Part Modeling > Engineering Features > Hole > Sketched Holes > To Create a Sketched Hole
  
To Create a Sketched Hole
1. Select the approximate hole location on the model. This is your placement reference. The selection is highlighted.
 
* You cannot create 2-sided Sketched holes.
2. Click Model > Hole. The Hole tab opens and the preview geometry of the hole is displayed in the graphics window.
3. Click on the Hole tab. The Sketched hole options are shown.
4. To use a sketch that meets the requirements to define a hole, do one of the following:
To open an existing sketch:
1. Click .  The OPEN SECTION dialog box opens.
2. Select an existing sketch (.sec) file and click Open.
To sketch a new section:
1. Click . The Sketcher window opens.
2. Create a new sketched section (sketch profile) for the hole and click OK in the Sketcher window to close Sketcher.
5. To relocate the hole, drag the placement handle to the new location or snap it to a reference.
6. To change the hole placement type, on the Placement tab select a new type in the placement Type box.
7. 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 the corresponding references to the Offset References collector on the Placement tab.
 
* Offset placement reference handles are not available if you select Coaxial as the hole placement type.
8. 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.
9. 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.
10. To modify the sketched section, click on the Hole tab. The sketched section opens in Sketcher. The hole diameter and depth are driven by the sketch. The Shape tab only displays the sketched section.
11. 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.
12. Click on the Hole tab.