Modified on
12 Sep 2024 06:56 pm
Mastering Assembly Design in CATIA V5: Building a Screw Jack and Caster Wheel
Skill-Lync
Welcome back to the CATIA V5 Design Series! In this guide, we’re diving into Assembly Design—an essential skill for mechanical designers. We’ll explore how to bring multiple parts together to form functional assemblies using constraints, and we’ll also learn how to generate drawings for the assemblies we create.
Today, we’ll focus on two practical assembly projects: a Screw Jack and a Caster Wheel. By the end of this guide, you’ll have mastered the fundamentals of assembly design in CATIA V5, including creating exploded views and generating a Bill of Materials (BOM).
Getting Started with Assembly Design in CATIA V5
Before we begin assembling our projects, it’s important to understand the Assembly Design Workbench and the toolbars that make it possible to bring individual parts together. Here’s a quick overview:
- Product Structure Tools: Used for inserting or replacing parts and products within an assembly.
- Constraints: Helps position parts by applying relationships between surfaces, axes, or points to limit their movement.
- Move: Allows us to manipulate the position of parts in the assembly.
- Assembly Features: Provides commands like split, symmetry, and tools for creating exploded views.
- Scenes: Used to create exploded views for better visualization.
In assembly design, constraints play a key role. They allow us to lock parts into place and control their motion in relation to one another. Now, let’s dive into our first project—the Screw Jack.
Step 1: Building the Screw Jack Assembly
We’ll begin by assembling a Screw Jack using the Bottom-Up Assembly approach. This method involves designing individual parts separately and then bringing them together in the assembly environment.
Setting Up the Assembly
- Start by opening a new Assembly File: Click on File > New, then select Product to initiate the Assembly Workbench.
- Rename the assembly as Screw Jack and save it.
You’ll notice that assembly files have a .CAT Product extension. This is different from the .CAT Part files used for individual parts.
There are two ways to insert parts into the assembly:
- Copy and Paste: If the parts are already open, right-click on the part name, select Copy, and paste it into the assembly window.
- Insert Existing Component: From the Product Structure Tools Toolbar, select Insert Existing Component, browse to your files, and add the required parts.
Once the parts are inserted, they might overlap. To fix this, we need to reposition and constrain them.
_1726143653.png)
Step 2: Positioning and Constraining Parts
To separate the overlapping parts, use the Manipulation Command from the Move Toolbar. This allows you to drag parts along specific axes, making it easier to visualize and prepare them for constraints. Use the Snap Command to align one part’s axis with another.
You can also spread the parts out using the explode Command, which makes all the components visible and easier to manage.
Let’s now apply constraints to lock the parts into place. Constraints help control movement along the X, Y, and Z axes as well as rotation.
- Fix the Base: Since the base of the screw jack should remain stationary, apply the Fix Constraint from the Constraints Toolbar.
- Align the Nut: Use the Coincidence Constraint to align the central axis of the nut with the base. Next, apply a Contact Constraint between the top of the base and the bottom of the nut to restrict vertical movement.
- Position the Screw: Align the screw’s axis with the nut’s axis using the Coincidence Constraint. Then, apply an Offset Constraint to set the correct height (e.g., 60 mm) for the screw.
- Add the Tommy Bar: Use the Coincidence Constraint to align the Tommy bar with the hole in the screw. Allow the bar to rotate freely by constraining only its position.
- Cap, Washer, and M12 Screw: Use a combination of Coincidence and Contact Constraints to accurately position these parts atop the screw.
Step 3: Creating an exploded view
An exploded view helps visualize and document the assembly by showing how the parts fit together.
- Switch to the Scene Toolbar and click on Enhance Scene to create a new scene.
- Use the Explode Command to spread the parts apart in a controlled manner.
- Save the exploded view for use in the drawing.
_1726143847.png)
Step 4: Building the Caster Wheel Assembly (Top-Down Approach)
Now, let’s move on to the Caster Wheel Assembly. We’ll use the Top-Down Assembly approach, where parts are designed relative to one another directly in the assembly.
Step 4.1: Designing the top plate
- Start a new assembly: Name it as Caster Wheel.
- Insert a new part: Click on Insert > New Part, and name it as Top Plate.
- Sketch the top plate: Use the Profile Command to sketch the plate. Apply Mirror, Pad, and Fillet Commands to complete the design.
- Add Holes: Create holes with a diameter of 11 mm, positioned 12mm from the edges.
_1726146616.png)
Step 4.2: Designing the Axle Support
- Insert a new part: Name it as Axle Support and start a sketch relative to the top plate.
- Sketch the axle support: Begin by creating the L-shaped support. Add holes and apply the Pad and Pocket Commands to shape the structure.
- Fillets: Smooth the edges with Fillets to ensure the design is ready for manufacturing.
_1726144308.png)
Step 5: Creating Assembly Drawings
Once the assemblies are complete, we’ll create technical drawings to communicate the design.
Step 5.1: Drafting the Screw Jack and Caster Wheel
Switch to the Drafting Workbench: Select File > New > Drawing, then choose an empty sheet for layout.
Insert Views: Use the Views Toolbar to add Top View, Section Views, and Isometric View for each assembly.
Add Dimensions: Use the Dimensioning Toolbar to specify key measurements for each part.
Insert the Exploded View: Use the scene we created earlier to add the exploded view, providing a clear illustration of how the parts fit together
Step 5.2: Generating the Bill of Materials (BOM)
Congratulations! You’ve successfully learned to:
- Assemble parts in CATIA V5 using both the Bottom-Up and Top-Down approaches.
- Apply constraints to lock parts in place.
- Create an exploded view to visualize complex assemblies.
- Generate a Bill of Materials (BOM) and assembly drawings for documentation.
With these skills, you’ll be able to tackle more complex assemblies and communicate your designs clearly through technical documentation. Stay tuned for the next session, where we’ll explore more advanced assembly techniques and delve deeper into creating detailed assembly drawings.
This blog is part of our ongoing CATIA Design Series. If you missed the previous posts, check them out here
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Author
Alda Rovina
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