Unfolding

This command launches the unfolding of a sheet.

Creation stages / Use:

Click the Unfolding icon or select the Unfolding > Unfolding... command from the drop-down menu.

Check Predefined positioning it has been defined in the sheet metal part.
Select the reference face for the unbending.
Select if the unfolding is put on or tuned over:

This option allows to turn the unfolding result to 180° around the X axis of the destination frame. All bends will be reversed (upward bends become downward bends and vice versa) and also the bend angles signs

The Put on mode corresponds to an usual use:

The origin face is put on the destination plane of the frame. It gives the bend direction.

The Turned over mode allows to reverse the sheet metal regarding the selected origin face. The bend direction is inverted, otherwise we will obtain a symmetrical sheet metal of the reference sheet metal.

Two positioning of the unfolding are available:

Position origin to select the origin point and the direction of the unfolding.
or Orient along longest length: if this option is enabled, an automatic rotation will be applied to the unfolding so that the longest length of its (minimum) bounding box is oriented along the X axis of the destination frame.

Enter the rotation angle if needed..
Select the unfolding destination frame. In this case, the center of the reference face is positioned on the XY plane of the selected frame and on its origin or check the In place unfolding option to position it on the selected face.
Select the unfolding style to use.
Validate the creation of the unfolding with the button.

You can also force the positioning of the unfolding by checking the Position at origin box then by indicating a point in one direction, the selected point will be positioned at the origin of the selected frame and the selected direction will be merged with the X axis of the selected frame. This stage is essential when the reference face is cylindrical.

If you wish to take into account certain faces for unbending, they need to be defined as lateral faces using the Face side command.
When the origin face of the unfolding is cylindric or developable, there is no need to use the Origin point option. The unfolding is automatically positioned at the center of the selected face (or on the boundary).

The imprinted segments can be displayed on the unfolding. They can be on plane faces, on bend, on unfolded faces. They can be in contact with borders or cut-outs or cut a part "in two parts". It is recommended to imprint them on the both sides. If not, regarding the chosen plane face, the imprinted segments will be displayed or not.

Available Options:

Unfolding with thickness:

If you're a user of the TopSolid'SheetMetal's machining module, you need to be able to work on a 3D shape so that you can manage the local deformations, the drillings/tappings, but also the chamfered parts.

By thickening: This mode will simply thicken the unfolding sketch. The imprint curves are also imprinted on one side of the sheet metal part.
By unfolding: This mode will unfold the bends, unroll the developable surfaces, and manage the extensions of the unfolding and the forming flanges. The drillings and local deformations are retained.

Favour the By thickness mode as it guarantees the conformity of edge geometries between the unfolding sketch and the unfolding shape.

The By unfolding mode must be used if you want to keep fillets, chamfers or slots on bends, drillings, spots facing and local deformations.

Example of unfolding with thickness by unfolding with deformation, drillings and chamfers.

Bends:

Representation:

This option selects the type of representation of the bend lines:
	Center	The center line of the bend is represented on the unfolding.
	Boundaries	These extremities of the bend are represented on the unfolding.
	Both	These extremities and the center line of the bend are represented on the unfolding.
	None	The bend lines are not represented on the unfolding.

Geometry:

This option selects the type of geometry of the bend lines:
	Complete line	A complete line represents the bend lines.
	Extremities of lines	The bends are represented by extremities of lines ( the length is defined below).
	Line without extremities	The bend line stops before the sheet metal boundary ( the length is defined below).

Extremities length:

When the geometry is not Complete line, enter the extremities length of the bend line.

Notches:

This option allow to choose the notches type to be applied on the extremities of the bend line
	None	There is no notch to apply.
	Rectangle	The notch will be rectangular.
	oblong	The notch will be an oblong.

Notches length / width:

If there is a notch, enter the its length and width.

Bend Note:

See the Bend Note command for details.

Bounding box:

This option allows to add the minimal or the aligned bounding unfolding:
	None	The bounding box is not displayed.
	Minimal	The minimal bounding box is displayed.
	Aligned	The bounding box is aligned with the frame and is displayed.

Attributes:

For each kind of element of the unfolding, you change its color, its kind of line and its thickness. The color can be removed by clicking the button .
It is possible to assign a specific layer for each kind of geometries provided by the unfolding sketch. So boundaries to cut can be isolate on a layer, and bend lines on another.

Formings:

This section allows to treat areas which are not strictly unbendable. Check the "Formings treatment" option.

Ignore: Formings are not managed. It is useful to predefining a template.
Border forming flanges: They are areas created with a swept flange on a continue edges path and non linear.

(In this part case, a local lost on the big cylindric face has to be added to consider it as a bend.)

The approximation tolerance is used to polygonized the boundary of the forming area. Sections are then extended from this boundary to report their lengths on the unfolding.

The options section for formings can be set in the unfolding style.
The forming boundary color can be set in the Attributes section. It is indicated by "Other formings".

Global : This mode creates a global "unstamping" unfolding by using the en FTI (Forming Technologies Incorporated) calculation module. It is useful for the treatment of unbendable or undevelopable parts.

