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

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