SheetMetal Examples

Introduction
The SheetMetal workbench has grown quite powerful now and it demands an appropriate documentation.

To avoid the overcrowding of the tool pages with examples this page was added to collect parts showing and explaining special SheetMetal features.

Planned phases to generate content:
 * 1) Collecting pictures
 * 2) Adding workflow descriptions
 * 3) Adding more detailed tutorials

Hinge Step by Step:

 * 1) Create a profile, preferably using the [[Image:Workbench_Sketcher.svg|16px]] Sketcher Workbench. (A line and a tangent arc)
 * 2) Activate the [[Image:SheetMetal_AddBase.svg|16px]] Make Base Wall command to create a BaseBend object.
 * 3) Edit the  BaseBend object's parameters:
 * 4) * Set to to let the profile extend symmetrically to both sides of the sketch plane.
 * 5) * Set and  to values of your choice.
 * 6) Create a cut-out contour, preferably using the [[Image:Workbench_Sketcher.svg|16px]] Sketcher Workbench.
 * 7) Use the [[Image:PartDesign_Pocket.svg|16px]] PartDesign Pocket command to cut off one half of the Round bit.
 * 8) Create a hole pattern, preferably using the [[Image:Workbench_Sketcher.svg|16px]] Sketcher Workbench.
 * 9) Use the [[Image:PartDesign_Hole.svg|16px]] PartDesign Hole command. Avoid the countersink and counterbore options to keep the body unfoldable.
 * 10) Activate the [[Image:SheetMetal_Unfold.svg|16px]] Unfold command to get an Unfold object.
 * Done!

Paper Clip Step by Step

 * 1) Create a profile, preferably using the [[Image:Workbench_Sketcher.svg|16px]] Sketcher Workbench on the XZ plane. [[Image:SheetMetal_Example-02e.png|300px|link=|Profile sketch]]
 * 2) Activate the [[Image:SheetMetal_AddBase.svg|16px]] Make Base Wall command to create a BaseBend object.
 * 3) Edit the  BaseBend object's parameters in the properties panel:
 * 4) * Set to to let the profile extend symmetrically to both sides of the sketch plane.
 * 5) * Set to 32 mm.
 * 6) * Set to 2 mm.
 * 7) * Set to 0.3 mm. [[Image:SheetMetal_Example-02f.png|200px|link=|BaseBend object and highlighted sketch]]
 * 8) Select the face between the round sections and activate the [[Image:Workbench_Sketcher.svg|16px]] Sketcher Workbench. [[Image:SheetMetal_Example-02g.png|200px|link=|Face to support the sketch]]
 * 9) To hide the curled part use the [[Image:Sketcher_ViewSection.svg|16px]] Sketche View section command.
 * 10) Create the cut-out contour. [[Image:SheetMetal_Example-02h.png|300px|link=|Cut-out contour]] [[Image:SheetMetal_Example-02i.png|200px|link=|Cut-out contour slightly touching the selected face]]
 * 11) Finish the sketch using the [[Image:Sketcher_LeaveSketch.svg|16px]] Sketcher Leave sketch command.
 * 12) Select the face again and add the Cut-out sketch to the selection. [[Image:SheetMetal_Example-02j.png|200px|link=|Face and sketch selected]]
 * 13) Use the [[Image:SheetMetal_SketchOnSheet.svg|16px]] Sketch on Sheet command to cut around the curled bit. [[Image:SheetMetal_Example-02b.png|200px|link=|Finished first half]]

Now one side is finished and we need to find a way to mirror the body.
 * The [[Image:PartDesign_Mirrored.svg|16px]] PartDesign Mirrored command fails, because it can mirror features but not bodies and SheetMetal features seem to be not valid in this case.
 * The [[Image:Part_Mirror.svg|16px]] Part Mirror command creates a mirrored part, but this is no longer unfoldable.
 * One way is to use clone. This still can't be mirrored, but it can use axial symmetry (turn it 180°).
 * Another way is to use link objects.

The flip a clone way:
 * 1) Select the body from the tree view
 * 2) Use the [[Image:PartDesign_Clone.svg|16px]] Create a clone command. It adds a new body containing a clone object. To apply a 180° turn set the  under the Placement property of either the body or the clone to 180°. (Z axis is default and should be fine if you started on the XZ plane as described) [[Image:SheetMetal_Example-02b.png|200px|link=|Cloned half]]  [[Image:Button_right.svg|16px|link=]] [[Image:SheetMetal_Example-02l.png|200px|link=|Flipped cloned half]]
 * 3) With the body still active, use the [[Image:PartDesign_Boolean.svg|16px]] PartDesign Boolean operation command to add the body of the clone and finally to fuse both halves. [[Image:SheetMetal_Example-02c.png|200px|link=|Fused halves]]
 * 4) Activate the [[Image:SheetMetal_Unfold.svg|16px]] Unfold command to get an Unfold object. [[Image:SheetMetal_Example-02m.png|200px|link=|Clip and Unfold object]]  [[Image:SheetMetal_Example-02d.png|200px|link=|Unfold object]]
 * Done!

The link objects way:
 * 1) Select the body from the tree view.
 * 2) Use the [[Image:Std_LinkMake.svg|16px]] Make link command. This adds a new link object.
 * 3) Duplicate the link object by setting the property  to 2.
 * 4) To apply a 180° turn set the  under the Placement property of either of the sub-linked objects to 180°. (Z axis is default and should be fine if you started on the XZ plane as described)
 * 5) Select both sub-linked objects in the tree view.
 * 6) Activate the [[Image:Part_Fuse.svg|16px]] Part Fuse command to fuse both halves. [[Image:SheetMetal_Example-02c.png|200px|link=|Fused halves]]
 * 7) Activate the [[Image:SheetMetal_Unfold.svg|16px]] Unfold command to get an Unfold object. [[Image:SheetMetal_Example-02m.png|200px|link=|Clip and Unfold object]]  [[Image:SheetMetal_Example-02d.png|200px|link=|Unfold object]]
 * Done!

Hex Bowl




When a Corner Relief is added (right side) it can be necessary to adjust the value of the Size property.

Extend Face Example


For the second use of Extend Face a Sketch with two contours is used for shape of the extension(s); and with the value of "use subtraction" set to true it provides the shape for the cut-outs, as well

USB shield contact


(The pull relief is just an artistic expression of what could be hidden inside a real plug)