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Description

The SheetMetal AddBase command creates a SheetMetal base object from a sketch.

From an open contour it creates a prismatic profile:

From a closed outline it creates a base plate (blank):

Usage

Profile

1. Select an open contour sketch.
2. There are several ways to invoke the command:
   • Press the Make Base Wall button.
   • Select the Sheet Metal → Make Base Wall option from the menu.
   • Right-click in the Tree View or the 3D View and select the Sheet Metal → Make Base Wall option from the context menu.
   • Use the keyboard shortcut: C then B.
3. A BaseBend object is created, corners along the contour are automatically converted into cylindrical bends, and the Sketched base shape properties Task Panel opens:
   • Optionally press the Sketch button and select a different sketch.
   • Adjust the profile parameters in the Task Panel.
4. Press the OK button to close the Task Panel and finish the command.
5. Optionally adjust the profile parameters in the Property View.

Plate

1. Select a closed outline sketch.
2. Invoke the command as described above.
3. A BaseBend object is created and the Generate Sheet Metal base shape Task Panel opens:
   • Optionally press the Sketch button and select a different sketch.
   • Adjust the plate parameters in the Task Panel.
4. Press the OK button to close the Task Panel and finish the command.
5. Optionally adjust the plate parameters in the Property View.

Task Panel

A task panel was introduced in version 0.6.01

Double-click an existing BaseBend object in the Tree View to re-open the task panel and edit the parameters.

• Sketch: Links a different Sketch to the Bend Sketch property.
• Bend Plane: Sets the Bend Side property.
• Radius: Sets the Radius property.
• Thickness: Sets the Thickness property.
• Length: Sets the Length property.
• Symmetric: Toggles the Mid Plane property.
• Reverse Direction: Toggles the Reverse property. (hidden if Symmetric is checked)

The last entered values for Radius and Thickness will be saved as default values for the following new BaseBend object.

Properties

See also: Property View.

A SheetMetal BaseBend object is derived from a Part Feature object or, if it is inside a PartDesign Body, from a PartDesign Feature object, and inherits all its properties. It also has the following additional properties:

Data

Parameters

• DatiBend Side (Enumeration): "Bend Plane", defines on which side of a profile curve the thickness applies. Outside (default), Inside, Middle. (not used for plates)
• DatiBend Sketch (Link): "Wall Sketch object". Link to the profile/outline sketch.
• DatiLength (Length): Extrusion length of a profile. Default: 100,00 mm. (not used for plates)
• DatiMid Plane (Bool): "Extrude Symmetric to Plane". The length of a profile or the thickness of a plate extends to one side of the sketch plane if false (default) or symmetrically to both sides if true.
• DatiRadius (Length): Inner radius of automatically added bends. Default: 1,00 mm. (not used for plates)
• DatiReverse (Bool): Reverses the direction of a profile extrusion or a plate thickness. Default: false.
• DatiThickness (Length): Wall thickness of a sheetmetal profile or plate. Default: 1,00 mm.