Extrude and Revolve Feature Data

This function can be used to define the perpendicular dimension (extrusion), angle (revolve), direction and conical angle of a feature. The same dialog box is used in the definition of the data for both extrusion and revolve features.

Dialog Box Options

Dimension: Defines the length, angle, draft angle or offset value.
Formula: Defines the variable for length, angle, draft angle or offset.
Length or Angle: Defines the length of the extrusion. Define the angle of rotation. You can also enter the value as a numerical calculation, such as 360/8. The same calculations are available as in the Formula field. You can also leave the length and angle empty and select To Selected Face or To Selected Point.
In Both Directions: Defines extrusion/revolution of the sketch from the origin of the sketch in both directions with the amount equaling half of the value in the Dimension/Angle field. The length of the extrusion will be the value of the Dimension/Angle field in total.; Note: You can change the direction of the extrusion by clicking the In Both Directions icon.
Thru All: Defines extrusion through the entire volume when extruded cutout is selected. The extrusion direction is highlighted in the volume.
To Next Face: Defines extruded cutout up to the next face of the part.
To Selected Face: Defines extrusion/revolve to a face clicked from the model. If In Both Directions is selected, select a surface for both directions. You can select more than one face from both sides of the sketch plane. The only limitation is that the faces must be connected to each other. The selected faces are displayed in the dialog box, where you can change or delete the faces. Select a face from the list, and select the context-sensitive Change or Delete.
To Selected Point: Defines extrusion/revolve in the direction of the sketch plane normal to a point selected from the model. If In Both Directions is selected, the extrusion is performed also in the opposite direction of the sketch's plane normal. You can select a single point from both sides of the sketch. You cannot select both points from the same side of the sketch. The selected point or points are displayed in the dialog box, where you can change or delete them. Select a face from the list, and select the context-sensitive Change or Delete.
Draft Angle: Defines a conical extrusion. Enter a conical angle as the draft angle value. A positive value will make the part wider in the direction of extrusion. A negative value will make the part narrower.
Make New Part: You can use a cutout feature to divide a part.
Make Tool: Defines the extrusion as a machining feature that can be used to machine sheet metal or parts in an assembly.
Offset: Defines either an offset or a difference for the extrusion.; If Length or Angle is selected, you can enter an offset into the Offset 1 field. For an extrusion, offset is the distance from the sketch plane, and for a revolution, it is the angle from the sketch plane around the rotation axis. An offset can not be defined, if In Both Directions is selected.; If To Selected Face is selected, you can define a difference between the selected face and the extrusion. A positive offset value takes effect in the direction of the selected face's normal. A negative offset value affects in the direction opposite to the selected face's normal. If In Both Directions is selected, you can specify individual offset values for the selected faces into the fields Offset 1 and Offset 2.
Selected Elements: You can later add, change or delete element selections in the fields Selected Elements 1 and Selected Elements 2 (if In Both Directions is selected). For example, select Face in the list and select the context-sensitive function Change.