Forming Flange Unfolding

This command allows you to unfold a piece of part by an unfolding by unstamping simulation. The unfolding computation is realized from a mesh of one shape side, projected on a surface.

It automatizes the steps of part separation in two areas, creation of surface and mesh to unfold, unfold shape creation and finally union of this shape to the fixed side of the original shape.

Creation stages / Use:

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

Determine the side of the shape to be unfolded.
Create or select the projection surface.
Adjust the parameters of the mesh used for the unstamping simulation.
Validate .

This command is only available with the TopSolid'FormingSimulation licence.
This module use the technology of our partner:
FTI, Forming Technologies incorporated.

The simulation calculation requires information on the mechanical characteristics of the part material.
An example material library is available on TopSolid'Store: Unstamping Materials.

Available options:

Forming Flange Unfolding :

Shape to unfold: The shape to strip is selected by default.

Two unfolding modes are available:

Local: With this mode, one side of the shape will be considered as fixed, the other will be unfolded.
- Face on part to unfold: This face allows you to identify the shape side which will be unfolded. This face does not need to be connected to the boundary edges between the two sides of the part.
- Projection surface: This option allows you to select the surface onto the unfolding result will be projected. It is necessary to select a surface, even to unfold on a plane.
  It is also possible to create an Extension surface with the "special inputs" icon.
- Stamping direction: this option is necessary to simulate the unfolding accurately according to the forming process of the part.
- Boundary edges: Select the edges loop to separate the shape to be unfolded into two pieces. If the loop is not closed, red balls are used to identify its extremities. It is possible to imprint any missing edges with the "special inputs" icon.

For any selected edge, its opposite edge is automatically added to the selection if found.
The lateral edges are automatically selected if found.
The edges of the selected projection surface are automatically considered as boundary edges.

Global : With this mode, the whole shape to strip is unfolded.
- Face on side to consider : This face indicates the sheet metal part side which be unfolded.
- Projection surface: This option allows you to choose the surface where the unfolding result will be projected. It is necessary to select a surface, even when this one is a plane.
  It is also possible to create an Extension surface with the "special inputs" icon.
- Stamping direction: this option is necessary to accurately simulate the unfolding according to the forming process of the part.
- Constrained edges: To ensure a right positioning for the unfolding, select a set of edges staying fixed during the forming process of the part.

If the chosen Shape to unfold is a surface (and not a surface sheet metal), additional options allow you to take in account the part thickness:
- Thickness: It allows you to set the thickness value.
- and how this thickness is distributed around the surface:
- 1. - Normal
    - Middle surface
    - opposite

Mesh:

Two unfolding calculation modes are available, the choice of the mode slightly modifying the dimensions of the flattening:
Progressive die: In this mode the forming process is done without stripper.
Draw die: This mode considers that the part forming process will be done with a stripper.
Approximation tolerance and Maximum element size: These options allow you to adjust the sharpness of the mesh, according to the part to be unfolded. Several pairs of values are proposed by default and allow to adjust the mesh of the majority of the parts.
Fill holes: The mesh will be created without taking in account the holes on the part. This option is dedicated to the global unfolding mode.
Interpolated edges, Maximum sampling distance: By default, 7 points are distributed on each edge to unfold. These 7 points are then positioned according to the calculation of the unfolding, on the projection surface. They are used to create the forming unfolding sketch. In the case of parts containing long edges, it is possible to ensure a minimum distance between these points. If the distance becomes greater than the chosen value, the number of calculated points is increased.

Advanced options:

Hide tools: It is possible to hide or not the projection surface after the command execution.

The forming unfolding sketch can be hided or not.

Partial execution: This option is useful when the command fails. Since this is a sequence of geometric operations, it is possible that only some of the operations fail, and that this will cause the command to fail globally.
In the case of partial execution, the part is cut in half at the boundary edges, and the forming unfolding sketch is created, projected onto the projection surface.
It is then possible to modify this sketch if necessary with the command Replace trimming sketch.
Finally, use the Trim and Thicken command to create the flat shape and sew it to the fixed part.
Fixed part mesh: This option makes it possible to create the Part additional mesh which will be associated to the Unfolding mesh. It is then possible to visualize these two meshes by displaying the Analyze Simulations.

Points : Selected characteristic points on the part can be also computed together with the unfolded shape. It could be used to position key construction geometries.

Modifications / Additional information:

After editing the command in the operations tree, this is the forming unfolding building command which is edited. This command is included in the Forming Flange Unfolding operation.

Following commands are only proposed in contextual menu :
- Show/Hide Trimming Sketch: This command allows you to Show/hide the trimming sketch used to create the unfolded shape.
- Replace trimming sketch: The trimming sketch is produced by simulation. It is possible to sharpen/modify this result. Replace the sketch will produce a new 3D sketch, copied from the first one, and modifiable. Then, it will automatically replace the first sketch in the trimmed and thickened projection surface.
- Restore computed trimming sketch: This command is only available when the computed sketch has been replaced. It is possible to go back to the first computed sketch. The other one that was created by copy is not deleted.