SheetMetal AddBase
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|
|
| Menu location |
|---|
| SheetMetal → Make Base Wall |
| Workbenches |
| SheetMetal |
| Default shortcut |
| C B |
| Introduced in version |
| - |
| See also |
| None |
Description[edit | edit source]
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[edit | edit source]
Profile[edit | edit source]
- Select an open contour
sketch.
- 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.
- Press the
- 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.
- Press the OK button to close the Task Panel and finish the command.
- Optionally adjust the profile parameters in the Property View.
Plate[edit | edit source]
- Select a closed outline
sketch.
- Invoke the command as described above.
- 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.
- Press the OK button to close the Task Panel and finish the command.
- Optionally adjust the plate parameters in the Property View.
Task Panel[edit | edit source]
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[edit | edit source]
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[edit | edit source]
Parameters
- DataBend Side (
Enumeration): "Bend Plane", defines on which side of a profile curve the thickness applies.Outside(default),Inside,Middle. (not used for plates) - DataBend Sketch (
Link): "Wall Sketch object". Link to the profile/outline sketch. - DataLength (
Length): Extrusion length of a profile. Default:100,00 mm. (not used for plates) - DataMid 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 iffalse(default) or symmetrically to both sides iftrue. - DataRadius (
Length): Inner radius of automatically added bends. Default:1,00 mm. (not used for plates) - DataReverse (
Bool): Reverses the direction of a profile extrusion or a plate thickness. Default:false. - DataThickness (
Length): Wall thickness of a sheetmetal profile or plate. Default:1,00 mm.
