Navigation:  Sheet Metal Operations > Creating a Base Part

To create a workpiece part, use the command SMC: Create new Base Part:

 

To create a workpiece, just select the source 3D profile in the model tree or in the 3D window. Profile selection activates automatically upon entering the command. This is indicated by the pushed automenu option:

To select a profile in the 3D window, point at one with the mouse. The pointed element will be pre-highlighted, and a tooltip next to the pointer will display its name. To select it, click .

The source profile will be selected automatically, if you call the command while drawing on the active workplane or from the context menu of an appropriate-type 3D profile.

The workpiece creation method (by the workpiece shape or by the workpiece cross-section shape) is defined in the command's properties window. The default method depends on the 3D profile selection. If a closed profile is selected, then the method of creating by the workpiece shape is set. If an open 3D profile is selected, the system activates the mode of creating the workpiece by the workpiece cross-section shape.

The workpiece creation method can be altered by setting the desired value in the parameter “Use 3D Profile as” (“Sheet Bound” or “Sheet Cross-section”).

The rest of the would-be workpiece parameters are also defined in the properties window. First of all, that is the workpiece thickness (the parameter “Thickness”) and the direction of extruding to the specified thickness (“Positive Direction”, “Reverse Direction” or “Symmetric”).

When creating the workpiece by the cross-section shape (“Use 3D Profile as| Sheet Cross-section”) the width of the workpiece sheet can be defined in the properties window (the parameter “Width”), as well as the rounding radius of the section corners (the parameter “Radius”). By default, the rounding radius is the value of the “Bend Radius” parameter in the command SMP: Sheet Metal Operation Defaults.

 

Initial workpiece for sheet metal operations

All sheet metal operations manipulate with the initial preformed workpiece. The workpiece can be a solid body of virtually any shape. A system requirement for defining various sheet metal operations is existence of two flat parallel faces in the area of deformation. One of such faces will be used as the base when defining the desired type of a sheet metal operation. Additionally, the side faces of the workpiece that will be subjected to deformation during bending must be perpendicular to the base face.

We recommend using a flat body as the sheet metal workpiece, with the side (end) faces perpendicular to main (top and bottom) faces. Such body can be created, for instance, by the extrusion operation or by the special command for creating a sheet metal workpiece.

The sheet metal workpiece creation operation is essentially an extrusion in the direction normal to a flat contour, to the specified depth. Use of this specialized operation instead of extrusion or other general-purpose operation simplifies workpiece creation, minimizing the number of parameters and settings to define.

The input data for creating a sheet workpiece are a flat closed 3D profile, the value of the desired thickness of the workpiece being created and the way (direction) of extruding the profile when creating the workpiece. We recommend using a single-contour 3D profile for defining the workpiece. However, if necessary, you can use a multi-contour profile satisfying the following conditions: the profile must have a single outer contour, and the inner contours without nesting.

         

The selected profile is extruded along the normal, to the specified depth equal to the width of the workpiece sheet metal. The extrusion is done in one of the three ways: upwards from the original profile, downwards from the original profile, or in both directions.

   

 

From now on throughout this chapter, any body subjected to a sheet metal operation will be referred to as "workpiece" regardless of the means of the body creation.