Creating a Hole  

This task shows you how to create a hole, that consists in removing material from a body.

Open the NEWHole1.CATPart document.

1. Click Hole .

   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. Should you need to change the position of the hole on the surface, click Positioning Sketch .

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

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

6. Exit the Sketcher workbench.

   The hole is positioned according to your settings.

7. 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 the Hole description in Part Design User's Guide for more information.

8. 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.

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

   Simple	Tapered
   Countersunk	Counterdrilled
   Counterbored

10. 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.

11. In the Thread Definition tab, click Threaded if you wish to create a threaded hole.

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

    	You cannot differentiate a threaded and a non-threaded hole on the wall.
    In the example below, the hole on the right is threaded when the hole on the left is not.
    	A threaded hole is visible only: in the specification tree; In the example below, Hole.1 is threaded when Hole.2 is not. in the preview;     Threaded hole Non-threaded hole on a drawing. In the example below, the hole on the right is threaded when the hole on the left is not.
    	To display threaded holes on a drawing, make sure Generate Threads is selected in the Drafting settings. To do so, go to Tools->Options, Mechanical Design, Drafting, View tab.
    	Refer to Creating Threaded Holes in Part Design User's Guide for more information.

13. Click OK to create the hole.

	You can constrain the hole's location when creating it.
	Select two edges on the wall and click Hole . Click the surface where you want to place the hole. Constraints defining the distances between the hole's center and the edges are displayed. Click OK to create the Hole.
	Refer to Locating Holes in Part Design User's Guide for more information.
	You can create a cylindrical hole in creation and dual view by checking No Deformation option in Deformation tab. The hole point positioning must be: located on sheet associative with selected surface Moreover the hole direction must be normal to selected surface. Hole should not cut separately more than one face.
	The hole can be created only on a planar and single support surface (i.e. a wall or the planar face of a flange). It can also be created on a cylindrical bend. May 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 part to create the hole. You cannot create a hole on a bend or a surface flange. 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. a feature built by thickening on a hole. You can create a hole on a hole; a hole on a half-height hole; a hole on a pocket.