SheetMetal Workbench/de

Überblick
Sheet Metal ist ein Zusatz Arbeitsbereich zum Entwerfen und Abwickeln von Blechteilen. Es ist nicht Bestandteil der Standardinstallation von FreeCAD.


 * SheetMetal Example.png''Im Bild oben: das Blech Modell, das mit dem Sheet Metal Arbeitsbereich (hinten) erzeugt wurde; davor der entfaltete Volumenkörper; Im Vordergrund die Abwicklungsskizze mit Biegelinien für den Export nach DXF.

Warnung: Wenn die Export nach DXF zur Steuerung von Maschinen verwendet wird (z. B. Lasercut), muss die DXF angepasst werden, um die Linien, die die Falten darstellen, zu entfernen, die die Maschine diese ansonsten als Schnittkanten annimmt.

Installation
Dieser Arbeitsbereich kann einfach über den Addon Manager installiert und aktualisiert werden, der in FreeCAD 0.17 und höher verfügbar ist. Informationen für Benutzer von FreeCAD 0.16 und andere Installationsmethoden finden Sie unter Installing_additional_contents.

Werkzeuge
Eine dataillierte Beschreibung der Werkzeuge kann unter on the author's blog gefunden werden.


 * [[Image:SheetMetal_Bend.svg|32px]] Bend: extends a wall from a side face of the metal sheet. Properties can be edited in the Data tab:
 * : Bend angle.
 * : Extends the wall on the left side.
 * : Extends the wall on the right side.
 * : Gap from the left side.
 * : Gap from the right side.
 * : Invert bend direction.
 * : Length of the wall.
 * : Bend miter angle on the left side.
 * : Bend miter angle on the right side.
 * : Bend radius.
 * : Rectangle or Round. Enabled only when a gap value is set.
 * : Relief depth. Enabled only when a gap value is set.
 * : Relief width. Enabled only when a gap value is set.
 * : K factor (also known as neutral factor) for the bend. Used to calculate bend allowance when unfolding.
 * : False (default) or True. If true, unfolds the bend.
 * [[Image:SheetMetal_Extrude.svg|32px]] Extrude: extends a face along normal. Properties can be edited in the Data tab:
 * : Gap from the left side.
 * : Gap from the right side.
 * : Length of the wall.
 * [[Image:SheetMetal_Unfold.svg|32px]] Unfold: flattens folded sheet metal object and generates a solid and a sketch. The Unfold objects are not parametrically linked to the model; if edits are made to the model, the Unfold operation needs to be redone.

Basic Usage
The work flow is pretty simple: start with a base plate or sheet, select a thin face representing the thickness of the metal sheet, and click on the Bend tool to add a bend, or on the  Extrude tool to extend the face.

The workbench does not have a tool to create a base plate, so you need to start your model with one of those methods: If you start with a PartDesign Body, you can mix Sheet Metal features with PartDesign features such as pockets or  holes.
 * A Part_Box.png Part Cube
 * An extruded solid made with Part Extrude.png Part Extrude from a Draft Rectangle.png Draft Rectangle, Draft Wire.png Draft Wire or a Sketcher NewSketch.png Sketch
 * A PartDesign Body.png PartDesign Body containing an PartDesign AdditiveBox.png additive box or a PartDesign Pad.png PartDesign Pad made from a Sketch.

To unfold a sheet metal part, select a planar face and click on the Unfold icon.

Limitations

 * The workbench is affected by the topological naming issue that is inherent to FreeCAD. If an edit of a bend earlier in the history of the part renumbers the faces, then the following bends may be affected and switch faces. If the bend features do not break, you can double-click on it to get a dialog where you can select the proper face in the 3D view, and update the Bend.
 * The Unfold tool has some limitations, and will fail in certain complex situations. When it fails, try to select a different face.

Sheet Metal Tutorial by meme2704
The following tutorial is reproduced from the PDF tutorial mentioned in Links.

Presentation of the workbench
After downloading the extension and install, open it.

