Mastering Part Design and Assembly: Creating a Caster Wheel in CATIA V5

Welcome back to the CATIA V5 Design Series! In this blog, we’ll focus on designing and assembling various components of a Caster Wheel Assembly using CATIA V5. We’ll dive into using essential part design features such as sketching, applying constraints, and generating drawing views, all while keeping things simple and efficient. By the end of this guide, you'll have a clear understanding of how to create parts like axles, bushings, and wheels, then assemble them to build a fully functional product. 

Step 1: Designing the Axle 

The first part we’ll design is the Axle. To create the axle, we’ll sketch its profile and use the Shaft Command to revolve it into a 3D model. 

1. Create a New Part: Start by adding a new part and renaming it as Axle in the properties window. 
2. Open in New Window: Right-click on the axle part, navigate to Axel Object, and select Open in New Window. This will allow us to focus on creating the axle design in its own space. 
3. Start a New Sketch: Select the YZ plane to begin sketching the profile of the axle. 
4. Draw the Profile: Use the Profile Command to sketch the lines representing the axle's dimensions.
5. Offset and Mirror: Use the Offset Command to copy lines, then apply the Mirror Command along the H-axis to replicate the sketch symmetrically. 

After completing the sketch, apply the Shaft Command to revolve the profile and create the circular 3D axle. Once done, switch back to the Assembly Workbench, where the axle will automatically update. In the specification tree, you’ll see the new axle part listed under the assembly. 

Next, we’ll reposition the axle using the Manipulation Tool to ensure it’s aligned properly within the assembly. 

Step 2: Designing the bushing 

Like the axle, the Bushing will also be created using the Shaft Command to revolve a sketch into a solid model. 

1. Create a New Part: Insert a new part, rename it as Bushing, and open it in a new window. 
2. Start a Sketch: Sketch the bushing profile on the YZ plane using the Profile Command. 

Apply the Shaft Command to create a solid model of the bushing. Once completed, switch back to the assembly, where the bushing will automatically appear. Use the 3D Compass to move the bushing away from the top plate, ensuring proper alignment within the assembly. 

Step 3: Designing the wheel 

The final part of our assembly is the Wheel. We’ll design it by sketching an I-shaped profile and using the Shaft Command and Edge Fillet for finishing. 

1. Create a New Part: Insert a new part, rename it as Wheel, and open it in a new window. 
2. Start a Sketch: Sketch the wheel’s profile on the YZ plane, using the Profile Command to draw the necessary dimensions. Make sure to apply dimensional constraints as you go. 
3. Mirror Command: Use the Mirror Command to replicate the sketch symmetrically across the V-axis. 

After the sketch is complete, apply the Shaft Command to add thickness to the wheel and form a 3D model. To smooth out sharp edges, apply a 5mm Edge Fillet to finish the wheel design. 

Step 4: Assembling the parts 

With all the parts designed, it’s time to assemble them. 

1. Insert another instance of the Axle Support and Bushing into the assembly. 
2. Use the 3D Compass or the Manipulation Feature to move the components apart for better visualization. 

Let’s begin applying constraints to lock each component into place. 

1. Fix the Top Plate: Select the Fix Component Command and apply it to the top plate, locking it into place. 
2. Align Axle Supports: Apply Coincidence Constraints between the axes of the axle support holes and the corresponding holes in the top plate. Then, apply Contact Constraints to position them correctly. 
3. Constrain the Axle: Use a Coincidence Constraint to align the axle with one of the axle supports. Then apply an Offset Constraint of 8mm between the surfaces of the axle and axle support. 
4. Position the Wheel: Apply similar Coincidence and Offset Constraints to position the wheel, giving an offset of 9mm between the wheel and axle supports. 
5. Constrain the Bushings: Apply Coincidence and Contact Constraints between the bushings and axle, ensuring they fit snugly into place. 

Step 5: Exploded View and Scene Creation 

To create an exploded view: 

1. Generate Numbering: Click on Generate Numbering to prepare for the balloon generation in the drawing. 
2. Create an Exploded View: Use the Enhanced Scene Toolbar to create a scene, uncheck Automatic Naming, and name the scene Exploded View. 
3. Explode the Assembly: Use the Explode Option to scatter the parts and visualize the assembly better. 

Step 6: Save management and document properties 

Before we move to the drawing phase, it’s crucial to save your work efficiently, especially in complex assemblies. 

• Use Save Management from the File Menu to save all opened files without switching between documents. 
• Modify and save only the updated parts to streamline the saving process. 

Document Properties can also be accessed from the File Menu, where you can check details such as file size, version, and path, which are useful when managing multiple files.  

Step 7: Creating the assembly drawing 

Now that the Caster Wheel assembly is complete, it’s time to generate detailed drawings, including views, a Bill of Materials (BOM), and exploded views. 

1. Switch to the Drafting Workbench: Select Start > Drafting under Mechanical Design. 
2. Set Drawing Layout: Choose the First Angle Projection layout, including front, top, and left views. 
3. Insert Isometric and Exploded Views: From the Views Toolbar, insert an isometric view, then expand the Scenes in the specification tree to insert the exploded view created earlier. 

Generating the Bill of Materials (BOM) 

1. Click Insert > Generation > Bill of Material to generate a table listing all parts and quantities. 
2. Customize the table by adjusting font size, column sizes, and content, such as adding item numbers or adjusting text. 

Balloon Generation 

Use the Balloon Generation Command to automatically assign numbered balloons to the parts in the views. These balloon numbers will match the BOM table. 

Conclusion 

In this session, we covered how to: 

• Design the Axle, Bushing, and Wheel using the Shaft Command in CATIA V5. 
• Assemble parts using Constraints to ensure proper alignment and functionality. 
• Create an Exploded View and generate a Bill of Materials (BOM) for technical documentation. 
• Draft comprehensive assembly drawings, including multiple views and part identification balloons. 

By mastering these techniques, you’ll be well-equipped to design and assemble complex products in CATIA V5. Stay tuned for the next session, where we’ll explore more advanced techniques in assembly design.  

This blog is part of our ongoing CATIA Design Series. If you missed the previous posts, check them out here

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