Learn how to create a Lofted Elbow in Fusion Sheet Metal

As a long-time Fusion user, I'm often tasked with creating complex sheet metal parts and assemblies. One particular challenge that comes up frequently is the need to design a 90° elbow unit in sheet metal. While Fusion's built-in Flange command makes this process relatively straightforward, there's a catch - the Flange tool can only loft between two profiles, leaving us in a bind when we need to create a more intricate elbow shape.

In this in-depth blog post, I'll walk you through a clever workaround that allows us to create a 90° lofted elbow in Fusion sheet metal. By building a "template model" first, we can generate the necessary profiles to feed into the Flange tool and achieve our desired elbow shape. I'll also share a pro tip on how to efficiently lay out all the flat pattern views on a single drawing sheet - a huge time-saver in your design workflow.

So, if you're ready to level up your Fusion sheet metal skills, let's dive in!

Understanding the Limitations of the Flange Tool

Before we get started, it's important to understand the capabilities and limitations of Fusion's Flange tool. This powerful feature allows us to create lofted flanges, where the sheet metal is bent and formed along a specified path. However, the Flange tool is constrained to only loft between two profiles - it cannot handle more complex shapes that require multiple profile transitions.

In the case of our 90° elbow, we need to create a series of angled profiles that gradually transition from the vertical to the horizontal orientation. That's where our "template model" approach comes into play.

Building the Template Model

The key to creating our 90° lofted elbow is to first build a template model that will serve as the foundation for the sheet metal components. Here's how we'll do it:

1. Start a New Component: In Fusion, create a new component and name it "Pipe Design Assembly". This will be the container for our template model.

2. Define the Pipe Diameter: Begin by sketching a 4-inch circle on the bottom plane. This will represent the diameter of our pipe.

3. Create the Elbow Path: Next, create a sketch on the front plane and use the Edge Polygon tool to sketch the path that the elbow will follow. Set the height to 3 inches and the number of sides to 12. This will give us a multi-angled profile that approximates the 90° bend. Use the Trim tool to remove the sections of the path we don't need.

4. Sweep the Profile: With the profile and path sketches complete, use the Sweep tool to create the 3D template model. This will form the basic elbow shape we're aiming for.

At this point, we have the foundation of our 90° elbow template. However, we still need to extract the individual profile sketches that will be used to create the sheet metal components.

Extracting the Profile Sketches

To get the necessary profile sketches, we'll need to create a series of construction planes that intersect the template model at key points along the elbow. Here's how:

1. Create Construction Planes: Use the "Plane Through 3 Points" tool to generate construction planes that slice through the elbow template at various angles. These planes will serve as the basis for our profile sketches.

   1. Use the Point on a Path command to create a 3rd point on the profile for the Plane Through 3 Points to work.

2. Project the Intersections: On each construction plane, use the "Project-Intersect" command to project the intersection of the template model onto the sketch. This will give us the profile shapes we need.

3. Repeat for Multiple Profiles: Create sketches on several construction planes to capture the different profile shapes along the elbow's transition.

With these profile sketches in hand, we're now ready to start building the actual sheet metal components.

Constructing the Sheet Metal Elbow

Now that we have the necessary profile sketches, we can begin creating the sheet metal parts that will make up our 90° elbow. Here's the step-by-step process:

1. Create a New Sheet Metal Component: Right-click on the "Pipe Design Assembly" and select "New Component". Change the component type to "Sheet Metal" and name it "Section1".

2. Use the Lofted Flange Tool: Use the Lofted Flange tool to create the first section of the elbow. Select the two profile sketches you created earlier and let Fusion loft the sheet metal between them.

3. Add the Rip/Cut: To allow the sheet metal to be unfolded flat, use the Rip tool to create a cut or seam along the inside of the elbow. Carefully select the appropriate vertices to ensure the rip is positioned correctly.

4. Repeat for Additional Sections: Create a new sheet metal component for each additional section of the elbow, repeating the Lofted Flange and Rip steps as needed.

5. Optional: Mirror the Components: To complete the elbow, use the Mirror tool to create the mirrored versions of the sheet metal sections.

   
   

By following this process, you'll end up with a fully parametric 90° elbow assembly, made up of individual sheet metal components that can be easily unfolded and laid out flat.

Laying Out the Flat Patterns

The final step in our 90° elbow design workflow is to create a drawing that includes all the necessary flat pattern views. This will allow you to easily fabricate the individual sheet metal pieces. Here's how to do it:

1. Make sure you have created Flat Patterns for each of your Sheet Metal components using the Flat Pattern command in Sheet Metal.

2. Create a New Drawing: With one of the flat pattern views active, go to "Drawing" > "New Drawing from Design". Choose the appropriate drawing standard (in this case, ASME inch) and select a C-size sheet.

3. Place the First Flat Pattern: The new drawing will be created with the active flat pattern view already placed on the sheet. Adjust the scale as needed (e.g., 1:2).

4. Save the drawing.

5. Add Additional Flat Patterns: To add the remaining flat patterns, simply activate each sheet metal component in turn and use the "Drawing" > "From Design" command again. This time, instead of creating a new drawing, select the existing "Pipe Example Drawing" and choose to place the new flat pattern on the same sheet.

6. Create a Base View: As a final touch, add an isometric base view of the assembled elbow to the drawing. This will provide a clear visual reference for the final 3D part.

By following this workflow, you'll end up with a comprehensive drawing that includes all the necessary flat pattern views, as well as a 3D representation of the completed 90° elbow assembly.

Conclusion

Mastering the art of creating lofted elbows in Fusion sheet metal is a valuable skill that can elevate your design capabilities. By leveraging the "template model" approach outlined in this blog post, you'll be able to tackle even the most complex sheet metal challenges with confidence. With a little practice, you'll be designing 90° elbows and beyond in no time.