How to design a Steering Knuckle (Request)

Yahya T Khedr

27 Aug, 2018 08:45 AM

==Request Tutorial==

I've spent 3+ hours working on this tutorial just to show you how to design this model in SolidWorks 2016: Steering Knuckle (2D to 3D Request)

Note: The Unit system we'll use is mm.

1. Step 1: Revolve1

   Make a Revolved Base from this sketch (on the Front plane)

   

2. Step 2: Cut-Extrude1

   Draw a new sketch on the face in the image.

   

   
   

   Draw a circle, add a "Vertical" relationship between its centre and the origin then use "Circular Sketch Pattern" command to make the other 4.

   The circles' centres must be on the construction geometry (dotted) circle.

   

   
   

   Choose "Extruded Cut", then choose "Up to Next" for Direction 1.

   

3. Step 3: Boss-Extrude1

   Draw a new sketch on the face in the image.

   

   
   

   Since this sketch is a complicated one, check this video to know how to draw it.

   You'll end up with something like this:

   

   
   

   Now Choose "Extruded Boss/Base", then make its depth 37 mm.

   

4. Step 4: CirPattern1

   Use "Circular Pattern" command to pattern (Boss-Extrude1) 3 times around the face selected in the image.

   

   
   

   
   

   
   

   
   

   
   

5. Step 5: Boss-Extrude2

   Draw a new sketch on the face in the image.

   

   
   

   Here we'll use "Convert Entities" command twice: for the outer circle (the dotted one from Sketch2) and for the 3 holes from (Boss-Extrude1)

   

   
   

   Choose "Extruded Boss/Base", then make its depth 29 mm (inwards).

   

   
   

6. Step 6: Boss-Extrude3

   Draw a new sketch on the face in the image.

   

   
   

   Draw one side (the upper one in my design).

   

   

   
   

   Then mirror the sketch about the selected (blue) centerline using "Mirror Entities" command.

   

   
   

   Choose "Extruded Boss/Base", add a 10 mm offset (inwards), then make its depth 10 mm (inwards).

   Don't extrude the whole sketch, only the part shown in the image.

   

   
   

   
   

   
   

7. Step 7: Boss-Extrude4

   Select (Sketch5), choose "Extruded Boss/Base",

   Under Direction 1 choose "Mid Plane", add a 15 mm offset (inwards), then make its depth 14 mm.

   

8. Step 8: Boss-Extrude5

   Draw a new sketch on the Front plane.

   

   
   

   Notice that the following arcs aren't tangent to the lines on their right, but to the ones on their left.

   

   

   
   

   Choose "Extruded Boss/Base", under Direction 1 choose "Mid Plane", then make its depth 30 mm.

   

   
   

   
   

9. Step 9: Cut-Revolve1

   Draw a new sketch on the Front plane.

   

   
   

   Notice that the 1st selected (orange) line is vertical, while the other line's endpoint is coincident with the 2nd selected (blue) line's midpoint.

   

   
   

   Do the same thing below.

10. Step 10: Cut-Extrude2

    Draw a new sketch on the face in the image.

    

    
    

    Draw this sketch by tracing along the edge, then add the arcs.

    

    
    

    Choose "Extruded Cut", "Up to Surface" for Direction 1, then select the bottom face as in the image.

    

    
    

11. Step 11: Boss-Extrude6

    Draw a new sketch on the Right plane.

    

    
    

    Choose "Extruded Boss/Base", add a 77 mm offset (inwards), then make its depth 8 mm (inwards).

    Ensure that the offset and extrusion directions are opposite to each other.

    

    
    

    
    

    
    

12. Step 12: Boss-Extrude7

    Draw a new sketch on the Right plane.

    

    
    

    The endpoint of the arc (from Boss-Extrude1) must be coincident with the selected (orange) line.

    

    
    

    Choose "Extruded Boss/Base", add a 53 mm offset (inwards), then make its depth 65 mm (outwards).

    Ensure that the offset and extrusion have the same direction.

    

    
    

    
    

13. Step 13: Cut-Extrude3

    Draw a new sketch on the Top plane.

    

    

    

    
    

    Choose "Extruded Cut", then choose "Up to Next" for Direction 1.

    

    
    

    
    

14. Step 14: Boss-Extrude8

    Draw a new sketch on the face in the image.

    

    
    

    

    

    
    

    Choose "Extruded Cut", from "Vertex", then select the marked vertex in the image.

    Make 1st direction 15 mm (upwards), 2nd direction 35 mm (downwards).

    Don't forget to uncheck "Merge result" option.

    

    
    

    
    

    
    

15. Step 15: Cut-Extrude4

    Draw a new sketch on the Front plane.

    

    

    
    

    Choose "Extruded Cut", then choose "Up to Next" for Direction 1.

    

    
    

    In "Feature Scope", under "Selected bodies", select (Boss-Extrude8).

    

    
    

    
    

    
    

16. Step 16: Combine1

    Go to Insert > Features > Combine, or search for it in "Search Commands"

    Choose "Add", then select both bodies.

    

    
    

    
    

17. Step 17: Sketch14

    Draw a new sketch on the face in the image.

    

    
    

    Draw 2 points, then make them horizontal with the circle's centre.

    

    
    

    
    

    
    

    
    

18. Step 18: Plane1

    Under "Reference Geometry", choose "Plane".

    Select the face first, then make it "Perpendicular".

    Select the 2 points from (Sketch14).

    

    
    

    
    

19. Step 19: Cut-Revolve2

    Draw a new sketch on (Plane1).

    

    
    

    The line's (on the right) endpoint must be coincident with the top line's midpoint.

    

    
    

    Use "Convert Entities" to convert these 2 lines from (Sketch7), then add a relation between them and their correspondents in the sketch (Equal relation).

    

    
    

    
    

20. Step 20: Revolve2

    Make a Revolved Boss from this sketch on the Front plane.

    

    

    
    

    Now your model should be like this:

    

    
    

    
    

    Hope you liked this tutorial...