Creating a Hole

You can create a hole.

1. Click Hole in the Cutting/Stamping toolbar (Holes sub-toolbar) and click the surface where you want to place the hole.

   A grid is displayed to help you position the hole.
   
   

   The Hole Definition dialog box is displayed, providing default values.

   
   
   

2. In the Extension tab, choose a bottom limit for the hole.

   Blind
   
   
   Up to Next
   
   
   Up to Last
   
   
   Up to Plane
   
   
   Up to Surface
   
   

3. Use the up and down arrows to specify the values as needed. In our example, we kept the Blind option with a diameter of 12mm and a depth of 8mm.

4. Keep the direction Normal to surface to create the hole normal to the sketch face.

   If you want to create a hole not normal to the sketch face, click to clear Normal to surface and select a line, an edge or a plane in the contextual menu of the field. Refer to Part Design User's Guide : Sketch-Based Features : Holes : Creating Holes for more information.

5. Choose a bottom type for the hole.

   
   

   • Flat;

   • V-Bottom;

   • Trimmed (available when selecting Up to Next, Up to Last, Up to Plane or Up to Surface).

   In our example, we selected a V-Bottom of 120 degrees.

   
   
   

6. In the Type tab, select the type of hole you wish to create.

   Simple
   
   
   Tapered
   
   
   Countersunk
   
   
   Counterdrilled
   
   
   Counterbored
   
   

7. Use the up and down arrows to specify the values as needed. In our example we chose a Counterbored hole of 15mm diameter and 5mm depth.

8. In the Thread Definition tab, select Threaded check box to create a threaded hole.

9. Use the up and down arrows to specify the values as needed.

10. Click OK to create the hole.

    
    
    
    
    

    Important: If you want to create a hole on an overlapping element or a bend with radius=0, either choose the top skin of the element, or unfold the shape to create the hole. You can create: A hole on a hole A hole on a half-height hole A hole on a pocket

You can create a hole with no deformation.

Before you begin: Create a wall or a web with a cylindrical bend or a flange.

1. Click Hole .

2. Select the surface where you want to place the hole. In our example we select a cylindrical bend.

   Important: The hole point positioning must be located on a sheet and must be associative with the selected surface. The hole direction must be normal to selected surface. The hole should not cut separately more than one face.

3. Select the Deformation tab in the Hole Definition dialog box.

   
   
   

4. You can choose either or not to select the No Deformation check box:

   Deformation
   
   No Deformation
   
   

   By default, No Deformation option is not selected.

Warning: When the No Deformation option is not selected: The hole can be created only on a planar or cylindrical, and single support surface. You cannot create a hole on a surfacic flange or a double cuvature hopper. If you try to, a warning is displayed and the Circular Cutout Definition dialog box opens so that you can create the hole on a bend or a flange. You cannot create a feature built by thickening on a hole.

You can change the position of a hole on a surface.

If you need to change the position of the hole on the surface:

1. Click Positioning Sketch . The Sketcher workbench opens and a point representing the hole's position is displayed on the surface.

   
   
   

2. Move the hole on the surface according to your needs.

   
   
   

3. Exit the Sketcher workbench. The hole is positioned according to your settings.

   
   
   

You can constrain the hole's location when creating it.

1. Select two edges on the wall and click Hole .

2. Click the surface where you want to place the hole.

   Constraints defining the distances between the hole's center and the edges are displayed.
   
   

3. Click OK to create the Hole.

   
   
   Refer to Part Design User's Guide : Sketch-Based Features : Holes : Locating Holes for more information.