SheetMetal Workbench

Introduction
Sheet Metal is an external workbench and does not belong to the standard FreeCAD installation. It is developed to supply tools to create and unfold sheet metal objects.

Characteristics of sheet metal objects are:
 * - They have a constant thickness
 * - They are made of planar walls and cylindrical connections

The unfolding tool in both of its versions is not restricted to parts being made with tools of this workbench, but can handle Part and PartDesign objects as well, as long as they meet above characteristics.



If the export in DXF is used to control machines (Lasercut for example), you have to modify the DXF to remove the lines showing the folds, as these lines may be used for cutting by the machine.

Installation
This workbench can be installed from the Addon Manager. For manual installation see Installing more workbenches.

Tools
A detailed description of the tools can be found on the author's blog. (It's a bit outdated now, since some new tools have been added)


 * [[Image:SheetMetal_AddBase.svg|32px]] Make Base Wall: Creates a sheetmetal wall from a sketch.


 * [[Image:SheetMetal_AddWall.svg|32px]] Make Wall: Extends a wall from a side face of the metal sheet.


 * [[Image:SheetMetal_Extrude.svg|32px]] Extend Face: Extends a face along normal.


 * [[Image:SheetMetal_AddFoldWall.svg|32px]] Fold a Wall: Folds a face at the chosen line with specified bend radius.


 * [[Image:SheetMetal_Unfold.svg|32px]] Unfold: Flattens folded sheet metal object and generates a solid and a sketch (provides a window to set parameters).


 * [[Image:SheetMetal_UnattendedUnfold.svg|32px]] Unattended Unfold: Flattens folded sheet metal object and generates a solid and a sketch (if parameters have already been set).


 * [[Image:SheetMetal_AddCornerRelief.svg|32px]] Add Corner Relief: Adds corner relief to a corner.


 * [[Image:SheetMetal_AddRelief.svg|32px]] Make Relief: Adds relief to a corner.


 * [[Image:SheetMetal_AddJunction.svg|32px]] Make Junction: Creates gap in the corner of two walls.


 * [[Image:SheetMetal_AddBend.svg|32px]] Make Bend: Folds a face at the chosen line.


 * [[Image:SheetMetal_SketchOnSheet.svg|32px]] Sketch On Sheet metal: Cuts hole in sheetmetal based on a sketch.


 * [[Image:SheetMetal_Forming.svg|32px]] Make Forming in Wall: Creates forming tool.

Brief description
This workbench provides tools for the two main tasks:
 * Create sheet metal objects
 * Unfold sheet metal objects

This section is meant to give a rough idea of how to use the supplied tools. More detailed information can be found on each tool's own page (see above) or in the linked tutorials (see below).

Start with a profile

 * 1) Create an open polyline (preferably with the sketcher)
 * 2) Use the [[Image:SheetMetal_AddBase.svg|16px]] Make Base Wall command to create a sheet metal profile.

Start with a blank

 * 1) Create a closed polyline (preferably with the sketcher)
 * 2) Use the [[Image:SheetMetal_AddBase.svg|16px]] Make Base Wall command to create a sheet metal blank.

Start with a PartDesign Pad

 * 1) Create a closed polyline (preferably with the sketcher)
 * 2) Use the [[Image:PartDesign_Pad.svg|16px]] PartDesign Pad command to create a prismatic body.
 * 3) The [[Image:PartDesign_Thickness.svg|16px]] PartDesign Thickness command will make it an object of constant thickness.
 * 4) To make it unfoldable it needs some gaps or connections between the walls:
 * 5) The [[Image:SheetMetal_AddRelief.svg|16px]] Make Relief command will cut off selected corners.
 * 6) The [[Image:SheetMetal_AddJunction.svg|16px]] Make Junction command will create junctions with gaps between adjoining walls that need to be disjoined.
 * 7) The [[Image:SheetMetal_AddBend.svg|16px]] Make Bend command will create cylindrical connections for the remaining walls that need to stay joined.

Some parameters will be inherited from the parent object(s) but it is better to check the relevant parameters at each stage.

The resulting sheet metal object should now be checked if it can be unfolded. (see Unfold... below)

Adding more features
The unfoldable basic sheet metal objects can be extended:
 * 1) Use the [[Image:SheetMetal_Extrude.svg|16px]] Extend Face command to enlarge walls.
 * 2) The [[Image:SheetMetal_AddWall.svg|16px]] Make Wall command will add new walls to the existing object.
 * 3) Use the [[Image:SheetMetal_AddCornerRelief.svg|16px]] Add Corner Relief command to add or reshape corner reliefs.
 * 4) The [[Image:SheetMetal_AddFoldWall.svg|16px]] Fold a Wall command will fold a wall at a chosen line, i.e. it will trimm a wall at said line, relocate the cut away side, and rejoin them with a cylindrical connection.
 * 5) Use the [[Image:SheetMetal_SketchOnSheet.svg|16px]] Sketch on Sheet metal command to cut holes into the object starting on a chosen wall and then following the adjoined walls and connections.
 * 6) The [[Image:SheetMetal_Forming.svg|16px]] Make Forming in Wall command will stamp a shape into a wall.

Several tools of other workbenches could be used to add holes or to reshape edges.

Unfold a sheet metal object
To unfold a sheet metal object aktivate the Unfold or the  Unattended Unfold tool.

The result will be a 3D object with an optional outline sketch including bend lines.

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.
 * Frequent case of crash: take a lot of precautions not to cut in the hinges (the folds) either along the faces or in the angles nor to make holes or notches through the angles.

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

 * 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).



Repeat as many times as there are sides to bend.

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



Videos

 * The Elegant Sheet Metal Workbench by Joko Engineering

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
 * Files:
 * Reporting bugs/Request feartures: 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!