BricsCAD offers bidirectional associativity between 3D Sheet Metal part and its flattened appearance. In this mode both representations exist in separate documents: Original part is stored in its native document and the Flattened part is stored in temporary document. Associativity is temporary and exists while both documents are opened. In order to work in associativity mode in next BricsCAD session or once the document were closed, one should repeat steps again.
What Does Associativity Mean?
Associative Unfolded allows you to the make cuts on flattened geometry and propagate the changes back to the 3D model. This helps simplify two scenarios:
Creating complex, non-standard Bends and Corner Relief cuts.
Avoid self-intersections in unfolding.
In these two scenarios both are easy to do in 2D rather than in 3D. In flattened mode Sheet Metal part is represented as set of separate flat solids (per-feature). Use the SmDelete command to delete solid flanges and bends on flat patterns.
Associativity is bidirectional - changes can be propagated from flattened parts back to 3D models and vice versa. Changes made on one of representations are propagated to the document with other representation once it becomes active.
Switching to Associativity Mode
The associativity mode is turned on using the SmUnfold command. Make sure there are no faces selected.
From Sheet Metal section of the Ribbon select Associatively Unfold Body icon and select Flange face.
Application will compute flattening of the given part and switch it to associative mode. Condition of success of given operation is the same as for regular unfolding.Continue working in associativity mode only if no errors or warnings appeared during the operation. A new temporary document containing the flattened part will be created.
Note: there is no need to save this document, it’s used to propagate editing operations from the flattened solid back to the 3D model.
Use Vertical Tile to view both the 3D model and associative unfolding documents.
Note: In the Mechanical Browser when flattened geometry is selected, it lists features are disabled.
Editing the Geometry
Working with flattened design document, draw a circle in the corner
Apply DmExtrude command to the circle, cutting the volume.
Click on original document again to make it active.
Model will be updated and the custom corner relief appears. Application writes to command line: Changes were successfully transferred to source model
Avoiding Collisions in Flat Pattern
Another useful application of associative unfolding is fixing the so not obvious material collisions.
In this example, we don’t know what changes to apply to the 3D model to avoid the collision when flattened. Let’s rework the model with using Associative Unfolding.
From Sheet Metal section of the Ribbon select Associatively Unfold Body icon , select Flange face, unfold and click Vertical Tile button on Toolbar or Ribbon to tile the opened documents vertically and zoom to the collision area.
Select boundary circular edge and offset it by 1.
Draw extra straight lines adjacent to the edge and join them.
DmExtrude the polyline on both sides.
DmThicken the surface by a bigger value.
Subtract thickened body from unfolded pattern.
Erase the leftover pieces.
Switch back to the document with the 3D model.
Make sure the that changes have been propagated.
Changes were successfully transferred to source model.
Zoom to the corner that updated.
To test the 2D unfold, export the file as a .dxf.