Create a Hem in a Sheet Metal Face

Sheet metal hem features are typically added to provide one or more thicknesses of material along an edge of a face or flange.

A hem provides stiffness to a design, or provides a smooth, rounded external edge on a part to eliminate sharp edges.

You can create single, double, rolled, and teardrop hems.

1. On the ribbon, click Sheet Metal tab Create panel Hem .
2. In the Type drop-down list, click one of the following:
   • Single
   • Teardrop
   • Rolled
   • Double
3. In the Shape panel, click Select Edge and select an edge. If you want to flip the direction of the hem, click Flip Direction .
4. To specify how the width of the hem, click More, and then click one of the following options in the Width Extents drop-down list:
   • Edge. Creates the hem on the selected edge.
   • Width. Creates a hem of a specified width at a specified offset from a selected vertex, work point, work plane, or planar face on the edge of a face. You can also specify that the hem is a specific width, centered on the midpoint of the selected edge.
   • Offset. Creates a hem offset from two selected vertices, work points, work planes or planar faces on the edge of a face.
   • From/To. Starts and ends the hem from selected points or planar faces intersecting the selected edge.
5. (Optional) In the Gap drop-down list, use Measure, Show Dimensions, or Parameter List to obtain a value from the model.
   • Gap. For Single and Double hem types, specifies the distance between the inside faces of the hem.
   • Length. For Single and Double hem types, specifies the length of the hem.
   • Radius. For Rolled and Teardrop hem shapes, specifies the bend radius to apply at the bend.
   • Angle. For Rolled and Teardrop hem shapes, specifies the angle that is applied to the hem.