1st operation

 * Get the base: use either the workbenches "part" or "draft", make 1 sketch that will contain all holes and any cuts, extrude this base to the thickness of the sheet.
 * Bear in mind that the edges will always be in addition as well as the folding radii.

2nd operation
Repeat as many times as there are sides to bend.
 * Open the Sheet_metal workbench.
 * Select 1 thickness of the edge (edge) of the base plate and click on the "bend" tool 90° default bend angle can be changed from 0 to 90°.
 * Edge height is 10mm by default, editable from 0.1 to xxxmm.
 * Bending radius is by default equal to thickness, editable from 0.1 to xxmm (never put 0).
 * Gap1, gap2 is the withdrawal of the folded edge from the corner of the base (0 accept).
 * Invert default: false folds to Z +, true to ZReliefd cuts the corner between the fold and the base (inactive if gap = 0).
 * Reliefw adds 1 slot between the crop and the edge (inactive if reliefd = 0).

Folding 1 return with use of "extend".

To add 1 back repeat the same operation by selecting the thickness of the concerned edge.

To reduce the space between the 2 edges, use "extends".

Select the thickness and specify the length to add.

Note that if the extension of the 1st edge is made before the fold of the return, it will not be taken into account, if 1 identical fold is added to the extension, it will appear correct but the unfolding will not be done.

Folding of 1 2nd edge:

Now we must separate the 2 edges otherwise they will merge and unfolding will be impossible.


 * 1st method: make 1 withdrawal of 1 edge.
 * Give 1 value slightly greater than gap1 (or gap2), at zero there is still fusion.
 * 2nd method make 1 cut at 45 ° see further, use this tool.

Unfolding
Choose 1 reference face (here the orange face) and click on the button in the toolbar.

We obtain the blue part of which it is enough to modify the values X, Y, or Z to see it in totality.



Cut the flaps at 45°
After folding the flaps without having made a withdrawal, the shape thus appears. To do it must split at 45 ° (or following the bisector flaps are unequal width).


 * Create 1 new skit related to the common part of the 2 flaps.
 * Create 1 linked stop by selecting the outer edge of the "hinge".
 * Draw 1 triangle whose top is constrained at the end, oriented 1 side at 45 °, give the small side 1 minimum width (0.1mm is enough), and make 1 pocket.

Be careful not to scratch the "hinge" where the nakedness of bound the tip of the triangle at the edge of the fold line. Unfolding

Piercing edges and flaps
Make these holes and cuts after folding and before unfolding.

Always take care not to "scratch" the fold lines.



Make wired flaps
Make 1 fold on the edge of the side, at 45 ° of 0.1mm long, then 1 other reverse at 45 ° of the length of the contiguous flap, then extend the opposite side, it will pass over and they will not be merged.



Special case of this same pierced edge
In this particular case, unfolding only works by choosing the yellow face as a reference.



Special case hole straddling the folds
Previously it is said several times that it is not necessary to cut the folding lines.

How to do ?


 * Make the base with its half-round hole and make the 2 half-sided and the 2 half-folds separately.
 * Then make 1 extension on 1 of the sides of the width of the opening minus 0.1mm, the 2 edges thus remain separated.
 * Then on this extension (in green) draw the contour of the cut and make 1 pocket
 * The result is the red piece above, and the unfolding works, stays the line that separated the 2 edges previously

Links

 * Macro_Sheet_Metal_Unfolder, the original macro the Unfold tool is based on.
 * Sheet Metal Workbench announcement on the FreeCAD Forum
 * An English and French tutorial in PDF format on the FreeCAD forum
 * Videos:
 * Files:
 * Reporting bugs: https://github.com/shaise/FreeCAD_SheetMetal/issues

External workbenches
FreeCAD workbenches are easy to program in Python, there are therefore many people developing additional workbenches outside of the FreeCAD main developers.

The external workbenches page has some information and tutorials on some of them, and the FreeCAD Addons project aims at gathering them and making them easily installable from within FreeCAD.

New workbenches are in development, stay tuned!