Creo Elements/Direct Part Library can create drilled holes through one or more parts, with or without sinks on either side of the hole.
You can save your drilled holes in groups called hole patterns. These groups are stored in the assembly as a feature with child objects. If you create a pattern group, you can move the entire group or change the pattern values, such as the distance between holes in the pattern.
However, if you change one hole in the pattern, the others will not change. For example, if you have a pattern group containing six plain drilled holes, and change one so it has an upper sink, only the hole you change will be affected.
You can choose from three commands to add a drilled hole:
• Point/Direction: Define the position by selecting a point and direction.
• 2 Points: Define the position by selecting two points.
• Normal: Define the position by selecting a point on a face, and the screw and hole direction are automatically set to the normal of the face.
If you create a hole through more than one part, you should create a hole feature at the assembly level. This allows you to modify the hole for all affected parts.
To add a drilled hole to your part or assembly,
1. Click Part Library and then, in the Drill group, click the arrow next to Create.
2. Select from the following commands in the Create section (see descriptions above):
◦ Click Point/Direction, then set the Center point and the drill Direction in the viewport. Press the Tab key to reverse the arrow when you set the direction.
◦ Click 2 Points, then set the entrance (Point 1) and exit (Point 2) in the viewport.
◦ Click Normal, then set the Center point in the viewport.
3. To drill a hole through only one part, select ThroughPart and check the Part field to verify that the correct part is selected.
4. To drill a hole through more than one part, deselect ThroughPart and select an option in the Scan parts section:
◦ To Face: Select a face, and the drilled holes will extend from the face you selected in the previous step to the face you select in this step, and they will pass through all faces in between. Only available if you use the Two Pts or Normal command.
◦ Face is separation face: This option is available if a tapped blind hole is defined for the drill. The part in which the blind hole ends is defined by the separation face and the direction of the drill.
◦ All parts: All parts in the path of the hole are drilled.
◦ Viewport: Only the parts visible in the selected viewport are drilled.
◦ Parts: Use the Select tool to create a list of parts to drill.
5. To create a pattern group, select an assembly as the Owner in the Create pattern features section.
6. To add this hole to an existing pattern group, select a pattern group in the Structure Browser for Hole Pattern in the Create pattern features section.
7. To create a pattern of holes, select Linear, Linear Grid, or Radial in the Copies field, then set the following options:
◦ Direction (linear): Select a direction in the viewport.
◦ Distance (linear): Type the distance between parts.
◦ Axis (radial): Select the axis for the pattern in the viewport.
◦ Angle (radial): Type the angle between parts.
◦ Number (both types): Type the number of parts you want in your pattern.
Create.
Point/Direction, then set the Center point and the drill Direction in the viewport. Press the Tab key to reverse the arrow when you set the direction.
2 Points, then set the entrance (Point 1) and exit (Point 2) in the viewport.
to complete the operation.