Create hole using sketch point or hole center

In a sketch, create a hole center with the Point command, or use a selected endpoint or center point on sketch geometry.

You can create identical holes in one feature using multiple sketch points.

  1. On the ribbon, click 3D Model tab Modify panel Hole .
  2. In Placement, select From Sketch. This option sets automatically if a sketch is visible.
  3. Center points are automatically selected. Holes are previewed when centers are selected. Press CTRL or SHIFT to omit center points from the selection set.

    If preferred, click endpoints of lines, rectangles, or arcs or center points of arcs or circles to specify hole centers.

    Drag with the left mouse button, and sketch points within the selected area can serve as centers of holes.

  4. If there are two or more solid bodies in the part file, click the Solids selector to choose the participating solid bodies.
  5. Specify the hole type: Drilled, Counterbore, Spotface, or Countersink.
  6. In Drill Point, select a type of drill point. If you choose the Angle drill point, set the angle.
  7. In Termination, select Distance, Through All, or To.

    For Distance or Through All, click Flip to reverse the direction of the hole, if needed. For a To termination, click a surface or an extended face to terminate the hole.

  8. Choose the hole type:
    • Simple No additional settings are needed.
    • Clearance Specify the fastener to fit to the hole. Select the standard, fastener type, fastener size, and fastener fit.
    • Tapped Set thread type, size, designation, and class, and select the right-hand or left-hand direction. If partial depth is needed, clear the Full Depth check box and set the depth on the hole preview image.
    • Taper Tapped Specify the thread type and size and right-hand or left-hand direction, and Autodesk Inventor automatically determines the diameter, taper angle, and thread depth.
      Note: You cannot use a Taper Tapped Hole with Counterbore.
  9. Set the values for the hole parameters in the hole preview image. Click the arrow to select a value, use the Measure command, Show Dimensions, or set Tolerances in the Tolerance dialog box.
  10. Optionally, select the Infer iMate check box to place an iMate automatically on a hole.
  11. Click OK to create the hole with the specified parameters.
    12. Note: To use a single sketch to position dissimilar holes, you can use a single sketch to lay out the position of multiple holes. Then share the sketch among several hole features. Sketches cannot be shared when creating the hole as an assembly feature.
Parent topic: Hole features