The 
SheetMetal workbench (an external workbench available through the Addon Manager) has grown quite powerful and merits to be appropriately documented.
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:
- Collecting pictures
- Adding workflow descriptions
- Adding more detailed tutorials
- Create a profile (a line and a tangent arc), preferably using the
Sketcher Workbench. - Activate the
Make Base Wall command to create a BaseBend object. - Edit the BaseBend object's parameters:
- Set Mid Plane to
Trueto let the profile extend symmetrically to both sides of the sketch plane. - Set radius and thickness to values of your choice.
- Set Mid Plane to
- Create a cut-out contour with the Sketcher Workbench.
- Use the
PartDesign Pocket command to cut off one half of the Round bit. - Create a hole pattern with the Sketcher Workbench.
- Use the
PartDesign Hole command. Avoid the countersink and counterbore options to keep the body unfoldable. - Activate the
Unfold command to get an Unfold object. - Done!
- Create a profile, preferably using the Sketcher Workbench on the XZ plane.
- Activate the Make Base Wall command to create a BaseBend object.
- Edit the BaseBend object's parameters in the properties panel:
- Set Mid Plane to
Trueto let the profile extend symmetrically to both sides of the sketch plane. - Set length to 32 mm.
- Set radius to 2 mm.
- Set thickness to 0.3 mm.
- Set Mid Plane to
- Select the face between the round sections and activate the Sketcher Workbench.
- To hide the curled part use the
Sketcher View section command. - Create the cut-out contour.
- Finish the sketch using the
Sketcher Leave sketch command. - Select the face again and add the Cut-out sketch to the selection.
- Use the
Sketch on Sheet command to cut around the curled bit.
- One side is finished. We now need to find a way to mirror the body.
Potential mirror options:
- The
PartDesign Mirrored command fails because it cannot handle SheetMetal features for some reason. So that does not work. - The
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:
- Select the body from the tree view.
- Use the
PartDesign Clone command. It adds a new body containing a clone object.
To apply a 180° turn set the Angle 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).
- With the body still active, use the
PartDesign Boolean operation command to add the body of the clone and fuse both halves.
- Activate the Unfold command to get an Unfold object.
- Done!
Mirror using a link object:
- Select the body from the tree view.
- Use the
Make link command. This adds a new link object. - Duplicate the link object by setting the property Element Count to 2.
- To apply a 180° turn set the Angle 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).
- Select both sub-linked objects in the tree view.
- Activate the
Part Fuse command to fuse both halves.
- Activate the Unfold command to get an Unfold object.
- Done!
When a Corner Relief is added (right side) it can be necessary to adjust the value of the Size property.
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
(The pull relief is just an artistic expression of what could be hidden inside a real plug)
This section tries to explain the properties of each SheetMetal object with simple images, where applicable.
Selected sketch +
Make Base Wall
→ BaseBend object with default settings
Edit length: Default length → Reduced length
Switch Mid Plane from {{False to True: Extrusion in one direction → Symmetric extrusion}}
Switch Reverse from {{False to True: Default direction → Inverted direction}}
Select Bend Side: {{value|Outside (default) → {{value|Inside}} → {{value| Middle}}}}
Edit radius: Default radius → Enlarged radius.
This property is the inner radius of the bends created at the vertices where two edges in the sketch have a non-tangential transition.
Edit thickness: Default Thickness → Enlarged thickness
A Bend object consists of sets of one cylindrical bend and one planar strip each. Each pair extends from a selected edge of a blank.
Selected edges +
Make Wall
→ Bend objects with default settings
(Two Bend objects in two separate bodies.)
Edit radius to vary the inner radius of all bends supplied by a Bend object. (See BaseBend object above)
Edit length to vary the length of all planar strips extending from the bends of a Bend object.
: Don't confuse the length with a flange length which is the sum of this length, radius, and thickness (90° only).
Switch invert from {{FALSE to True:Default flanges (Bend objects) → Inverted flanges}}
Edit angle:Default angle (90°) → Enlarged angle → Decreased angle
We don't have to care about trimming the edges, because Auto Miter is activated by default. If deactivated, the result would look like this:
Switch Auto Miter from {{TRUE to False: Default angle (90°) → Enlarged angle → Decreased angle
(Auto Miter has no effect on single flanges)}}
To manually miter a flange edge miterangle1 and miterangle2 are used:
Edit miterangle1 and {{PropertyData|miterangle2: No miter (default) → Differently mitered edges, positive angle → Symmetrically mitered edges, negative angles}}
Mitering only effects the planar strips, not the bends.
