SheetMetal Examples/pl

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 (a line and a tangent arc), preferably using the [[Image:Workbench_Sketcher.svg|16px]] Sketcher Workbench.
 * 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 with 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 with 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.
 * 11) 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: [[Image:SheetMetal_Example-02f.png|200px|link=|BaseBend object and highlighted sketch]]
 * 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.
 * 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|x240px|link=|Cut-out contour]] [[Image:SheetMetal_Example-02i.png|x240px|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]]
 * 14) One side is finished. We now need to find a way to mirror the body.

Potential mirror options:
 * The [[Image:PartDesign_Mirrored.svg|16px]] PartDesign Mirrored command fails because it cannot handle SheetMetal features for some reason. So that does not work.
 * The [[Image:Part_Mirror.svg|16px]] Part Mirror command creates a mirrored part, but this is no longer unfoldable. So that does not work either.
 * One way that can work is to use a clone. This still can't be mirrored, but it can use axial symmetry (turn it 180°).
 * Another way that works is to use a link object.

Mirror using a clone:
 * 1) Select the body from the tree view.
 * 2) Use the [[Image:PartDesign_Clone.svg|16px]] PartDesign 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 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]]
 * 5) Done!

Mirror using a link object:
 * 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]]
 * 8) 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)