Creating a Hole

This task shows you how to create a hole by removing material from a body.

Open the NEWHole1.CATPart document.

  1. Click Hole in the Aerospace Sheet Metal toolbar (Holes sub-toolbar).

    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 want 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.
 

  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 Locating Holes in Part Design User's Guide for more information.

You can create a cylindrical hole in folded and unfolded view by selecting the No Deformation option in the Deformation tab.

  • The hole point positioning must be:

    • located on the sheet
    • associative with selected surface

    Moreover the hole direction must be normal to selected surface.

  • The hole should not be cut separately in more than one face.

  • By default, No Deformation option is not selected.
  • 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.