Create positive holes when a target body does not exist

This example shows how to create positive holes before the target body has been created.

Procedure

1. Choose File tab → Open. Load a sketch section that you can revolve around a central axis.
2. Choose Home tab → Base group → Hole.
3. Create two separate hole features on opposite sides of the sketch using datum CSYS origins to position them. For each hole, use these parameters to make them positive holes:
   • Choose any hole Type except Hole Series.
   • In the Direction group set the Hole Direction option to Along Vector, and specify a direction for the hole.
   • In the Boolean group, from the Boolean list, select None.
4. Create a solid body that intersects the two positive holes. In this example a solid body is created by revolving the sketch section and adding blend and detail features to it.
5. Edit each positive hole using the Hole dialog box:
   • In the Boolean group, from the Boolean list, select Subtract.
   • With Select Body active, select the destination target body for the hole.
   • Click OK.
   • The volume of each positive hole is subtracted from the target body.

How do I

• Create a countersunk hole
• Create a screw clearance hole
• Create a hole on a nonplanar surface
• Create a Hole Series feature
• Customize standard data tables for hole features

Learn more

• Hole
• Hole Series
• Editing a Hole Series feature

Look up more details

• Hole dialog box
• Standard data tables for hole features
• Counterbored, countersunk, and tapered hole types
• Screw clearance hole types
• Threaded hole types
• Tapered Hole

Quick links

• Revolve and unite a section

Create positive holes when a target body does not exist, NX 2212 Series © 2023 Siemens