Whenever possible, you should create the screw and drill the hole using the Creo Elements/Direct Part Library commands. However, you may need to add a screw to an assembly that already has holes for the screw. Only the screw and hardware (nuts, washers, etc.) are added. You must have an existing hole in your part.
You cannot modify this type of screw connection using Creo Elements/Direct Part Library commands.
To add only a screw to your part,
1. Click Part Library and then, in the Screw conn group, click the arrow next to New.
2. Click ConnPoints. The Create Screw Only dialog box opens.
3. Select the center of the Upper connection point and Lower connection point. If your screw has a conical head, use Cone for the upper connection.
It is easier to select the center of a hole if you set the catch tool to Center. Click View > Catch to open the Catch toolbar.
4. Select the assembly Owner for the screw.
5. Select the length for the screw:
◦ Automatic: This setting should be used with a connection that includes a nut. The length will be calculated for you.
◦ Automatic + short, Automatic + normal, or Automatic + long: Use these settings when the hole is threaded and no nut is required. The appropriate length is automatically determined, then the next longer or shorter length for the standard is used.
◦ Part: You select the screw from the library and choose its length.
6. If you select a pattern type in the Copies field, you will need to set one or more of the following values:
◦ Direction (linear): Select a direction in the viewport.
◦ Offset (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.
New.
ConnPoints. The Create Screw Only dialog box opens.
to complete the operation.