Designing an IMPELLER using SOLIDWORKS

Shahadatuliskandar Rosli

18 Apr, 2022 06:24 AM

Beginner-level SOLIDWORKS tutorial aimed at improving your 3D modelling skills to the next level. I tried to simplify the steps while making the workflow as efficient as possible. At the end of this tutorial, you would be able to:
1. Create Points reference
2. Create Splines and Splines on surface
3. Create Revolve surface
4. Create Projections curves along a direction and a workaround to project curves normal to surface
5. Create Loft Surfaces
6. Split a curve using point on curve

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1. Step 1: Before you start...

   1.     Your units are set to English. Go to Document Properties -> select IPS for Units.

   2.     The model orientation is using Z-up views.

   3.     Surfaces tab is visible.

2. Step 2: Create a sketch on the YZ plane: Sketch1

   1.     Create 5 points according to these values:

   a.     X: -2.00, Y: 0.00

   b.     X: -1.98, Y: 0.10

   c.     X: -1.20, Y: 0.70

   d.     X: -0.20, Y: 1.50

   e.     X: 0.00, Y: 2.60

   2.     Create a spline connecting all points above

   3.     Make sure the spline is horizontally constrained at the last point

   4.     Create a vertical axis line through the sketch origin

3. Step 3: Create a revolve surface: Surface-Revolve1

   1.     Select Revolved Surface from the Surfaces tab

   2.     Use the Sketch1 to create a revolve surface

   3.     Enter 360deg as the Direction 1 angle

   4.     Click OK

4. Step 4: Create a sketch on the offset plane: Sketch2

   1.     Create 4 points according to these values:

   a.     X: -0.20, Y: 0.59

   b.     X: 0.25, Y: 1.00

   c.     X: 0.70, Y: 1.80

   d.     X: 1.25, Y: 2.165

   2.     Create a spline connecting all points above

   3.     Exit sketch

5. Step 5: Create projected curve on Surface-Revolve1: Curve1

   1.     Select Project Curve from Curves command

   2.     Use Sketch2 as item to project

   3.     Select Surface-Revolve1 as projection face

   4.     Click OK

6. Step 6: Create a sketch on the YZ plane: Sketch3

   1.     Create 3 points according to these values:

   a.     X: -2.00, Y: 1.30

   b.     X: -0.50, Y: 1.80

   c.     X: -0.20, Y: 2.50

   2.     Create a spline connecting all points above

   3.     Create a vertical axis line through the sketch origin

7. Step 7: Create a revolve surface: Surface-Revolve2

   1.     Select Revolved Surface from the Surfaces tab

   2.     Use the Sketch3 to create a revolve surface

   3.     Enter 360deg as the Direction 1 angle

   4.     Click OK

8. Step 8: Create a normal line to Surface-Revolve2 from start point of Curve1: 3DSketch1

   1.     Select 3D Sketch

   2.     Select Line

   3.     Pick start point of Curve1

   4.     Make sure the line ends outwards from Surface-Revolve1, passing through Surface-Revolve2

   5.     Multi-select the line and Surface-Revolve2

   6.     Set Perpendicular as sketch relation

   7.     Exit sketch

9. Step 9: Create a vertical line upwards from end point of Curve1: 3DSketch2

   1.     Select 3D Sketch

   2.     Select Line

   3.     Pick end point of Curve1

   4.     Make sure the line ends upwards from Surface-Revolve1, passing through Surface-Revolve2

   5.     Exit sketch

10. Step 10: Create a loft surface: Surface-Loft1

    1.     Select Lofted Surface from the Surfaces tab

    2.     Select 3DSketch1 and 3DSketch2 as the Profiles

    3.     Select Curve1 as the Guide Curve

    4.     Click OK

11. Step 11: Create an intersection curve: 3DSketch3

    1.     Select 3D Sketch

    2.     Select Intersection Curve from Convert Entities command

    3.     Pick Surface-Revolve2 and Surface-Loft1

    4.     Click OK

    5.     Exit sketch

12. Step 12: Create a loft surface: Surface-Loft2

    1.     Select Lofted Surface from the Surfaces tab

