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

Tutorial by Constantin STANCESCU
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We have to abide all the conditions from the technical drawing

  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

Comments

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    Luis Arias

    Excelente tutorial, Felicitaciones Profesor!

    May 19th, 2017 00:25