1. Create a profile (a line and a tangent arc), preferably using the Sketcher Workbench.
2. Activate the Make Base Wall command to create a BaseBend object.
3. 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.
4. Create a cut-out contour with the Sketcher Workbench.
5. Use the PartDesign Pocket command to cut off one half of the Round bit.
6. Create a hole pattern with the Sketcher Workbench.
7. Use the PartDesign Hole command. Avoid the countersink and counterbore options to keep the body unfoldable.
8. Activate the Unfold command to get an Unfold object.
9. Done!

1. Create a profile, preferably using the Sketcher Workbench on the XZ plane.
2. Activate the Make Base Wall command to create a BaseBend object.
3. Edit the BaseBend object\'s parameters in the properties panel: - Set **Mid Plane** to `True`to 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.
4. Select the face between the round sections and activate the Sketcher Workbench.
5. To hide the curled part use the Sketcher View section command.
6. Create the cut-out contour.
7. Finish the sketch using the Sketcher Leave sketch command.
8. Select the face again and add the Cut-out sketch to the selection.
9. Use the Sketch on Sheet command to cut around the curled bit.
10. 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:

1. Select the body from the tree view.
2. 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).
3. With the body still active, use the PartDesign Boolean operation command to add the body of the clone and fuse both halves.
4. Activate the Unfold command to get an Unfold object.
5. Done!

Mirror using a link object:

1. Select the body from the tree view.
2. Use the Make link command. This adds a new link object.
3. Duplicate the link object by setting the property Element Count to 2.
4. 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).
5. Select both sub-linked objects in the tree view.
6. Activate the Part Fuse command to fuse both halves.
7. Activate the Unfold command to get an Unfold object.
8. Done!

*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:

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}}

A Fold object is the result of a sheet metal plate bent at a given line.

Change the property Position to control where the bend is positioned according to the bend line.

Cross-section of the bend: The bend line lies on the upper face of the blank (black) with a 10 mm offset from the edge, its position is maked with a pentagon. It also defines the virtual intersection of the blank and the bent wall