Mastering Surface Design in CATIA V5: Modeling an Enclosure

Welcome to another session of our CATIA V5 Design Series! In this tutorial, we will explore surface modeling by designing an enclosure, a structure often used in product design. We will walk through several commands from both the Part Design and Generative Shape Design workbenches to achieve a hollow, smooth-surfaced enclosure. 

This enclosure consists of two rectangular bodies with filleted edges, a base frame with holes and stiffeners, and a hollow interior. Let’s get started! 

Step 1: Creating the Enclosure Sketch 

We begin by creating the main profile of the enclosure. 

1. Create a New Part: Open a new part in CATIA and name it Exercise 2. Rename the Geometrical Set as Top Sketch. 
2. Create the Base Sketch: In the Sketcher Workbench, create a positioned sketch. Using the Centered Rectangle Command, draw two rectangles, one inside the other. Apply the Corner Command to round the sharp edges of one side of the profile. 
3. Convert the Sketch to 3D: To keep the sketch visible after exiting the sketcher, use the 3D Profile Command. This makes it easier to reference the profile later. 

Step 2: Drawing the Section View 

Next, we’ll create a section view sketch for the front profile of the enclosure. 

1. Insert a New Geometrical Set: Rename this new set as Section Sketch. Start a new positioned sketch on the XY plane. 
2. Draw the Section Profile: First, create a horizontal axis through the origin. Then, draw a centered rectangle and a circle, constraining the circle so it is tangent to the top line of the rectangle. Use the Quick Trim Command to remove any unwanted edges, leaving the section view ready for extrusion. 

Step 3: Extruding and Trimming Surfaces 

Now, we will extrude the 3D profiles and trim the unnecessary surfaces to form the enclosure’s body. 

1. Switch to Generative Shape Design: Make the Top Sketch the active work object and use the Extrude Command to create a surface from the profile. Make sure the extrusion extends beyond the actual height, as we will trim it later. 
2. Extrude the Section Sketch: Similarly, extrude the section profile. Again, make sure the extrusion extends beyond the necessary limits. 
3. Trim the Surfaces: Use the Trim Command from the Operations Toolbar to clean up the excess surfaces. Select the extruded surfaces to define which areas to trim, ensuring the correct final shape is achieved. 
4. Fillet the Edges: Apply the Edge Fillet Command to smooth the sharp corners of the surfaces for a polished finish. 

Step 4: Using a Sphere for the Curved Top 

To create the curved top surface, we will switch to using a sphere rather than the extruded surface from the earlier step. 

1. Edit the Sketch for Reference: Go back to the section sketch and convert the center point of the circle into a 3D profile. This will allow us to use the point as a center for the sphere. 
2. Use the Sphere Command: From the Surfaces Toolbar, select the Sphere Command and input a radius of 250 mm. Ensure the sphere is a full 360° by selecting the Create Whole Sphere option. 
3. Replace the Extruded Surface: Replace the previous extrusion with the newly created sphere surface. This creates a more natural curvature across all planes. Finally, modify the trim operation to integrate the sphere with the other surfaces. 

Step 5: Creating the Base Frame 

Next, we will create the base frame for the enclosure. 

1. Draw the Base Sketch: Start a new positioned sketch on the YZ plane. Use the Project 3D Silhouette Edges Command to reference the outer profile of the existing model. 
2. Constrain the Sketch: Add circles to represent the holes on the base, with radii of 6 mm and 15 mm, respectively. Mirror the circles across the V direction axis. 
3. Extrude the Base Profile: Convert the base sketch into a 3D profile and extrude it perpendicular to the YZ plane. 

Step 6: Splitting and Trimming the Surfaces 

Now that we have the base and the enclosure, we’ll apply splitting and trimming operations. 

1. Extrude a Horizontal Line: Extrude a horizontal line from the base sketch to form a flat surface normal to the XY plane. 
2. Apply the Split Command: Use the Split Command to remove the unwanted portions of the extruded surfaces. This will hollow out the bottom of the enclosure. 
3. Final Trim: Apply a Trim Command to remove the remaining unwanted surfaces, creating a clean hollow enclosure. 

Step 7: Thickening the Surface 

To transform the surface model into a solid object, we will add thickness and strengthen the structure. 

1. Switch to Part Design Workbench: Use the Thick Surface Command to add 5 mm thickness to the hollow surfaces. 
2. Apply Fillets: Use the Edge Fillet Command to smooth the sharp corners. Apply 20 mm fillets to the large edges and 10 mm fillets to the smaller ones. 
3. Add Holes: Use the Pocket Feature to create holes in the base, referencing the earlier sketch. Apply 3 mm fillets to the top and bottom edges of the enclosure for a refined look. 

Step 8: Adding Stiffeners 

Stiffeners provide additional strength to the enclosure, particularly to prevent deformation. 

1. Create Stiffener Sketch: On the XY plane, draw a line angled at 75° to the YZ plane. Constrain the line at 15 mm vertically from the surface of the model. 
2. Use the Stiffener Command: With the line selected, use the Stiffener Command to add material. Set the thickness to 5 mm. 
3. Mirror the Stiffener: Use the Mirror Feature to duplicate the stiffener on the opposite side of the model. 

Step 9: Creating the Final Drawing 

To finalize the design, we will create a detailed drawing of the enclosure. 

1. Switch to Drafting Workbench: Open a new empty drawing sheet and use the Front View Command to place the main view of the enclosure. 
2. Add Projected and Section Views: Create a Projected View and a Section View to provide additional perspectives. 
3. Insert Detail Views: Add a Detail View for specific areas of the section view, showing finer details of the enclosure. 
4. Add Dimensions: Use the Dimensioning Toolbar to label the linear, radius, and angular dimensions in the drawing. 
5. Include Isometric Views: Finally, add Isometric Views to complete the drawing, showcasing all aspects of the model. 

Conclusion 

In this tutorial, we’ve covered the complete process of creating an enclosure model using Surface Design in CATIA V5. From sketching and extruding to applying fillets, stiffeners, and thickness, you now have a solid understanding of the workflow for surface modeling. By following these steps, you can confidently tackle more complex designs in CATIA and create high-quality 3D models ready for manufacturing. 

Stay tuned for more advanced tutorials and explore further features of CATIA V5 in our upcoming sessions! 

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

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