To Create a Tapped Hole
Use this procedure to create a threaded 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. 
Straight and 
Tapped are selected by default.
Standard to create a standard hole. The standard hole options are shown. Straight and Tapped are selected by default.3. Select the approximate hole location on the model. The selection is highlighted. This is your placement reference.
 | You can also select the placement reference before you activate the hole tool. |
4. To change the hole placement type, select a new type from the placement Type box on the Placement tab.
5. 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. The system automatically snaps the handle to the reference and adds them to the Offset References collector on the Placement tab.
6. 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. Click 
to make the hole parallel to the orientation reference, or click 
to make the hole perpendicular to the orientation reference.
to make the hole parallel to the orientation reference, or click to make the hole perpendicular to the orientation reference.7. In the 
Thread type list, select the industry-standard hole chart (ISO, UNC, or UNF for cylindrical tapped holes).
Thread type list, select the industry-standard hole chart (ISO, UNC, or UNF for cylindrical tapped holes).8. In the 
Screw size box, type or select a screw size.
Screw size box, type or select a 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. |
9. To define the hole depth, select a depth option from the Depth list, or drag the depth handle in the graphics window.
| | • 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.• For holes created at the assembly level, when  Through All is selected for the hole depth,  Through Thread cannot be selected for the thread depth. |
10. To define the thread depth, click the Shape tab, and select one of the following options:
◦ Through Thread to thread the entire depth of the hole.
Through Thread to thread the entire depth of the hole.| | For holes created at the assembly level, when Through Thread is selected for the thread depth, Through All cannot be selected for the hole depth. |
◦ Blind, and then type a depth value.
Blind, and then type a depth value.◦ 
To Reference, and then select a surface, quilt, body, plane, edge, curve, axis, point, or vertex.
To Reference, and then select a surface, quilt, body, plane, edge, curve, axis, point, or vertex.11. To specify the drilled hole depth measurement method, select an option, and then type a value in the adjacent box:
◦ 
Shoulder—Measures depth to the end of the cylinder.
Shoulder—Measures depth to the end of the cylinder.◦ 
Tip—Measures depth to the tip of the hole.
Tip—Measures depth to the tip of the hole.12. 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.
diameter or countersink angle in the corresponding boxes.13. 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.
diameter or counterbore depth in the corresponding boxes.14. To represent the hole with lightweight geometry, click 
Lightweight.
Lightweight.15. To ensure that the entire top of the hole intersects the outside of the solid geometry, on the Shape tab, select the Top Clearance check box.
16. 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.
17. Click 
OK.
OK.