Creating Part

To create a workpiece, use the command SMD:  Create Part:

 

 

The operation allows you to create a sheet workpiece in two ways.

●Sheet Bound

●Sheet Cross-section

Both methods use a flat 3D profile as the source.

All sheet metal operations are created on the basis of a previously created workpiece. The workpiece can be a solid body or imported body of virtually any shape. A system requirement for defining various sheet metal operations is the 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. We recommend using a flat body as the sheet metal workpiece, with the side (end) faces perpendicular to main (top and bottom) faces.

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.

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 body creation.

 

Command Parameters

Command parameters related to general ones are described in the corresponding section above.

Select the way of creation.

Thickness. Input field for sheet thickness in millimeters.

A variant of the direction of extrusion to a given thickness.

Width. The parameter sets the width of the workpiece if created using the Sheet Cross-section option.

Automenu Options.

Finish input. The option allows to build geometry by given parameters. If there are not enough parameters, the option is inactive.

Set entity Parameters. Invokes the standard dialog of the parameters of the 3D modeling command.

Exit command. The option closes the command with the cancellation of the specified parameters.

Preview Operation Result. The option enables/disables the standard option to view 3D modeling results.

Select 3D Profile. The option allows to select the profile according to which the workpiece will be built. The option is mandatory to create a workpiece.

Draw Profile. The option allows to create a workpiece using profile. The option allows you to switch to drawing mode on the selected work plane to create the original profile. In this case, when you exit the drawing mode on the workplane, the created profile will be automatically selected.

 

Creating a Base Part

To create a workpiece, just specify the source 3D profile. When entering the operation, the 3D profile selection mode is activated automatically. The type of the selected profile will determine the option to create a workpiece. If the contour is closed, then the option of creating according to the shape of the sheet will be automatically selected. If the contour is not closed, then the option for the sheet cross-section will be selected. Indicate the necessary parameters and complete the entry.

Sheet Bound. The initial 3D profile defines the contour of the future workpiece body. We recommend using a single-contour 3D profile. However, it is allowed to use a multi-contour profile, which meets the following requirements: A 3D profile should consist of only one wraparound contour and the nested contours should be the first level.                  

When you select this way of the sheet workpiece creation you should specify the width of the workpiece and direction of the profile extrusion. The selected profile is extruded by normal to the specified thickness of the workpiece sheet. Extrusion is done in one of three ways: upward relative to the plane of the source profile, downward relative to the plane of the profile or in both directions symmetrically.

Sheet Cross-section. The 3D profile determines the sectional shape of the workpiece body. In this case, only a flat single-contour 3D profile can be used. It can be closed (which will result in a “pipe”-type workpiece), or open. If you select a closed profile, you should manually change the type of the workpiece.

As in the previous case, extrusion by the sheet thickness can be done in three ways relative to the surface resulting from the first extrusion. The edges of the resulting sheet body (the corners of the workpiece cross-section) are automatically rounded. The width of the workpiece (extrusion value) is determined by the Width parameter.