BE 1205 UNIGRAPHICS

Lesson 3

Lessons Learned

You have learned how to:

Create a new part file, open a part file, view the various part views, locating things off the Part Navigator and Assembly Navigator, and start modeling.

You have learned hot to create a:

Block, Cylinder, Pad, Pocket, Hole, Boss (cylinder), Edge Blend, Line, Work Layer, Extrusion, Instance, and Thread.

Today’s Objectives:

Learn how to:

Constraint and correctly build an assembly using different part files.

Make sure you have the base, cap and bushing NX files, which we created on lessons 1 and 2, on a single folder together with the assembly file we will be creating today. All the part files and assemblies must have your initials including your middle name/s.

GETTING STARTED – Building a Double Bearing Assembly

PART NAME: DoubleBearingAssembly

  1. Click on Start, Programs, NX 3.0 and then the NX 3.0 icon, or double click on the NX 3.0 icon located on your desktop.

  2. Go to File, click on New or click on the New Part icon located on the upper left corner of the screen.

  3. Change the units to inches. If you did your previous parts in millimeters, please change the units to millimeters to keep consistency. (Located on lower left corner).

  4. Click on the arrow next to the Look in, and make sure the file will be saved onto your memory disk.

  5. Type DoubleBearingAssembly_utepusername

  6. Under the Assemblies tab, go to component, and click on add existing.

  7. A select part window appears. Click on choose part file. Find where you saved all of your part files. Then click on the BASE part and press OK.

  8. A component preview and add existing part window appears. Focus on the add existing part window. Reference set should be MODEL, positioning should be ABSOLUTE, and layer options should be ORIGINAL. Click OK.

  9. A point constructor window appears. The x, y and z coordinates should be at least 0, 0 and 0. Press OK.

  10. A select part window appears. If the window does not reappear, repeat step 6. Click on choose part file. Choose the CAP part and press OK.

  11. A component preview and add existing part window appears. Focus on the add existing part window. Reference set should be MODEL, positioning should be MATE, and layer options should be ORIGINAL. Click OK.

  12. Under the mating type, select MATE. Go into the component preview window and click on the middle bottom surface of the CAP. Then click on the top middle surface of the BASE.

  13. Under the mating type, select align. Go into the component preview window and click on the side surface of the CAP. Then click on the side surface of the BASE. Then click on Apply.

  14. Under the mating type, select align. Click on the front surface of the CAP. Then click on the inner front surface of the BASE. Then click on Apply and press OK.

  15. A select part window appears. If the window does not reappear, repeat step 6. Click on choose part file. Choose the BUSHING part and press OK.

  16. A component preview and add existing part window appears. Focus on the add existing part window. Reference set should be MODEL, positioning should be MATE, and layer options should be ORIGINAL. Click OK.

  17. Under mating type, select MATE. Select the bottom circular surface of the larger cylinder off the bushing. Then select the side surface of the BASE.

  18. Under mating type, select CENTER. Select the curved surface of the BUSHING and then select the top curved surface of the BASE. Then Click Apply.

  19. Repeat Steps 15-18 for the other hole.

Comentários