    2.     Select Curve1 and 3DSketch3 as the Profiles

    3.     Click OK

13. Step 13: Create a circular pattern: CirPattern1

    1.     Select Circular Pattern from the Features tab

    2.     Uncheck Features and Faces box

    3.     Check Bodies box

    4.     Select Surface-Loft2 as Solid/Surface Bodies to Pattern

    5.     Select circular edge from Surface-Revolve1 as Pattern Axis

    6.     Enter 10.00deg as Angle

    7.     Enter 2 as Number of Instances

    8.     Make sure the circular pattern arrow is pointed upwards (click on Reverse Direction if not)

    9.     Click OK

14. Step 14: Create reference point: Point1

    1.     Select Point from Reference Geometry command

    2.     Pick inner edge of CirPattern1

    3.     Enter 1.00 as distance along curve

    4.     Click OK

15. Step 15: Create reference point: Point2

    1.     Select Point from Reference Geometry command

    2.     Pick outer edge of CirPattern1

    3.     Enter 1.30 as distance along curve

    4.     Click OK

16. Step 16: Create spline on surface: 3DSketch4

    1.     Select 3D Sketch

    2.     Select Spline on Surface

    3.     Pick Point1 & Point2

17. Step 17: Trim surface using 3D Sketch: Surface-Trim1

    1.     Select Trim Surface from the Surfaces tab

    2.     Select the lower surface area relative to 3DSketch4 as Pieces to Keep

    3.     Click OK

18. Step 18: Create a circular pattern: CirPattern2

    1.     Select Circular Pattern from the Features tab

    2.     Uncheck Features and Faces box

    3.     Check Bodies box

    4.     Select Surface-Loft2 as Solid/Surface Bodies to Pattern

    5.     Select circular edge from Surface-Revolve1 as Pattern Axis

    6.     Enter 5.00deg as Angle

    7.     Enter 2 as Number of Instances

    8.     Make sure the circular pattern arrow is pointed upwards (click on Reverse Direction if not)

    9.     Click OK

19. Step 19: Create reference point: Point3

    1.     Select Point from Reference Geometry command

    2.     Pick inner edge of CirPattern2

    3.     Enter 1.50 as distance along curve

    4.     Click OK

20. Step 20: Create reference point: Point4

    1.     Select Point from Reference Geometry command

    2.     Pick outer edge of CirPattern1

    3.     Enter 1.93 as distance along curve

    4.     Click OK

21. Step 21: Create spline on surface: 3DSketch5

    1.     Select 3D Sketch

    2.     Select Spline on Surface

    3.     Pick Point3 & Point4

22. Step 22: Trim surface using 3D Sketch: Surface-Trim2

    1.     Select Trim Surface from the Surfaces tab

    2.     Select the lower surface area relative to 3DSketch4 as Pieces to Keep

    3.     Click OK

23. Step 23: Create a circular pattern: CirPattern3

    1.     Select Circular Pattern from the Features tab

    2.     Uncheck Features and Faces box

    3.     Check Bodies box

    4.     Select Surface-Loft2 and Surface-Trim1 as Solid/Surface Bodies to Pattern

    5.     Select circular edge from Surface-Revolve1 as Pattern Axis

    6.     Enter 360.00deg as Angle

    7.     Enter 18 as Number of Instances

    8.     Make sure the circular pattern arrow is pointed upwards (click on Reverse Direction if not)

    9.     Click OK

24. Step 24: Create a circular pattern: CirPattern4

    1.     Select Circular Pattern from the Features tab

    2.     Uncheck Features and Faces box

    3.     Check Bodies box

    4.     Select Surface-Trim2 as Solid/Surface Bodies to Pattern

    5.     Select circular edge from Surface-Revolve1 as Pattern Axis

    6.     Enter 360.00deg as Angle

    7.     Enter 36 as Number of Instances

    8.     Make sure the circular pattern arrow is pointed upwards (click on Reverse Direction if not)

    9.     Click OK

25. Step 25: Clean-up

    Make all the necessary clean-up to make sure only related surfaces are visible.