Part Modeling > Engineering Features > Hole > Simple Holes > To Create a Linear Hole by Referencing an Axis
To Create a Linear Hole by Referencing an Axis
1. Click Model > Hole. The Hole tab opens with the default hole type set to Simple hole and the default placement Type set to Linear.
2. Select a surface on the model where you want to place the hole. The selection is highlighted. This is your placement reference. The preview geometry of the hole is displayed in the graphics window.
* You can also select the placement reference surface before you activate the hole tool.
3. Click the Placement tab and click the Offset References collector to activate it. Alternatively, right-click the graphics window and choose Offset References Collector on the shortcut menu.
4. Select a datum axis or an axis of an existing hole from the model. Alternatively, drag the handle of the secondary placement reference to an axis.
The secondary placement reference axis should be normal to the primary placement reference.
If you select the axis of a linear hole or a datum axis created with two offset references as the secondary reference, then the system assigns the first reference used to create the linear hole or datum axis as the default dimension orientation reference and fully constrains the hole.
If you select a datum axis other than the one created with two offset references or an axis of a hole other than a linear hole as the secondary reference, then you must specify a dimension orientation reference.
5. To align the hole to the secondary placement reference, click the Placement tab and select the secondary reference in the Offset References collector. Click Offset and change it to Align.
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. Select either Parallel or Perpendicular from the list.
7. To change the system-assigned default dimension orientation reference, click the Placement tab and activate the Dimension orientation reference collector by clicking it.
8. Select a straight curve, straight edge, datum axis, datum plane, or a planar surface as the dimension orientation reference.
9. Select the required depth option from the depth options list.
10. 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.
11. Click .