Cut and Bend

To create bending at sheet bodies SME: Cut and Bend operation is used:

Icon	Ribbon
	Sheet Metal → Cut and Bend
Keyboard	Textual Menu
<SME>	Operation > Sheet Metal > Cut and Bend

Only a certain part of the workpiece is folded when bending.

In this type of folding the base line should be a segment lying entirely within the base face limits. You can also set the base line by one of the side edges of the workpiece but in this case it is necessary to set the bending line displacement.


3D profile workpiece	Result of bending

A special kind of bending is bending by 3D profile. An unclosed 3D profile built at the workpiece face is used as a template for the bent lug. The base line is set by finite profile points.

3D profile workpiece

Bending by 3D profile

When bending by profile the base line always sets the start of bending area. In this case it is impossible to set bending line displacement and indents from base line edges.

Command parameters

Command parameters are general for sheet metal commands and are described in the corresponding subsection above.

The command automenu options are:

	<Ctrl+Enter>	Finish input
	<P>	Set entity Parameters
	<X>	Exit command
	<F5>	Preview Operation Result
	<L>	Select Line
	<E>	Select first Vertex or 3D Node
	<S>	Select second Vertex or 3D Node
	<W>	Draw Profile
	<R>	Select profile to bend
	<A>	Cancel Selection
	<D>	Change the part to be bend

Finish input. Builds a geometry according to the given parameters. In case there are not enough parameters set, the option is not available.

Set entity Parameters. Calls a standard dialog of 3D modeling command parameters.

Exit command. Shuts down the command with cancelling all the set parameters.

Preview Operation Result. Enables/disables the standard option of 3D modeling commands review.

Select Line. Selects a straight line determining the base bending line. The line can be set basing on the path, profile or the trace. The line should be a segment lying entirely within the face limits.

Select first Vertex or 3D Node. Chooses the first point determining the base bending line.

Select second Vertex or 3D Node. Chooses the second point determining the base bending line.

Draw Profile. Sets the base bending line or a profile in transparent mode. When choosing the option you should set the workpiece face (the system automatically switches to drawing at the selected work plane mode), after which you should create the profile outline at the selected face. The outline should be a segment lying within the workpiece face or an unclosed succession of lines also lying within the workpiece face. When exiting the drawing at the selected work plane mode the profile created will be selected automatically.

Cancel Selection. Cancels all the elements selected and clears the operand window.

Change the part to be bend. If the bending line is a straight line, there are two variants of bending, from two different sides. This option enables users to swap the bending side. In case of bending by profile the option is not available.

Creating the bend

A typical procedure when creating a bend is:

●To select an unclosed profile or a straight line lying within the workpiece face.

●To set general bending operations parameters.

●To change the bent part in case of a straight bending line if necessary.

●Finish entering.