To Create a Standard Hole
1. Click > 
Hole. The Hole tab opens.
Hole. The Hole tab opens.2. Click 
Standard to create a standard hole. The standard hole options are shown.
Standard to create a standard hole. The standard hole options are shown.3. Select the approximate hole location on the model. This is your primary placement reference. The selection is highlighted, and preview geometry of the hole is displayed.
4. To relocate the hole, drag the primary placement handle to the new location or snap it to a reference.
5. To change the hole placement type select a new type from the placement Type box on the Placement tab.
6. Drag the offset placement reference handles to the appropriate references to constrain the hole. As you drag each handle, the available references are highlighted as your pointer moves over them. This enables you to target the correct reference. The system automatically snaps the handle to the reference and adds them to the Offset References collector on the Placement tab.
7. To align the hole with an offset reference, select the reference from the Offset References collector on the Placement tab and change Offset to Align.
 | You can change the reference type only for holes that use the Linear placement type. |
8. To orient the hole to be parallel to or perpendicular to a reference:
a. Click the Placement tab, click the Hole orientation collector, and select a planar, axial, or linear reference.
b. Select either Parallel or Perpendicular from the list.
9. To create a tapped hole, select 
Add Tapping.
Add Tapping.10. To create a tapered hole, select 
Tapered.
Tapered.| | Tapped and tapered holes are available only if Add Tapping is selected. |
11. To create a drilled hole, click Add Tapping to deselect it, and click 
Drilled.
Add Tapping to deselect it, and click Drilled.12. To create a clearance hole, click Add Tapping to deselect it, and then click 
Clearance.
Add Tapping to deselect it, and then click Clearance.13. Select the desired hole chart in the box adjacent to 
Thread type on the Hole tab. Thread type enables you to select industry-standard hole charts (ISO, ISO_7/1, NPT, NPTF, UNC, or UNF).
Thread type on the Hole tab. Thread type enables you to select industry-standard hole charts (ISO, ISO_7/1, NPT, NPTF, UNC, or UNF).14. Type or select a screw size in the box adjacent to 
Screw size.
Screw size.| | If you enter a screw size that is not listed, the system selects the closest screw size. You can also drag the hole diameter handle to select a screw size. |
15. To define the hole depth, select a depth option from the Depth Options list, or drag the depth handle in the graphics window. The following depth options are available:
| | To define a new depth by dragging the depth handle, or by typing or selecting a new value, you must select the Blind depth option. |
◦ 
Blind—Drills the hole from the placement reference to a specified depth. This is the default option.
Blind—Drills the hole from the placement reference to a specified depth. This is the default option.◦ 
To Next—Drills the hole up to the next surface of a solid. This option is not available in Assembly.
To Next—Drills the hole up to the next surface of a solid. This option is not available in Assembly.◦ 
Through All—Drills the hole to intersect with all surfaces.
Through All—Drills the hole to intersect with all surfaces.◦ 
Through Until—Drills the hole to intersect with the selected surface. The Depth Reference collectors activate on the Hole tab and on the Shape tab. This depth option is not available in Assembly.
Through Until—Drills the hole to intersect with the selected surface. The Depth Reference collectors activate on the Hole tab and on the Shape tab. This depth option is not available in Assembly.◦ 
To Selected—Drills the hole to the selected point, curve, plane, surface, quilt, or body. The Depth Reference collectors activate on the Hole tab and on the Shape tab.
To Selected—Drills the hole to the selected point, curve, plane, surface, quilt, or body. The Depth Reference collectors activate on the Hole tab and on the Shape tab.16. To add countersink to the hole:
a. Click 
Countersink on the Hole tab.
Countersink on the Hole tab.b. To define the countersink diameter or angle, click the Shape tab and type or select a new countersink diameter or countersink angle in the corresponding boxes.
17. To add counterbore to the hole:
a. Click 
Counterbore on the Hole tab.
Counterbore on the Hole tab.b. To define the counterbore diameter or depth, click the Shape tab and type or select a new counterbore diameter or counterbore depth in the corresponding boxes.
18. To ensure that the entire top of the hole intersects the outside of the solid geometry, on the Shape tab, make sure that the Top Clearance check box is selected.
19. To select the bodies from which geometry is removed, click the Body Options tab and select an option:
◦ To cut geometry from all the bodies that the feature passes through, select All.
◦ To cut geometry from selected bodies:
1. Select Selected.
2. Click the body collector, and then select bodies from which to cut geometry.
20. Click 
OK.
OK.