How to model a Bearing Support Lug in SolidWorks

Jack K

28 Nov, 2018 11:24 PM

Denisa Maria asked for help with modeling this part. Looked like an easy part, until I noticed the rounded perimeter (R100). Here's the steps I used to make it with SolidWorks.

1. Step 1: Reference drawing

   The drawing below has most of the dimensions to define this part

   

   
   

   I don't see dimensions for the size of the two smaller holes on the bottom - I made them Ø10.

   
   

2. Step 2: Start with the main shape

   1. Make a new Part file
   2. Draw the sketch shown below in the Front plane

   
   

   (the 5.300 distance was calculated by adding the 1.3 lip and the R4 fillet)

   
   

   Using the sketch to make an Extruded Boss feature. Use the Mid Plane option with a total depth of 40mm

   

   
   

   
   

   
   

   
   

3. Step 3: Round off the outer perimeter

   
   

   
   

   1. Based on the R100 dimension in the section view of the drawing, draw a sketch like this in the Top plane. Make sure the R100 arc is touching the sketch1 profile. 

   

   2.  Add a Swept Cut feature to round off the outside: The profile is Sketch2, the path is Sketch1

   

   
   

   Here's the model so far: 

   

   
   

4. Step 4: Round off the sharp edges

   
   

   1. add a R4 fillet to the front and back faces

   

   
   

   
   

5. Step 5: Add the shoulder

   1. draw a sketch like this in the Front plane:

   

   
   

   2. Revolve the sketch about the center axis to form the shoulder

   

   
   

   3. Add a R4 Fillet along the edge

   

6. Step 6: Add the threaded hole

    Use the Hole Wizard to add the M45 threaded hole at the center of the shoulder.

   

   
   

   (I don't have a M45 thread with a 2mm pitch in my SolidWorks catalog, so I used a different pitch)

   
   

   
   

7. Step 7: Add the bearing hole

   1. Draw a sketch of the profile of the Ø75 hole in the Top plane.  Include the two retaining ring slots.

   

   
   

   2. Add a Revolved Cut using the sketch to create the hole

   

   
   

8. Step 8: Add the small holes

   
   

   
   

   1. draw a sketch of the two center points in the Front plane

   

   
   

   2. use the Hole Wizard again to add these two drilled holes.  (I used Ø10 for the size and added countersinks to both sides.) Select both centerpoints in the Positioning tab page

   

   
   

9. Step 9: Fini

   The part is done!   Add some material, and change the View Settings to get a realistic rendering of your part.  And don't forget to save your part file!

   

   
   

   I'm still learning SolidWorks myself, so I would appreciate any tips and advice on how to improve my modeling techniques.

   
   

   And if you liked this tutorial, please give me a "thumbs up" reply.