 1 Determines how the feature extends. Set the end condition type. If required, 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.

Through All - Both

Extends the feature from the sketch plane through all existing geometry for Direction 1 and Direction 2.

Up to Next

Extends the feature from the sketch plane to the next surface that intercepts the entire profile.

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 required, select Reverse offset to offset in the opposite direction. Example: Translate Surface

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. Example: Specifying the Direction of Extrusion
  Flip side to cut (Extruded cuts and revolved cuts only). Removes all material from the outside of the profile. By default, material is removed from the inside of the profile.
Default cut Flip side cut
  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.

The Link to thickness option in the Extrude PropertyManager lets you link the dimension of the present extrusion to the dimension of the existing extrusion to which it is coincident. If the depth of the original extrusion changes, the new extrusion changes to match it.

This is available only when sheet metal features are present in the FeatureManager design tree. The Link to thickness option is useful in sheet metal parts because the part must be of uniform thickness.

Draft On/Off Adds draft to the extruded feature. Set the Draft Angle. Select Draft outward if required.
No draft
10° draft angle inward 10° draft angle outward

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. Example: Extruding Thin Features
Thin Feature is required when using an open contour sketch. Thin Feature is optional when using a closed contour sketch.
  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 the 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 option is available only for the first extruded body in a model.

Selected Contours

Selected Contours Allows you to use a partial sketch to create extrude features from open or closed contours. Select sketch contours and model edges in the graphics area.

Example: Using Selected Contours in a Cut Extrude

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.