Creating a Hole

You can create a hole of a specific type and a size through a single or multiple bodies.

Before you begin: Create a sketch geometry and apply features to it.
  1. From the Features section of the action bar, click Hole .

    If your geometry does not have a sketch entity to use as the hole origin, you need to add a sketch object on the geometry.

    1. From the Sketch section of the action bar, click Point .
    2. In the work area, click on the geometry to place the point where you want the hole.

      You can use other sketch commands to create sketch entities on the geometry, for example, sketch a rectangle to use the four corner entities as the location for the holes.

  2. In the Hole dialog box, click the Placement tab.
  3. Select a sketch entity from the work area to specify the location for the hole.

    You can select multiple sketch entities if all the holes have the same design requirements. If you have a sketch object selected with multiple entities, all the possible hole positions are selected by default.

  4. Optional: Click Ignore construction geometry to exclude any construction geometry from your selections.
  5. Optional: To skip some of the selected sketch entities in a sketch object, click Skip instance.
    A marker is displayed on all the sketch entities in the selected sketch object. Click the marker to prevent that entity from creating a hole.

  6. Click the Design tab.
  7. Select the Hole Type from the menu.
    OptionDescription
    Straight. Creates a simple hole.
    Straight Tapped. Creates a hole with a straight thread.
    Counterbore. Creates a counterbore hole.
    Countersink. Creates a countersink hole with head clearance.
    Taper Tap. Creates a countersink hole with head clearance.
  8. From the Standard list, select the engineering and manufacturing standard for dimensioning holes.
    OptionDescription
    ASME Inch General-purpose standard for dimensional inch series engineering and manufacturing.
    ASME MetricMetric standards for worldwide engineering and manufacturing.
    DIN German Institute for Standardization (Deutsches Institut für Normung) for engineering and manufacturing.
    ISO The International Organization for Standardization meets the requirements, specifications, guidelines, or characteristics that ensure that materials are consistent in the products.
  9. From the Hardware Type list, select a type of drill or dowel.
  10. From the Size list, select a size for a hole.
    The sizes vary depending on the Standard selection.
  11. From the Fit list, select the tightness of hole to fit the hardware.
    • Close
    • Normal
    • Loose
    This option is available only for Straight, Counterbore, and, Countersink hole types.
  12. Under Hole Dimensions, specify the dimensions such as Diameter, Depth, Distance, and Bottom treatment for a hole.

    Note: Click to reset the dimensions to the default values.

    The Dimension Edit Box is displayed. Type the value for the dimension and press Enter.

    The Hole dimension options vary depending on the selection of hole type.
  13. Specify Near Side Options and Far Side Options.
  14. Click .