: (It takes the whole edge into account and so cannot be used to chamfer flange edges)
To display the different choices of Bend Type we introduce an auxiliary cuboid that extrudes from the same outline as the blank and has the same height as the Bend object (its flange length).
Select Bend Type: {{value|Material Outside (default) → {{value|Material Inside}} → {{value|Thickness Outside}} → {{value|Offset}}}}
- Outside: The bend starts at the selected edge (The whole Bend object lies outside the cuboid).
- Inside: The outer side of the bend ends on the cuboid surface (The whole Bend object lies inside the cuboid).
- Thickness Outside: The inner side of the bend ends on the cuboid surface (only the planar strip is protruding from the cuboid surface).
- Offset: According to the value of offset the bend is moved in outward direction from its default position.
: An extension is inserted for positive values (high-lighted strip). : Negative values are allowed to move the bend inwards.
If we don't want to use the whole length of an edge we can use gap1 and gap2.
Edit gap1 and {{PropertyData|gap2: Default flanges → Flanges with different values for gap1 and gap2}}
If the length of a gap reaches or extends the value of min Relief Gap, a relief will be added to the gap. Reliefs are controlled by relief Type, reliefd (relief depth), and reliefw (relief width) which are enabled only when a gap value is set.
Edit reliefd and {{PropertyData|reliefw: Default values → Relief depth enlarged → Relief depth and width enlarged}}
Switch relief Type from {{value|Rectangle to {{value|Round}}: Default rectangular relief → Round relief}}
The round option will only be applied, if the relief depth is larger than the relief width.
Switch Use Relief Factor from False (default) to True to set the values of reliefd and reliefw automatically. Both are set to the object's (inherited) thickness multiplied by the value of Relief Factor.
: In this case the round option is useless, since the relief depth is as large as the relief width. (See above)
A new property Length Spec (v0.21) enables us to choose how to measure the length of the Bend object:
*Side view of four 120° flanges with default length (10 mm) and different **Length Spec* values: {{value|Leg** (default), {{value|Outer Sharp}}, {{value|Inner Sharp}}, {{value|Tangential}}}}
With the {{value|Tangential}} option selected the property length is the equivalent of the flange length.
{{value|Outer Sharp}}
and {{value|Tangential}} are identical for 90° angles.
An Extend object extends a sheet metal plate at one or more selected edge faces or edges.
Selected edge face and edges +
Extend Face
→ One Extend object with default settings.
A first issue occurs here: Although the property Refine is set to True two of the extensions still show their seam lines. Only the extension of the last selected element will be refined.
To refine all extensions they have to be created separately:
3x Selected edge face or edge +
Extend Face
→ Three Extend objects completely refined and with default settings.
Altered properties apply to all edges listed in the related base Object of the Extension object.
Edit length to adjust the length of the extension.
Edit gap1 and {{PropertyData|gap2 to reduce the width of the extension.
Left: Extension object with 3 edges. Right: One of the Extension objects with one single edge.}}
Link a sketch to the property Sketch to shape an extension. The properties length, gap1 and gap2 will be ignored once a sketch is linked. (This seems not to work with still unbent blanks).
A selected sketch lying on the flange to be extended → Resulting extension
It is plain to see that it doesn't matter which edge was selected for the Extend object, the shape of the flange is changed wherever sketch geometry protrudes, the new shape can even contain parts that are disconnected from the original flange. Multiple outlines are no problem, but the flange is not cut into.
This example shows that designers are responsible for their construction and shouldn't rely on the results of their tools, which do not make sense in this case. The Sketch attached to a flange face is problematic as well due to the toponaming problem, but for this a solution is in sight.
But there are better use cases for this tool involving almost closed shapes such as one of the examples on the SheetMetal Extrude page:
An almost closed profile → The added default extension is fused with the opposite side creating a closed profile (a tube) that is not unfoldable
Link a rectangular sketch to the property Sketch: Closed profile → Profile with rectangular extension, still fused
Switch Use Subtraction to {{true to provide a (hardly visible) default gap between the Extension object and the opposite side, then increase Offset to widen the gap:
Fused profile → Profile with interlocking extension, this final result is unfoldable}}
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