Extended modules > Creo Elements/Direct Part Library > Screw connections > Add a screw connection
  
Add a screw connection
Before you add screw connections, you should put the intended parts in the same assembly. If the parts belong to other assemblies, you can put these assemblies into a parent assembly.
If you include parts that are outside an assembly, no features are created and you can't modify the connections from Creo Elements/Direct Part Library. The same is true if you choose not to create features.
You can choose from three commands to add a screw connection:
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.
To add a screw and drilled holes to your part,
1. Click Part Library and then, in the Screw conn group, click the arrow next to New.
2. Select from the following commands in the Connection And Drill section (see descriptions above):
Click Point/Direction, then set the Center point and the drill Direction in the viewport.
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. Select the parts that should be drilled and connected by the screw in the Scan parts section:
To Face: Select a face, and the screws and 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.
4. You can set the owner of the screw parts in the Load new parts to section of the dialog. The screws must belong to the same assembly or sub-assembly as the drilled features.
5. Set the owner of the drilled hole features in the Create features section of the dialog. By default, the features are created in the assembly that holds the first face you selected in the operation. If you don't have an assembly, no features will be created.
To change the owner assembly, click Owner and select an assembly in the Structure Browser.
To change the owner pattern, click Pattern and select a pattern.
6. You can choose a different screw in the Select screw section of the dialog, or you can accept the default, which is the last screw you loaded from Creo Elements/Direct Part Library.
7. To change the screw, hole, or hardware, click Parameter at the bottom of the dialog.
8. To create a pattern of screws, 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.
9. Click OK to complete the operation.
Limitations
If you choose not to create features, you will not be able to modify the screw holes using Creo Elements/Direct Part Library commands.