Extrude notes

Start and end limits when the extrude is the first feature in a part

When creating an Extrude feature in a part that contains no other entities, the only options that are available for the Start limit and the End limit are Value, Symmetric Value, and Value from Start Limit.

Defining the extrude section on a planar face outside of a sketch

If you select a planar face when defining the section curves for an extrude, and Selection Intent is set to Infer Curves, the Sketch automatically opens to let you sketch new curve sections on the selected planar face.

If you don't want the Sketch to open automatically, choose File tab → Utilities → Customer Defaults → Modeling → General. On the Miscellaneous page, clear the Automatically Sketch on Planar Faces check box.

Adding and removing objects from the section string

When you edit an extrude feature, you can add and remove objects from the section string.

• To add objects to the section of an extrude feature you are editing, click the objects to add.
• To remove objects from the section, hold Shift and click the objects to remove.

Note that the setting of the Type Filter on the Top Border bar and the current Selection Intent rule in effect when an extrude feature is first created are both still in effect when you edit the feature. For example, if you use the Feature Curves selection intent rule to select a sketch for an extrude section string, when you later edit the extrude feature you will find that you can deselect only the entire sketch, and not individual curves within it. To remedy this, first deselect the entire sketch, change the selection intent rule to Single Curve, and then reselect the individual sketch curves you want for the section string.

Deleting separate bodies in an extrude feature

To remove a body from a multiple-body extrude feature, deselect its section string or face during edit. Any other bodies in the extrude feature are unaffected.

Editing pre-NX 3 extruded body features

If you edit an extrude feature that was created in an earlier NX release, you may see the older legacy dialog boxes (Extruded Body) instead of the current Extrude dialog box.

Note that the current Extrude command creates features identified by the label EXTRUDE or Extrude, while the old Extruded Body command created features are identified by the label EXTRUDED or Extruded.

How do I

• Extrude a solid body
• Create an extrude feature with an offset
• Subtract an extrude feature
• Extrude between two bodies
• Extrude with an asymmetric angle
• Extrude using a section with self-intersecting curves

Learn more

• Extrude

Look up more details

• Extrude dialog box
• Extrude warnings
• Extrude handles

Extrude notes, NX 2212 Series © 2023 Siemens