Creating Hems in Fusion Sheet Metal

https://www.youtube.com/watch?v=vPr_UiozhQI

Autodesk recently updated Fusion with a powerful new feature for sheet metal designers. You can now create sheet metal hems directly without using complex workarounds. In the past, you had to rotate flanges to 179.99 degrees to mimic a hem, which often caused issues in drawings and dimensioning. This update adds a dedicated Hem command that simplifies the process and offers several styles to fit your engineering needs. Whether you are building enclosures or brackets, these new tools make your workflow much faster and more accurate.

Getting Started with the Hem Command

The new hem functionality is easy to find within the Fusion interface. You can access it through the Create menu in the Sheet Metal tab or directly within the Flange command menu. Most users start by creating a base flange to establish the initial sheet metal body. Once you have a base, you can select the edges where you want the hem to appear.

The tool uses smart formulas by default. For example, a standard hem length might be set to the material thickness multiplied by four. This keeps your design intent intact even if you change the material thickness later. You can click the FX icon in the menu to see the exact numbers or type in your own specific dimensions, such as one inch.

Understanding Hem Positions

When you create a hem, you must choose how it sits on the edge of your part. Fusion offers two main options for bend positions:

• Adjacent: The bend happens around the original edge of the part. This keeps the outer dimensions of your flat sheet consistent with the original edge.

• Tangent: The bend happens tangent to the face of the edge. This moves the hem slightly so the outer face of the bend stays in line with the original edge of your part.

Exploring the Six Hem Types

Fusion provides six different hem styles. Each one serves a different purpose for strength, safety, or assembly.

Flat Hems

The flat hem is the most basic style. It folds the material back so it sits flush against the main face. This is great for hiding sharp edges on a metal sheet. It creates a tight fold that adds stiffness to the edge of a panel without adding much bulk.

Open Hems

An open hem leaves a small gap between the fold and the main face. By default, Fusion sets this gap to match the material thickness. You can adjust this gap using formulas. For example, if you want a tighter gap but not a flat one, you could set the formula of thickness divided by two. This style is useful if you need to slide another piece of material into the gap later.

Rolled Hems

The rolled hem creates a circular profile at the edge. It uses a radius and an angle to define the shape. The default angle is 270 degrees, which creates a nice rounded edge. You can increase the radius to create a larger "grab handle" style edge or decrease it for a subtle rounded finish. This style is often used to create built-in sheet metal hinges.

Teardrop Hems

A teardrop hem is a mix between a flat and a rolled hem. It features a radius at the bend but then flattens out as it reaches the end of the fold. You can control the radius, the length, and the gap. A unique feature of the teardrop style is that the angle changes automatically when you change the length. This ensures the fold remains tangent to the bend, creating a smooth transition.

Rope Hems

The rope hem is very similar to the teardrop style but adds an extra radius at the end of the fold. This creates a very smooth, rounded look that resembles a rope edge. You can adjust the gap and the length to "squish" the hem down or leave it more open. This is a high-quality finish often seen on premium metal products.

Double Hems

The double hem is a complex fold where the metal folds back on itself twice. It introduces a new setting called setback. Setback is the distance from the original edge to the inside face of the second fold. This style is sometimes used for joining two different sheets of metal together by sliding them into each other.

Working with Multiple Edges and Corners

One of the most powerful parts of the new update is the ability to select multiple edges at once. You can hold down the control key and select all four edges of a square part. Fusion will apply the hem to all sides simultaneously.

When you have multiple hems meeting at a corner, you need to manage how they overlap. Fusion includes override rules to handle these situations. You can choose from several corner relief types:

• Round Relief: Creates a circular cutout where the hems meet.

• Square Relief: Uses a simple square cutout.

• Linear Weld: Prepares the corner for a straight weld bead.

• Arc Weld: Creates a curved space that is ideal for adding weld material.

You can also adjust the gap between the hems at the corner. This ensures that when the part is physically manufactured, the metal has enough room to bend without hitting the neighboring side.

Flexible Hem Lengths

You do not always have to apply a hem to a full edge. Fusion allows you to change the extent of the hem just like a standard flange.

1. Full Edge: The hem runs from one corner to the other.

2. Symmetric: You pick a center point and the hem grows outward in both directions.

3. Two Sides: You can drag each end of the hem to a specific distance from the corners.

4. Two Offsets: You can reference other parts of your design to set the start and end points of the hem.

This flexibility is great for creating tabs or specific reinforced sections on a larger sheet of metal.

The New 180-Degree Bend Ability

Before this update, Fusion struggled with 180-degree bends in the sheet metal environment. Users had to stop at 179.9 degrees to prevent the software from throwing an error. This made technical drawings messy because the angles were never exactly 180 degrees.

Now, Fusion supports a full 180-degree bend. You can create a flange and rotate it all the way back until it is parallel with the first face. To make this work smoothly, ensure your height datum is set to tangent to bend. This prevents the flange from changing its height as you rotate it. This small change is a huge win for designers who need accurate flat patterns for manufacturing.

Changes to Sheet Metal Rules

Autodesk renamed some settings in the Sheet Metal Rules menu. In older versions, there was a setting called "miter/seam/gap width." This name was confusing for many users. It has been renamed to Minimum Gap.

The Minimum Gap setting controls the distance between miters and the spacing in your hems. If you want your parts to have very tight corners, you can edit your rule and change the minimum gap from "thickness" to "thickness divided by four." This will instantly update your model and make all your gaps tighter.

Verifying Designs with Unfold

A sheet metal part is only useful if it can be flattened for a laser or waterjet cutter. The new hem tool works perfectly with the Unfold command. Even with complicated double hems or rope hems on multiple edges, Fusion can calculate the flat pattern accurately. This ensures that your physical part will match your 3D model exactly once it is bent in a press brake.

Conclusion

The addition of the Hem command is a major improvement for Autodesk Fusion. It replaces slow workarounds with a fast, professional toolset. By offering six different hem styles and the ability to handle 180-degree bends, Fusion has become much more capable for serious sheet metal engineering.

These tools do more than just make the model look good. They provide accurate data for manufacturing and allow for better control over corner reliefs and material gaps. If you haven't tried the new Hem command yet, start by experimenting with the different styles and formulas to see how they can improve your next project.