Creating scalable associative geometry/features in NX

cmalco

5 Jan, 2018 04:43 PM

Pinion Gear using Through Curves with associative, scaled geometry (NX9)

1. Step 1:

   

   
   

   Before we get started; looking at this design as with any design, we want to parameterize elements that could change at a later date. This is beyond the scope of a simple model making exercise and more in step with actual real-world, dynamic, product design environments. For the sake of this tutorial, we are going to parameterize the helix angle but this could be the pinion shaft diameter, spline count, and/or any number of elements. This is where design 'future proofing' and paramaterization really come into play.

2. Step 2:

   Create an expression, name it angle_sections with a value of 15, units = degrees

3. Step 3:

   Create the following sketch on the XY plane:

   Tip: Construct the highlighted curves; use symmetry across Y, then use a circular pattern to create 6 instances. The unneeded portions of the base diameter are then trimmed away. Finished sketch should be fully constrained.

   

   
   

4. Step 4:

   Insert > Associative Copy > Pattern Geometry

   For the Pitch Angle, select formula, then the expression angle_sections, select OK

   Notice the option in Settings for Associative geometry generation? You will want to look for Associative options in everything NX.

   We now have 3 sets of associative curves, 15 degrees apart, all on the same plane. We still need elements at 45 mm, 95 mm and those elements need scaling; 75% and 50% respectively.

   

   
   

   
   

5. Step 5:

   Extrude the first 15 degree instance 45 mm

   

   
   

   
   

6. Step 6:

   Scale the extrude to 75% in all directions but 'Z'

   

   
   

   
   

7. Step 7:

   Extrude the second 15 degree section to 95 mm

8. Step 8:

   Scale this body to 50% in all directions but 'Z'

9. Step 9:

   Hide the "Pattern Geometry"

   Resulting bodies thus far:

   We now have 3 sections with associative orientation and displacement in 'Z'

   

   
   

   
   

10. Step 10:

    Create a Through Curves feature; section 1 is the base profile, section 2 is the edge curves of the 1st (45 mm) scaled body, section 3 is the edge curves of the 2nd (95 mm) scaled body.

    Tip: The selection order is important; you want the same start curve & direction in each section. Using the Connected Curves filter, look to "options" and select Chain Between. This will allow automatic chaining after selecting a few curves.

    

    

    
    

    
    

    
    

    
    

11. Step 11:

    Remove reference bodies from Reference Set and hide bodies

12. Step 12:

    Final solid body

    

    
    

    
    

13. Step 13:

    Test associativity:

    Edit User Expression/angle_sections to 25 degrees and the resultant change; all sections are associative.