Designing a Bottle in CATIA V5: A Structured Guide

Welcome to yet another post in our CATIA V5 Design Series! Today, we’ll explore more features of the Part Design Workbench by creating a bottle model. This exercise will teach you how to use essential commands like Shaft, Shell, Fillet, and even how to generate a helix for threading. Let’s dive into this hands-on tutorial and transform a 2D sketch into a fully realized 3D model. 

Step 1: Creating the bottle profile with sketch tools 

Let’s begin crafting the bottle by sketching its profile! 

This simple outline will soon evolve into a stunning 3D creation with a quick revolve. 

1. Start a new part by clicking on Part Design from the shortcut we created earlier. Name the part "Bottle." 
2. Create a Point at the center, then select Position Sketch with the YZ plane as the reference. Set Point 1 as the origin. 

Now, let’s sketch the profile: 

1. Use the Profile and Spline Commands to draw lines and curves as shown in the reference image. The bottom horizontal line should be 45 mm, the vertical line 70 mm, and the spline should be drawn with three points. 
2. Apply dimensions as you draw by accessing the Properties Window. For instance, the vertical dimension should be 90 mm and the length of the spline line 60 mm. 
3. Continue by adding a 60 mm vertical line, a 50 mm line at a 135° angle, and a horizontal line of 25 mm, followed by a vertical line of 30 mm. 

Once the profile is complete, click Exit Sketcher. 

Step 2: Revolving the sketch with shaft command  

With the bottle profile sketched, it’s time to bring it to life in 3D!  

Let’s use the Shaft Command to revolve the sketch and form the body of the bottle. 

1. After exiting the sketch, define the Part Body as the work object. 
2. Select the Shaft Command from the Sketch-Based Features Toolbar. 
3. If you encounter an error indicating the sketch is not closed, zoom in to check for protruding lines. Correct this by adjusting the constraints or deleting problematic dimensions. 

After ensuring the sketch is valid, select Profile 1 for the Profile or Surface field, and choose the V Direction Axis as the Axis. Click OK to revolve the sketch and form the body of the bottle. 

Step 3: Hollowing the bottle with shell command 

Now that the bottle shape is formed, let’s carve out the inside with the Shell Command and give it a hollow, functional interior! 

1. Click on the Shell Command from the Dress Up Features Toolbar. 
2. In the Shell Definition Window, set the Inside Thickness to 2 mm. 
3. Select the top face of the shaft to remove it, and click OK. 

Now, the model should have a hollow interior. 

Step 4: Adding fillets to smooth edges 

Next, we’ll apply Fillets to smooth the edges of the bottle. 

1. Click on the Edge Fillet Command from the Dress Up Features Toolbar. 
2. Set the Fillet Radius to 5 mm for the bottle neck edge, and 3 mm for the smaller edges. 

This gives the bottle a polished and smooth appearance, making it more realistic and ready for production.  

 Step 5: Creating the bottle cap screw with helix command 

We’ll now add a threaded cap screw to the neck of the bottle. This involves creating a circle, a plane, and a helix profile. 

1. On the YZ plane, start a new sketch and draw a 3 mm diameter circle. Position it 25 mm from the V Direction Axis and 7 mm from the top of the bottle. 
2. Create a vertical line through the circle’s diameter, then convert the circle into a 3D Profile.

Next, we’ll generate a helix: 

1. Create a new plane by selecting the Parallel Through Point option. Choose the XY plane as a reference and use Sketch 2 Vertex for the point. 
2. Switch to the Generative Shape Design Workbench and access the Helix Command. 
3. Set the Helix Type to Pitch and Revolution, with a pitch of 5 mm and two revolutions. Choose the starting point from Sketch 2, and set the V Direction Axis as the reference. 

You should now see a helix surrounding the bottle neck. 

Step 6: Creating the screw shape with rib command 

 To create the solid shape of the screw, we’ll use the Rib Command.  

1. Return to the Part Design Workbench. 
2. Select the Rib Command from the Sketch-Based Features Toolbar. 
3. For the Profile, select the 3D Circle we created earlier, and for the Center Curve, select the Helix. 

 Click OK to complete the command. You’ll now see the screw profile added to the neck of the bottle.  

Step 7: Finishing the bottle design with fillets and project 3D elements 

With the screw shape complete, it’s time to smooth out the edges and add the final touches using the Project 3D Elements Command for a polished finish!  

1. Use the Project 3D Elements Command on the end face of the helix to create an outline sketch. 
2. Select the Shaft Command again, set the first angle to 90°, and draw a vertical line for the axis. 
3. Repeat the process on the opposite end of the helix to smooth the entire screw profile. 

 The Project 3D Elements Command is useful for creating precise sketches by projecting existing geometry.   

Step 8: Applying materials and finalizing the design 

To give your model a more realistic appearance, we’ll apply materials to the bottle. 

1. Activate the Apply Material Toolbar from the View Menu. 
2. Choose a material from the library, such as plastic or glass, and apply it to the bottle. The appearance of the model will change accordingly. 

You can also measure the volume, mass, and density of the model by using the Measure Inertia Command from the Measure Toolbar. These details are crucial for analysing the part’s behavior in real-world scenarios. 

Finally, explore the Graphics Properties Toolbar to change surface colors and identify different parts, especially when working on complex assemblies. 

Conclusion 

Congratulations! You’ve just completed the design of a bottle with a threaded cap screw in CATIA V5. We covered essential commands like Shaft, Shell, Fillet, Helix, and Rib, and learned how to apply materials and measure part properties. 

In the next discussion, we’ll dive deeper into advanced Part Design techniques, so stay tuned! 

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

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