How to model a Centrifugal Pump Body (Spiral construction) using Inventor 2014?

Constantin STANCESCU

12 Mar, 2015 03:33 PM

We have to abide by all the conditions from the technical drawing

Note: You can watch my live tutorial for modeling this part here: https://youtu.be/yxEAv2p31zw

1. Step 1:

   1. New work plane at 45° from XZ Plane around the Y Axis (see 1, 2, 3, 4 steps)
   

   

2. Step 2:

   2. New sketch: Circle Ø26.75 with center at 123.5 on the same vertical with the origin (Center Point)
   

   

3. Step 3:

   3. Coil tool with Spiral option (Pitch=28, Revolution=7/8)
   

   

4. Step 4:

   4. Result from Coil/Spiral applying
   

   

5. Step 5:

   5. Creating of 5 sketches (5 circles), where the last 4 of them are related to the Center point only
   

   

6. Step 6:

   6. Loft tool on 5 sketches, using the spiral curve on the spiral feature as Centerline
   

   

7. Step 7:

   7. Result from Loft tool applying
   

   

8. Step 8:

   8. Revolving half circle on S1 around its diameter on 180° to create a hemisphere
   

   

9. Step 9:

   9. Extrude tool on a circle (radius=123.5) in the Center point using a 24 simmetrical distance
   

   

10. Step 10:

    10. Move Bodies tool to move the (unique) solid 200 to the back

    

11. Step 11:

    11. New 5 similar sketches (only one dimension differs), related to the same Center point as above
    

    

12. Step 12:

    12. Changing color of the Solid1 using Right click/Properties
    

    

13. Step 13:

    13. Loft tool with New solid option, on the 5 sketches with Centerline from the spiral curve
    

    

14. Step 14:

    14. The result is another solid in the same .ipt file (or two solids of different colors)
    

    

15. Step 15:

    15. New sketch on an existing plane - a circle is automatically projected (like in 005 or 008 picture)
    

    

16. Step 16:

    16. New work plane parallel with XZ Plane through the circle center (see 1, 2, 3 steps)
    

    

17. Step 17:

    17. New sketch on XZ Plane - a centerline from the projected circle center, and other 3 lines
    

    

18. Step 18:

    18. Revolving the closed loop to obtain a conic feature associated with the Solid1
    

    

19. Step 19:

    19. New sketch for the Solid2 with a line projected from the circle of the Solid1
    

    

20. Step 20:

    20. The sketch also related to the Center point will be revolved - attached to the Solid2
    

    

21. Step 21:

    21. A sketch created on the sloped plane is revolved between it and the next one, to fill the gap
    

    

22. Step 22:

    22. Filling the central hole of the Solid2
    

    

23. Step 23:

    23. New sketch with a circle of Ø310 in a new work plane at -65 from the XZ Plane
    

    

24. Step 24:

    24. Extruding the circle To next with a taper of 3°, as in the above part drawing
    

    

25. Step 25:

    25. A new sketch in the plane XZ to extrude simmetrically on 120
    

    

26. Step 26:

    26. The result of the last two extrudes
    

    

27. Step 27:

    27. Move Bodies tool on Y Offset = 200 to get back the Solid1
    

    

28. Step 28:

    28. Combine tool to subtract (Cut) the Solid1 (as Base) from Solid2 (as Toolbody)
    

    

29. Step 29:

    29. The result (intentionally sectioned)
    

    

30. Step 30:

    30. A new sketch for creating the revolved external body
    

    

31. Step 31:

    31. Result of Revolution
    

    

32. Step 32:

    32. A new sketch for creating the revolved internal body
    

    

33. Step 33:

    33. The result (intentionally sectioned)
    

    

34. Step 34:

    34. New sketch with a Ø34 circle to create a boss for a G1/2" hole
    

    

35. Step 35:

    35. The ISO Pipe G1/2" hole, through but not through all
    

    

36. Step 36:

    36. Rib tool to create a rib, starting from a sketch in XZ Plane with a sloped line at 30°
    

    

37. Step 37:

    37. Final part