AutobuildZ > Creating Features in the Current Part > To Create a Feature of Type Extrude
  
To Create a Feature of Type Extrude
1. Click Feature > Protrusion on the AutobuildZ tab. The Extrude Feature wizard opens.
2. Specify a name for the extruded feature and specify whether you want to create an extruded feature of type Protrusion or Cut on screen Step 1 Of 4 on the Extrude Feature wizard.
3. Click to switch between Side1 and Side2 to indicate the direction of the cut if you are creating an extruded feature of type cut.
4. Select entities to define the section profile on screen Step 2 Of 4 of the Extrude Feature wizard. The section profile is automatically validated.
5. Select a line entity to define the sketching plane on screen Step 3 Of 4 of the Extrude Feature wizard.
6. Click Flip if you want to change the sketch view direction.
7. On screen Step 4 Of 4 of the Extrude Feature wizard, under Depth Reference, click to select a draft entity as reference to define the extent of depth for the extruded feature.
The box next to displays the ID and drawing view of the selected entity.
If a surface or datum plane exists in the part, by default, Through Until is selected, and this surface is used as a reference.
Click if you want to clear the selection and select the entity again.
8. Under Depth Options, select one of the following options to specify the depth of the extruded feature:
Blind—Specifies the required depth for the extruded feature. Type a value in the box. A default depth value is calculated automatically based on the reference entity selected and displayed.
 
* is not available. You cannot select an entity.
Through Until—Specifies an existing surface on the part that is used as the "upto" reference. This is the default.
Through All—Specifies that the depth of the extruded feature extends through all the surfaces in the model. You can use this option only for an extrude feature of type cut.
9. Click to flip the direction of depth of the extruded feature.
10. Click Preview to preview the following feature elements in a Creo Parametric window during the relevant step of the extrude feature creation process:
The reference surface or datum plane that represents the sketching plane
The reference surface or datum plane that represents the "Through Until" depth
The section profile on the sketching plane
The 3D extrude feature when all feature elements are defined
11. Click OK.