Creating the Connecting Bush in CATIA V5: A Step-by-Step Guide

Welcome back to our CATIA V5 Design Series! In this session, we’ll explore how to construct a connecting bush between the circular and rectangular bosses of a model, as shown in the image below. This blog will walk you through the process of using CATIA's Sketcher, Surfaces, and Part Design commands to achieve this, as well as how to create the corresponding drawings.

Let’s jump into the process and discover how surface-based features and solid modeling commands come together to create a functional component.

Constructing the Connecting Bush

To start, we’ll create the connecting bush using a combination of sketches and surface design commands.

1. Insert a New Geometrical Set: In the CATIA window, begin by inserting a new geometrical set and renaming it as Connecting Bush. This will help organize the steps of the model.
2. Create a Plane: Hide the 3D profiles and bush surfaces for better visibility. Then, create a new plane at a 78 mm distance from the ZX plane. This plane will serve as the base for our next sketch.
3. Draw the Base Sketch: Start a positioned sketch on the new plane, aligning the V and H directions properly. Draw a rectangle and apply the necessary constraints to match the dimensions seen in the reference image.
4. Extrude the Profile: Switch to the Generative Shape Design Workbench and use the Extrude command from the surfaces toolbar. Extend the surface of the profile perpendicular to the XZ plane. Set the limit one type to up to element and select the inside face of the circular boss as the limiting element. The limit two dimension should remain at zero.

1. Perform the Split Operation: Define the base part body as the active work object, and use the extruded connecting bush surface as the splitting element. Repeat this split operation for both the circular boss and rectangular boss to integrate the connecting bush into the model.

Converting the connecting bush into a solid body

Now that we’ve constructed the connecting bush as a surface, we need to convert it into a solid body.

1. Insert a New Body: Under the part body, insert a new body and name it Connecting Bush. This new body will be used to differentiate the connecting bush from the other components.
2. Thicken the Surface: Use the Thick Surface Command from the surface-based features toolbar to add a 6 mm thickness to the connecting bush surface. Ensure the offset direction is correct by using the reverse direction button if needed.
3. Apply a Boolean Operation: To combine the connecting bush with the circular and rectangular bosses, perform an Add Boolean Operation. This will merge the subpart bodies into one cohesive unit.

Creating Holes and applying Fillets to the base frame

Now, let’s create holes on the base frame and apply fillets to smooth the edges.

1. Unhide the Sketch for the Holes: Ensure the Part Design Workbench is active, and unhide the sketch that contains the pre-drawn holes for the base frame.
2. Use the Pocket Command: Define the base part body as the work object, then select the Pocket Command from the sketch-based features toolbar. Select the sketch for the holes as the profile and apply the reverse direction to cut through the base frame. Click OK to complete the pocket feature.
3. Apply Fillets to the Edges: Use the Edge Fillet Command from the Dressup Features Toolbar. Select the edges of the base frame and set the fillet radius to 3 mm. Preview the fillet to ensure accuracy, then confirm the operation by clicking OK.

Creating the drawing for the model

Finally, we’ll create a technical drawing of this model, allowing us to verify all dimensions and showcase the final design.

1. Switch to the Drafting Workbench: From the start menu, click on Mechanical Design and select the Drafting Workbench. Choose an empty sheet and click OK to create a new drawing sheet.
2. Add Views to the Drawing: Use the Front View Command to place the front view of the solid model on the drawing sheet. Add a Projected View for more perspective. Insert a Section View by drawing the section line across the model and positioning the view above the front view.
3. Adjust View Layout: If necessary, move the Section View below the front view by clicking on the view frame and dragging it to the desired position. Edit the view properties to display the centerlines for improved clarity.
4. Add Dimensions: Use the Dimensions Command to add linear, radius, and diameter dimensions in each view. Ensure all key measurements are included to accurately describe the model.
5. Place the Isometric View: Finally, click on the Isometric View Command and switch back to the model window. Place the isometric view on the drawing sheet for a complete visual representation. You can also add another side of the isometric view to further clarify the geometry.

With all the views, dimensions, and details in place, the drawing of the model is now complete!

Conclusion

In this session, we successfully walked through the process of creating a connecting bush between the circular and rectangular bosses using CATIA V5. From the initial sketch and surface extrusions to converting the surfaces into solid bodies and applying final touches like holes and fillets, we explored key tools in the Sketcher, Surfaces, and Part Design workbenches.

Creating drawings of complex models not only helps verify their dimensions but also ensures a clear, visual understanding of how each part fits together. Stay tuned for more tutorials in our CATIA V5 Design Series, where we’ll dive deeper into advanced modeling techniques and drafting best practices.

For more hands-on learning, explore our FREE CATIA V5 Course at Skill-Lync and build your skills to become #IndustryReady!

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

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