Create hole at specified distance from two linear edges

Define a hole and place it relative to two linear edges.

1. On the ribbon, click 3D Model tab Modify panel Hole .
2. In the Holes dialog box, in Placement, click Linear. This option is automatically set if no visible sketch exists.
3. In the graphics window, specify the hole position:
   • To place the hole, select a face.
   • To dimension the placement of the hole, select two linear edges.
   • To correct the placement of the hole, edit the dimensions .
4. If there are two or more solid bodies in the part file, click the Solids selector to choose the participating solid bodies.
5. Select the hole type: Drilled, Counterbore, Spotface, or Countersink.
6. In Drill Point, select a type. If you choose Angle, enter the angle.
7. In Termination, select Distance, Through All, or To.

   For Distance or Through All, you can click Flip to reverse the direction of the hole. For a To termination, click a surface or an extended face on which to terminate the hole.

8. Choose the hole type:
   • Simple Requires no additional settings.
   • 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. For a partial depth, clear the check box for Full Depth, and set the depth on the hole preview image.
   • Taper Tapped Specify the thread type and size, and right-hand or left-hand direction. The program automatically determines the diameter, taper angle, and thread depth.
     Note: You cannot use Taper Tapped Hole with Counterbore.
9. In the hole preview image, set the values for the hole parameters. In the drop-down list, select a value, use the Measure command, Show Dimensions, or set Tolerances in the Tolerance dialog box.
10. Click OK. A hole generates with the specified parameters.

Show Me how to create a hole from linear references