Extruding a Surface

You can linearly project a sketch to add or remove material from the model.

  1. From the Surfaces section of the action bar, click Extrude Surface .

    Tip: In the top menu of the dialog box, you can switch between Extrude , Revolve , and Sweep features.

  2. Select the feature options in the Extrude dialog box.
    OptionDescription
    Add. Creates a feature by adding multiple profiles.
    Cut. Creates a feature by subtracting one profile from another.
    New. Creates a feature from another feature.
    Solid. Creates a solid feature.
    Thin. Creates a feature with a constant wall thickness. To set the wall thickness, drag the handle, or enter a value in the callout in the work area.

    You can set the wall thickness to be equal in both directions from the profile's midplane by clicking Thin Midplane.

    Surface. Creates a feature with a zero-thickness wall.
  3. Select the profiles to extrude.



    Direction 1 is available by default.
  4. Select the extrude type and end condition.

    Not all end conditions are available in every situation.

    • Blind. Extends the feature for the specified distance.

    • Midplane. Extends the feature for the specified distance from the sketch plane in both directions.

    • Through All Both. Extends the feature from the sketch plane through all existing geometry in both directions.

    • Through One Way. Extends the feature from the sketch plane through all existing geometry in one direction.

    • Up to Geometry. Extends the feature to the selected plane, feature, or sketch entity.

    • Up to Next. Extends the feature to the next body.

    • Up to Body. Extends the feature to the selected body.

  5. Set the extrude distance by dragging the handle or enter a Distance value.



  6. Optional: To reverse the extrude direction, click .
  7. Optional: To taper the face of the feature, click Draft and specify an angle. To reverse the draft direction, click .
  8. Optional: If Midplane was selected, enter a Thickness value for the thickness of the midplane. To reverse the midplane direction, click .
  9. Optional: To extrude a second direction, expand Direction 2 and select one of the following options from the menu.
    • Off. Turns off Direction 2.
    • Blind. Extends the feature for the specified distance.
    • Up to Geometry. Extends the feature to the selected plane, feature, or sketch entity.
    • Up to Next. Extends the feature to the next body.
    • Up to Body. Extends the feature to the selected body.
    1. If Up to Geometry or Up to Body is selected, select an entity or body to which the extrude extends.
    2. To taper the face of Direction 2, click Draft and specify an angle. To reverse the draft direction, click .
    3. If Offset is available, you can extrude the sketch profile an offset distance from the sketch plane's original position. To reverse the direction, click .
  10. To set additional options, expand Advanced and select one of the following Start Conditions from the menu.

    Applies an optional offset for the extrusion.

    • At Sketch. Extrudes the sketch profile from the sketch's plane.
    • End to End. Extrudes the sketch profile the length of the entire sketch.
    • From Offset. Extrudes the sketch profile an offset distance from the sketch plane's original position.
    • From Selected Geometry. Extrudes the sketch profile an offset distance from the selected geometry.
  11. Optional: Select a merge option:
    1. Click Auto Merge to merge the extrude feature with all other possible bodies.
    2. If Auto Merge is not selected, select the bodies to merge with the extrude feature.
  12. Click .