Specifying Depth for Extrusions and Holes
You can specify one of the following depths for an extruded feature of type protrusion or cut and a straight hole:
• Blind
• Up to a reference surface or through until
• Through all surfaces in the active part
Specifying Depth upto a Reference Surface
You can specify depth up to a surface on the part, by default. Depth for the extruded or hole feature is calculated "upto" or "Through Until" this surface on the part.
When you select an entity on the drawing, the part is searched for an existing surface up to which depth is calculated after confirming that the selected entity does not represent blind depth.
Specifying Blind Depth
You can specify a value as the blind depth for the extrusion or the hole. If you do not specify a value, the selected drawing entity represents the blind depth of the feature in the following instances:
• The selected entity is perpendicular to the entity that you select to define the sketch plane, and both entities exist on the same drawing view.
• The selected entity is not perpendicular or parallel to the entity that you select to define the sketch plane, and a surface does not exist on the part to represent depth up to this surface. The length of the entity is the extent of the blind depth.
• The selected entity is parallel to the entity that you select to define the sketch plane, and a surface does not exist on the part to represent depth up to this surface. The distance between the two parallel entities is the extent of the blind depth.
The direction for the feature is the default direction specified by Creo Parametric.
Specifying Depth through All Surfaces
When you create an extruded feature on the active part that already consists of solid features, you can specify a depth that extends through all the surfaces in the model to remove material and create a cut on the part.