Extrude Shape - "Add" Method

 

 

Extrude Shape - "Remove" Method

 

 
Extrude Faces

 

 

 

The Add, Remove and Intersect options are similar to the Combine Shapes command.

 

	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 active part.
	Remove - This method removes material from the active part.
	Intersect - This method returns the intersection of material with the active part.

 

• Profile - Select a profile to extrude or middle-click to Create a Feature Sketch.
  
  You can select wireframe geometry, face edges or a sketch.
   

• 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 Faceinput 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.

 

 

 

Draft angle

Enter the draft angle if desired. Positive and negative values are acceptable.

 

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

This option is only active if the profile is open (i.e., it does not form a closed loop)  You can use this option to specify a "cap" for the profile. This face will serve to close the open profile.

 

 

 

 

Offset, 1st offset, 2nd 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

 

• Shrink/Expand - Create an offset by shrinking or expanding the profile.  A negative (-) value expands to the outer side and a positive (+) value shrinks to the inner side of the profile.

 

• Thicken - Create a thickness from the profile determined by two distance values.  The first shrinks the profile toward the inner side. The second expands the profile toward the outer side.

 

• 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.

 

 

 

Use these options to control the placement of end cap faces on the start and end of shapes. This can automatically form closed volumes when a closed profile is used or when an open profile with the Boundary option is used. Select the icon to apply.

 

 

 

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.

 

 

 

• More about Adding Shapes with Open and Closed Profiles (see CAD Tips & Techniques).

• During Profile input, you can right-click and select Make 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.

• 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.