CATIA Part With 2 Cones

Jack K

2 Jun, 2022 09:17 PM

In response to a GRABCAD question from Ayo, here are the steps to make this 3D model in CATIA V5. There are probably many other methods to model this part, but these steps are pretty commonly used.

I'm assuming that users of this tutorial know the CATIA basics (like how to make a sketch).

1. Step 1: Start

   Attached is a dimensioned drawing of Ayo's part. I've added where I want the part origin to be in red for reference.

   
   

   Before we start;

   *** change the CATIA workbench to PART DESIGN

   *** and change the UNITS to millimeters

   
   

   

   
   

2. Step 2: 2 Pads

   Begin the model by making a sketch (XY plane) of the base and make a Pad (I think it's 15mm thick - hard to read).

   
   

   Then sketch the vertical wall and make a second Pad (20mm thick).

   
   

   Here's what we should have to start:

   

   
   

3. Step 3: Fillets between pads

   Using the Edge Fillet tool, select both of the sharp edges, enter a Radius of 17, and click OK.

   

   
   

4. Step 4: Add the gusset

   In the YZ plane, sketch the top of the gusset (50 x 50).

   

   
   

   Then use the Stiffener tool to make the gusset 12mm thick.

   

   
   

   
   

5. Step 5: Upper Cone

   Again in the YZ plane, sketch the half profile of the upper cone. Change the centerline to be the Axis, and dimension as shown. The axis (centerline) should be constrained as concentric to the half circle on top. Rotate this sketch with the Shaft tool to make the cone.

   

   
   

6. Step 6: Lower cone

   Repeat Step 5, make another profile sketch of the lower cone, with the axis colinear with the Z axis.

   

   
   

   
   

   Just like the other cone, use the Shaft tool to rotate the sketch profile 360°

   

   
   

7. Step 7: oops - forgot something

   I just noticed the two rounded corners on the base plate.

   
   

   It doesn't really matter where we add them, but I like to organize the tree by placing fillets immediately after the pad or pocket they belong to. So, right-click on Pad.1 in the tree and choose the DEFINE IN WORK OBJECT option. This will temporarily ignore everthing below the pad, and let us add new features below.

   
   

   Using the Edge Fillet tool, round-off the left most edges with a 14mm radius, like this:

   

   
   

   Good! Now right-click on the PartBody and again choose the DEFINE IN WORK OBJECT option to continue adding new features at the bottom of the tree.

8. Step 8: Upper hole

   Referring to Ayo's drawing, the upper cone has a Ø20 thru hole, with a Ø30 C'bore, 12mm deep.

   
   

   Using the CATIA Hole wizard; click on the half circle to center the hole, and then click on the front face where the hole starts, and then click on the Hole icon in the toolbar.

   
   

   The Extension should be set to UP TO LAST, with the Diameter = 20mm.

   
   

   The Type should be set to COUNTERBORED, with the Diameter = 30, and Depth = 12.

   

9. Step 9: Lower hole

   Use the Hole wizard again for the lower hole.

   
   

   Referring to the drawing; Ø16 thru hole with Ø 30 C'Bore, 12mm deep.

   

10. Step 10: The end

    Here's the final 3D model. Don't forget to save your file!

    

    
    

    Please use the comments if you have any questions about this.

    
    

    And please give me a LIKE vote if you learned something and this tutorial was useful - thanks