SheetMetal Forming

Description
The SheetMetal Forming command creates an embossed shape in a SheetMetal wall using a separate solid object.

The back side plane of the shape defining solid and the face to be embossed are used to position and orient the embossed shape, i.e. their local coordinate systems will have the same origin and the same orientation by default. The angle around the z-axis and offsets in x, y, and z direction may be altered by changing the parameter values in the properties window.

A sketch can be added to multiply and distribute the embossed shape in regular or irregular patterns (using the center points of circles or arcs)

A small selection of features that can be created:



Dimple

 * 1) Select the face of the SheetMetal object to be embossed
 * 2) Select the bottom face (back side) of the shape defining solid
 * 3) *Note: Don't forget the / key!
 * 4) Activate the [[Image:SheetMetal_Forming.svg|16px]] Make Forming in Wall command using:
 * 5) * button
 * 6) * drop down menu
 * 7) * keyboard shortcut: then

Louvre

 * 1) Select the face of the SheetMetal object to be embossed
 * 2) Select the bottom face (back side) of the shape defining solid
 * 3) Select a side face adjoined to the bottom face to mark the area to be cut open
 * 4) *Note: Don't forget the / key!
 * 5) Activate the [[Image:SheetMetal_Forming.svg|16px]] Make Forming in Wall command (see above)

Bridge

 * 1) Select the face of the SheetMetal object to be embossed
 * 2) Select the bottom face (back side) of the shape defining solid
 * 3) Select a side face adjoined to the bottom face to mark one area to be cut open
 * 4) Select the opposite face adjoined to the bottom face to mark the other area to be cut open
 * 5) *Note: Don't forget the / key!
 * 6) Activate the [[Image:SheetMetal_Forming.svg|16px]] Make Forming in Wall command (see above)

Drawn Cutout

 * 1) Select the face of the SheetMetal object to be embossed
 * 2) Select the bottom face (back side) of the shape defining solid
 * 3) Select the top face opposite the bottom face to mark the area to be cut open
 * 4) *Note: Don't forget the / key!
 * 5) Activate the [[Image:SheetMetal_Forming.svg|16px]] Make Forming in Wall command (see above)

Multiply and Pattern
To muliply and pattern the embossed feature a sketch containing circles and arcs can be added to the WallForming object's property.

The centerpoints of the circles or arcs are used to provide positions to put instances of the embossed feature; they don't influence the instances' orientation.

The orientation still depends on the orientation of the first selected face.

Adding Fillets

 * 1) Switch to the [[Image:Workbench_PartDesign.svg|16px]] PartDesign workbench
 * 2) Select an edge on the upper side of the SheetMetal object to receive a fillet
 * 3) Activate the [[Image:PartDesign_Fillet.svg|16px]] Fillet command using:
 * 4) * button
 * 5) * drop down menu
 * 6) Set the Fillet object's property  to . (It is quite important for the next fillet)
 * 7) Select an edge on the bottom side of the SheetMetal object to receive a fillet
 * 8) Activate the [[Image:PartDesign_Fillet.svg|16px]] Fillet command (see above)

Properties
See also: Property editor.

A SheetMetal WallForming object is derived from a Part Feature object and inherits all its properties. It also has the following additional properties:

Data

 * : Default value: (+ a sequential number for second and following items). The user editable name of this object, it may be any arbitrary UTF8 string.
 * : Base Feature. Link to the parent feature.


 * : "Suppress Forming Feature". Default value is.
 * : "Tool Position Angle". Default angle:.
 * : "Base Object". Link to the planar face to be embossed.
 * : "Offset from Center of Face". Default:.
 * : "Thickness of Sheetmetal". Thickness of the :.
 * : "Forming Tool Object". Link to the planar face used to position the Forming Tool


 * : "Point Sketch on Sheetmetal". Link to the sketch containing information how to multiply and distribute instances of the Forming Tool. (Center points of circles and arcs are used to create and position these instances)

Preparation
This bowl is made of a folded sheet metal object with a shape embossed, both have to be prepared in advance.

No need to work with coplanar sketches here.



Workflow

 * 1) Select the wall of the SheetMetal object to be embossed
 * 2) Select the back side of the shape defining solid (Don't forget the / key!) [[Image:SheetMetal_Forming-04.png|240px]]
 * 3) Press the  button or use the keyboard shortcut:  then  [[Image:SheetMetal_Forming-05.png|240px]]
 * 4) Fillet the sharp edges:
 * 5) * Flip the bowl and select one or more edges for the smaller inner radii
 * 6) * Press the button [[Image:SheetMetal_Forming-12.png|240px]]  -->  [[Image:SheetMetal_Forming-02.png|240px]]
 * 7) * Flip the bowl again and select one or more edges for the bigger outer radii
 * 8) * Press the button [[Image:SheetMetal_Forming-13.png|240px]]  -->  [[Image:SheetMetal_Forming-01.png|240px]]  Done!
 * 9) Alter orientation and position (should be done before filleting)
 * 10) * Activate the [[Image:SheetMetal_Forming.svg|16px]] WallForming object in the Tree view
 * 11) * Set the value of the property to e.g. 45° [[Image:SheetMetal_Forming-14.png|240px]]
 * 12) * Set the value of the property to e.g. greater than 0 [[Image:SheetMetal_Forming-06.png|240px]] Here it is plain to see that it doesn't make sense to move the embossed geometry outside the selected wall.
 * 13) * Setting the value of the property to e.g. greater than 0 isn't any better: [[Image:SheetMetal_Forming-07.png|240px]] At least the FreeCAD doesn't crash when a part has two bodies...
 * 14) Some hints
 * 15) The height of the defining solid determines the depth of the embossed shape. That means changing the parameter offset, z to alter the depth won't deliver expected results.
 * 16) The embossed geometry is made of a shell object i.e. it has a constant thickness. And so the defining solid has to be offsetable, otherwise the tool will fail to create the emboss.
 * 17) If the outer edges are filleted first it may rip the object into several pieces when the radii are set too large.