In this Article:

Extrude Shape

Insert > Shapes (Standard) (Part Level)

 Use this command to create an extruded shape feature.  Required inputs include the extrude method, the profile to extrude and the start/end locations.

Extrude Shape Examples

Extrude Shape - "Remove" Method

Extrude Faces

Required Inputs

• Profile
  Select a profile to extrude or middle-click to Create a Feature Sketch.  You can select face, wireframe geometry, face edges or a sketch.
  
  
• Select profile region
  Select the closed region in the sketch to extrude. Pick the selected region again will cancel it.
  
  
• Extrude type
  Specify the extrude type from the following.
  

  1 side
  The start position is decided by the selected Profile, and to specify the End position to determine the extrude length.
  
  2 sides
  Specify the Start and End positions to determine the extrude length.
  
  Symmetrical
  This type is similar to the "1 Side", but it will extrude the same length along the opposite direction decided by the End position.
  

• Start, End
  Specify the start and end of the extruded feature. You can enter the exact values, drag the preview echo on the screen or right-click for additional input options. When you right-click, the Boundary Face input option is available.  This will trim the start and/or end of the feature to the selected boundaries.  If you use the Base method above, the feature is trimmed while retaining a separate shape.

Options Tab

• Boolean shapes
  Specify the boolean operation and the boolean shapes. If the input is null, ZW3D will recalculate all the shapes in the graphic window. Excepting the Base option in the Required Inputs, this parameter is available for all other options.
  
  
  • Base
     Base features are used to define the initial basic shape of a part. The Base method is automatically selected if the active part has no shape geometry. If geometry exists, this method creates a separate base shape.
    
  • Add
     This method adds material to the boolean shapes.
    
    
  • Remove
     This method removes material from the boolean shapes.
    
    
  • Intersect
    This method returns the intersection of material with the boolean shapes.
    
    
  
  
• Draft angle
  Enter the draft angle if desired. Positive and negative values are acceptable.Typically, a positive value will make the feature bigger along the positive direction of the extrude.
  
  
• Blend
  Use this option to select the corner blend method. Refer to the figure below.

Variable
Corners are not modified. They maintain the same convexity/concavity (default)

Constant
Filleted/rounded corners will maintain the same radius.

Round
Convex corners are rounded. Concave corners are not rounded.

• Draft in extrude direction
  Check the box to apply draft in the extrude direction. Otherwise, draft will be applied in the direction normal to the profile or sketch plane.
  
  
• Direction
  Specify the direction to extrude. This option will override the default extrude direction that is normal to the sketch plane.
  
  
• Profile cap
  For Base, use this option to specify a "cap" for the extruded shape which is intersected with others and profile is closed. For Add, use this option to specify a "cap" if profile is closed, or specify the boundary if profile is open.
  

• Offset, Outer offset, Inner offset
  Specify an offset method and distance(s) to be applied to curves, curve lists, or open or closed sketched profiles.  This option adds thickness to the feature automatically.
  

None
Do not create offset.

Shrink/Expand
Create an offset by shrinking or expanding the profile. A negative (-) value offsets (=shrinks) the profile to the inner side and a positive (+) value offsets (=expands) to the outer side of the profile.The inner side, by convention, is defined as the concave side of an open sketch or the inside of a closed profile.

Thicken
Create a thickness from the profile determined by two distance values. The first offsets the profile toward the outer side. The second offsets the profile toward the inner side. A negative value (-) for 1st and 2nd offset means flipping the offset direction.

Thicken Same
Create a symmetrical thickness about the profile.  The total thickness equals 2 times the distance.

Connected perimeter faces are created by this option. The ends of the faces will remain open unless the End caps option is used (see below). If both end caps are specified, a solid is created.

 

• Keep profile
  Check this box to Keep profile selected during the Required Inputs (see above) used to Extrude. Otherwise it will be deleted.
   
• Flip face direction
  Check this box to reverse the all faces directions. Please note that only when the extruded shape is open, this option is available.
   
• Use these options to control the placement of end cap faces on the start and end of shapes.

Advanced Tab

• Twist point
  Use this option to rotate (twist) the feature as it is extruded. Select a point to twist about. The Twist angle below is also required for this option.
  
  
• Twist angle
  If the Twist point option is used, enter the twist angle. This is the total angle that the extruded feature will twist from its start to end.
  • The limit is 90 degrees because the resultant surface is basically a ruled surface. If you need more,
    • Use Sweep (ZW3D Designer and higher)
    • Use a Helix and Bi-rail Loft (Innovator Plus)

Notes

1. More about Adding Shapes with Open and Closed Profiles (see CAD Tips & Techniques).
   
   
2. During Profile input, you can right-click and select Insert Curve List from the Input Options Menu. This will allow you to make a parametric list of existing curves to use as input for this command.
   
   
3. If the RMB (Right Mouse Button) Input Option "Boundary Face" is used to specify the "Start" or the "End" distance, the extruded feature is trimmed using the specified face and the side the extrusion "start" is on is kept rather than the face normal side. This only applies to single boundary face cases.