Extrude : Options and Results

Access: Open this function from one of the following locations:

Click the button in the toolbar.
Select Solid > Main Tools > Extrude from the menu bar.
Select Extrude on the popup menu if a sketch or 2D composite curve is selected.
Select Die Design > Insert Tools > Extrude from the menu bar.
Select Mold Design > Insert > Extrude from the menu bar.
Select Insert > Extrude button in the Mold Design Guide Toolbar or Parting Guide Toolbar.

Extrude a contour to add or remove material.

Create a new solid object, add to an existing solid object or remove material from a solid object by extruding a 2D sketch, composite curve, 3D face or face with tolerant edges in a given direction.

The following main options are available:

	New	Create a new solid object by extruding the selected entities. New extrusions are considered independent objects.
	Add	Add to an existing solid object by extruding the selected entities. Added extrusions are added to the active object.
	Remove	Remove material from a solid object by extruding the selected entities. Material is removed only from the active object.

Important: Objects created by New will be considered independent objects. Those created by Add will be added to the active object. For Remove operations, material will be removed only from the current active object.

Notes:

If only one object exists in the file it is automatically active, unless manually deactivated or if the active object is deleted. See Activate / Deactivate and Activating Objects.
For Add and Remove operations you can use wires or faces from a non-activated component (external reference).

Required Step 1

Pick a single entity to be extruded (pick a closed 2D composite curve, sketch or a face). Multiple faces from the same object can be picked.

Notes:

If you enter Extrude immediately after creating a closed 2D composite curve or sketch, the entity is automatically included in Step 1.
If you select a sketch that contains more than one closed curve sequence, all closed curve sequences will be extruded. In order for a sketch to be selected, however, it must contain only closed curve sequences.

The following parameters are displayed:

Add/New Extrude example:	Remove Extrude example:

Single

Pick a single entity to be extruded (a closed 2D composite curve, sketch or a face).

When the entity is selected, the system automatically jumps to the next step of the function.

Multi Faces

Pick multiple faces to be extruded. The faces must be from the same object.

When all the faces are selected, press <exit><exit>(middle mouse button) to jump to the next step of the function.

Required Step 2

Set the extrusion parameters and the direction. The default direction is normal to the 2D contour or sketch plane. You can flip the direction by clicking the displayed arrow head or body, or you can click on the arrow origin to set another direction.

The following parameters are displayed, depending on the selected main option:

New Extrude:	Add Extrude:	Remove Extrude:

Parameters:

New

This is a dropdown list of the following main options:

New	Create a new solid object by extruding the selected entities. New extrusions are considered independent objects.
Add	Add to an existing solid object by extruding the selected entities. Added extrusions are added to the active object.
Remove	Remove material from a solid object by extruding the selected entities. Material is removed only from the active object.

The default displayed option is determined as follows:

New, if there is no object.

Add, if there is an object and the last used option was New or Add.

Remove, if there is an object and the last used option was Remove.

Delta/Reference

This is a dropdown list of the following extrude options:

Delta/Reference	Extrude the selected geometry on one or both sides, either by Delta (by a given value and direction) or by Reference (to a reference face, plane or point). For additional information, see: Add/New - Delta/Reference Remove - Delta/Reference
Delta Mid Plane	Extrude by the same amount equally in both directions. For additional information, see: Add/New - Delta Mid Plane Remove - Delta Mid Plane
To Closest	Extrude to the closest faces of an active object, according to a defined direction. This option is displayed for the Add and Remove main options only. For additional information, see: Add - To Closest Remove - To Closest
Through	Extrude through a solid object material. This option is displayed for the Remove main option only. For additional information, see: Remove - Through

One Side

This is a toggle option One Side / Both Sides enabling you to extrude to one of both sides of the entity selected in the first step.

One Side

Extrude on one side of the contour.
Example:Example:

Both Sides

Extrude on both sides of the contour.
Example:Example:

In the Delta/Reference option, additional parameters are displayed. These parameter settings for each extrude side are displayed under their respective Primary Side and Secondary Side headings (for more information on these headings, see Additional Delta/Reference Notes and the labeling rules). This option is useful in Die tools, where, in many cases, it is necessary to create the punch (for example, to a reference) and also to define a delta to the other side.

By Delta

This is a toggle option By Delta / By Reference. This option is displayed if the Delta/Reference option is selected above.
For additional information, see:
Add/New - Delta/Reference
Remove - Delta/Reference

Invert Active Object

Use the Invert Active Object option as required. This parameter appears in the Add and Remove main options and is available only for open objects and deals with issues of object direction.

Inside

This is a toggle option Inside / Outside that enables you to select which side of the selected geometry to remove. This option is displayed for the Remove main option only.
Example:Example:

The following geometry is selected for this example:

Inside

Remove the "inside" of the selected geometry. This is the default option.
Example:Example:

Option Selection:	Result:

Outside

Remove the "outside" of the selected geometry.
Example:Example:

Option Selection:	Result:

Note: When using the Outside option, if the active object is an open object, a message is displayed prompting you to use the options Inside or Invert Active Object (see above) and to try again.

Thin Wall - Off

This toggle option enables you to create a thin-walled solid.
ExampleExample

Sketch	Extrude: Thin Wall Off	Extrude: Thin Wall On

The Thin Wall toggle option appears in the following functions:

Drive

Extrude

Revolve

For additional information, see Thin Wall.

Examples of Extrude on a FaceExamples of Extrude on a Face

Extrusion on a Rounded Edge

Extrusion on a 3D Face

Optional Step 1

Add a draft angle to the extrusion; see Defining a Draft Angle.

Optional Step 2

Change the active object. This option is only available in the following cases:

for Add and Remove operations when creating a feature. The option is not available when editing a created feature.
if there is more than 1 object in the active part.

A toggle parameter is displayed; Keep Original Active Object / Activate Selected Object.

Keep Original Active Object	Keep the active object originally used in the function. This is the default option.
Activate Selected Object	Change the active object to the selected object. Pick an object as required.

Press <exit><exit>(middle mouse button) when finished. Or, if this is the final result, click OK or Apply in the Feature Guide to complete the function.

When completed, the Extrude feature will appear in the Feature Tree as follows:

Extrude > New:	Extrude > Add:	Extrude > Remove:

Some functionality may be dependent on the product package. Contact your Reseller if you require a license.