You can specify normal cuts or cuts across a bend. You can also project unfolded geometry in your sketch.
What's New: 2025
For convenience, you can also project the unfolded geometry in your sketch.
When creating a profile sketch to use for a cut feature that cuts across bends, it is useful to have unfolded geometry projected in your sketch. This command projects the flattened face along with bend lines, which you can use to dimension your sketch.
On the ribbon, click Sheet Metal tab Modify panel
Cut
.
In the property panel, for Input Geometry, the Profile selector is active and if there is only one profile it is automatically selected.
Next to the Profiles selector, click Cut Across Bend. The cut feature extrudes to the specified distance, Thickness is the default, and wraps across bends normal to the affected faces while maintaining the sketch geometry parameters. In the Flat Pattern, the cut matches the sketch profile.
Click OK or Apply if additional cut features are needed and the profiles are ready.
On the ribbon, click Sheet Metal tab Modify panel
Cut
.
In the property panel, for Input Geometry, the Profile selector is active and if there is only one profile it is automatically selected.
Next to the Profiles selector, click Cut Normal.
Under Behavior, choose the options needed to create the desired cut feature:
Distance. Establishes the depth of the cut. The default method creates a cut perpendicular to the sketch plane. To the right of the Distance field, click the method you want to use to define the distance. The cut feature result previews in red.
Specify a distance for the cut feature.
Through All: Extrudes the cut profile through all features and sketches in the specified direction.
To: Extrudes the cut profile to the selected face or work plane. (You can terminate the cut on a face that extends beyond the termination plane.) In an assembly, the face or plane can be on another part. Specify whether the cut extends beyond the selected face.
To Next: Selects the next possible face or plane on which to terminate the extrusion in the specified direction. Use this selector to pick a solid or surface on which to terminate the cut and determine the direction.
Other ways of specifying the distance are accessed from the selector flyout and include:
The Sketch plane specifies the direction. There are options to the sketch plane direction, these are:
. Flips the direction of the cut from the default setting. Useful when the cut sketch is created on a reference plane. When the sketch is created on a sheet metal face, results in no material removal.
. Removes material from the plane of the selected sketch towards the material thickness of the part. Default direction.
. Defines the cut sketch as the midplane of the cut thickness. Useful when the cut sketch is created on an appropriately positioned reference plane.
Click Profiles selector, if not already active, and then select one or more profiles.
To the right of the From selector, click Between and select the starting face for the cut feature. The Distance parameter updates to show Between is selected.
If not active, click the To selector and then select the face at which the cut feature will end.
Click OK to create the cut feature.