The calculation uses a mesh of the sheet metal surface. The approximation tolerance is used to polygonize edges as near as possible.

The maximum element size is the maximum size of a mesh triangle.

Predefined values are proposed (in green) in the two drop-down lists.
These values are quiet corresponding to "very thin", "thin", "medium" or "large" meshes. When one of these values is selected from one of the list, the value of the complementary field is automatically adjusted.
As first approximation, the medium mode is recommended. It is not recommended to enter too small or to high values.

The Filled holes option allows to use the part without holes to calculate.

Stamping direction: if it is not filled, it is automatically calculated by taking the normal direction of the selected face. If it is filled, this selected direction is taken into account.

It is recommended to avoid undercuts.
The origin face should not specially be plane if this calculation mode is activated.
The simulation calculation requires information on the mechanical characteristics of the part material.
An example material library is available on TopSolid'Store: Unstamping Materials.

With this calculation mode, only external and internal boundaries are displayed. Bends or imprints are not.
The Global option needs a specific license to be able to use FTI.

Advanced options:

Dressing:
Tapping / Facing and csinking: It is possible to automatically dress tapped holes, faced and csinked holes on the unfolding.

By default, tapping symbols are extracted, but facing and ccsinking symbols are not. When these symbols are extracted, their geometry is created in an complementary sketch of the unfolding main sketch.
They have specific attributes, which can be set in the unfolding or in the style.
Downward facings and tappings are with full line (they are shown from top view), and upward ones are with dotted lines (they are hidden from top view).
The goal is to have clearly defined symbols for TopSolid'PunchCut which uses groups of curves to automatically select tools.
Simplification:
- Extract corners relief: Corners relief are not displayed on the unfolding.
- Simplify corners relief: Corners relief will be simplified to keep constant dimensions on the unfolding without regarding the used loss at bends.
- Extract spot facings and counter sinkings: Drillings with spot facings or counter sinkings are automatically represented on the unfolding by their smallest diameter (when this option is checked).Cylindrical and conical faces have to be coaxial.

If the hole contains some cylindrical faces, TopSolid will take as hole diameter on the unfolding, the diameter of the smallest cylindrical face (and also if the hole contains conical faces with smallest diameters).

If the hole contains only conical faces,TopSolid will keep as diameter, the smallest diameter of cones.

TopSolid only considers through all drillings crossing the sheet metal on the side where the origin face is selected for the unfolding.

TopSolid only considers edges "strictly" circular, which excluded tilted drillings regarding the thickness direction.

Example:

It manages geometries done by TopSolid drilling operations, but also all other kind of origin (file import, boolean operations, ...)

- - Extract torn bends: This option allows to remove torn bends (bend without notches which rips the sheet metal) in the unfolding.
  - Arcs lines conversion: This option allows to transform to arcs and lines complex curves like ellipses, splines,... to allow certain machining software to read our unfolding exports.
  - Linear Tolerance: It indicates the maximum gap value authorized with simplified curves.
  - Angular tolerance: It indicates the maximum angle value authorized at the angle of tangency between two successive segments.
  - Large radius poligonization: This option, when it is checked, allows to replace by a polygon, arcs whose radius is larger than the given value, to avoid errors of punch or cut machining NC.
- Unfolding rules:
- - Use preferred tool for radii not listed in tables: When this option is selected and none of the tools defined in the table match the unbending radius, TopSolid uses the first preferred tool that is declared for the part thickness.
  - Ignore local unbending processes: Some local unbending can be added to the bend with the Unbending process command of the unfolding document. These processes can be ignored.
- Invalidity cases:
- - Presence of complex formings: By checking this option, the presence of formings or other complex deformations will make the document invalid.
  - Presence of quasi developpable faces: Remember what is a quasi developpable surface.
  - Open external profile: Allows to make invalid the unfolding if the external profile is open.

In general, it happens when the part has very small segments. Very often, the use of a smaller calculation tolerance allows to solve this problem.

The error indicates the smallest detected segment.

This option is activated by default for new unfolding documents created without template. It can be set in the unfolding style.

Modifications / Additional information:

This command generates a sketch representing the unfolding of the part. The content of this sketch cannot be modified but sketch operations may be applied.
The unfolding operation becomes invalid if it produces an empty unfolding sketch.
A memory limitation of the software does not allow to unfold parts with more than 100 consecutive bends. For parts exceeding this bend limit, a message warns the user, suggesting to try to change the original facein order to balance the unfolding tree

The unfolding command allows to treat multi-bodies parts. These multi-bodies are created with the Bodies mode of the Removing command. Its Keep bodies option allows to separate a multi-bodies shape in several distinct shapes.

It is the selected origin face which select the shape to treat. The origin face can be predefined in the part document by using the Unfolding positioning command.

Generally, sheet metal to consider must be defined in the detailed and design representations of the part document.

The inclusion in the unfolding document allows to select the representation and the shape to consider.

However, from the PDM point of view, the fact to have a part document with several shapes in not relevant. The best way is to use the Tools > Derivations > Partial parts... command to isolate each shapes of the detailed representation in distinct documents. These part documents are automatically included in an assembly document.