Creo Tutorials > Creo Intelligent Fastener Tutorials > Advanced Tutorials > Assembling Fasteners > Exercise 1 – Assembling Fasteners with Orientation
Exercise 1 – Assembling Fasteners with Orientation
1. In Creo Parametric set the working directory to <downloaded files location>\IFXTraining\IFX_Asm\Exercise1 and open ifx-exercise-1.asm.
2. Click View > Saved Orientations and then click TAPER.
3. Click Datum Display Filters and select the Axis Display check box.
4. Click Tools > Screw > Assemble on reference. The Select References dialog box opens and the Position Reference box is activated.
5. Refer to the diagram below and select the references as described in the list below:
1. Select the hole axis as the Position Reference.
2. Select the top surface for the Screw head.
3. Select the lower surface of the ibeam for the Nut or Thread.
4. Click Saved Orientations and then click RIGHT. The green arrows are not aligned.
5. Click Saved Orientations and then click TAPER.
6. In the Select References dialog box, click the Orientation box to activate it and then select a surface at the top of the ibeam to define the fastener orientation. The green arrows are vertical.
6. Click OK. The Screw Fastener Definition dialog box opens.
7. Click Measure a diameter and select the axis hole.
8. Select the Side 2 Washers check box and select DIN 435 I.
9. Click OK to complete the definition of the fastener and close the dialog box. The Pattern Options dialog box opens.
10. Select Assemble fastener on all instances? and click OK. The TAPER orientation is automatically rotated by 180° on the right side.
* If you select Pattern fastener?, the TAPER orientation incorrectly orients as shown below:
11. Save and close the assembly.
12. Click File > Manage Session > Erase Not Displayed. The Erase Not Displayed dialog box opens.
13. Click OK to erase all files from memory.