How to Work with Form and Bead Features in BricsCAD Mechanical

Quick answer: Form and bead features are both created by a forming tool; bead features specifically come from imprinting a wheel that rolls over the flange along an arbitrary trajectory. This article uses “form” to refer to both form and bead features collectively. Form features can be recognized in imported geometry or inserted from built-in or user-defined libraries, and edited either directly or parametrically. They list in the Mechanical Browser along with their parameters, also viewable and editable in the Properties panel once selected.

Commands for Form Features

A library of parametrized sheet metal form features is available from the Form Features tab of the Tool Palettes panel, covering the most commonly used types; drag a feature’s icon from there, or from the Library panel, onto a flange to insert it. SMDEFAULTFORMFEATUREUNFOLDMODE controls how form features appear in 2D and 3D unfolded model representations.

Inserting a Form Feature

Make sure Dynamic Dimensions (DYN) and Dynamic UCS (DUCS) are active first.

1. Launch BMINSERT via the Form Feature tool button on the Sheet Metal toolbar or ribbon bar, Insert Form Feature in the Sheet Metal menu, the command itself, or by selecting a form feature directly from the Form Features tab of the Library or Tool Palettes panel. Using the command opens the Select file to insert dialog at the FormFeatures folder ([BricsCAD Installation folder]\Support\DesignLibrary\SheetMetal\FormFeatures); select the desired feature and double-click it, or click Open.
2. Move the cursor over the flange face you want to insert into; the dynamic UCS aligns to that face (its orientation depends on which edge the cursor entered from), and dynamic dimensions show from the UCS origin to the insertion point. You’re prompted to select an insertion point, or choose Edit inserted entity, Rotate component, set Base point, Name, insertion Type, Flip, or mUltiple.
3. Optionally choose an option: Edit (edits the insert’s parameters), Rotate (sets its rotation angle), Base Point (a different insertion base point), Name (the insert’s name), Insertion Type (Local or External), Flip (inserts on the opposite flange face), or Multiple (inserts several copies, or creates an array).
4. Specify a point, or type a distance in the dynamic dimension fields (press Tab to switch between fields).
5. Repeat to insert another copy, or press Enter to stop.

To have Form Features available in the Library panel, create or use a Mechanical Profile in the Get Started dialog.

Editing Library Form Feature Parameters

Library form features are parametric components. Length, Width, Height, and Radius parameters are named L, W, H, and R respectively; a feature’s thickness automatically matches the sheet metal part’s thickness. Edit a single feature’s parameters in either the Properties panel or the Mechanical Browser; editing multiple features at once is only possible in the Properties panel.

Selecting Form Features

• Enable Select Faces in SELECTIONMODES, then click the feature(s) directly in the model.
• Select the feature(s) in the Mechanical Browser, then press the spacebar, or right-click and choose Select (hold Ctrl for multiple).
• Use SMSELECT to select every form feature identical or similar to a chosen one, especially useful on parts with many different form features where deletion or replacement needs to target only specific ones.

Editing parameters in the Properties panel: select the form feature(s), then select a parameter under the Parameters node.

Editing parameters in the Mechanical Browser: select the feature under the Form node of the component structure tree, then select a parameter in the panel’s lower grid and type a new value.

Creating a Custom Form Feature

1. Open a new drawing using the Mechanical-mm.dwt template.
2. Create the form feature’s 3D geometry.
3. Set SMCONVERTPREFERFORMFEATURES to 1.
4. Run SMCONVERT.
5. Run BMMECH; you’re prompted for a name for the mechanical component (defaults to Component_1).
6. Type a name for the form feature.
7. You’re prompted whether to convert blocks and external references to mechanical components (defaults to Yes).
8. Choose No.
9. In the Mechanical Browser’s Extension type field, choose Sheet Metal Form Feature.
10. Select the Flange_1 and Form_1 features under the Bodies node, right-click, and choose Disable.
11. Create two new layers: UNFOLD_SYMBOL_UP and UNFOLD_SYMBOL_DOWN.
12. Turn off layer 0 and UNFOLD_SYMBOL_DOWN, and set UNFOLD_SYMBOL_UP current.
13. Draw the unfold symbol that will appear on the face the feature sits on.
14. Turn off UNFOLD_SYMBOL_UP, turn on UNFOLD_SYMBOL_DOWN, and set it current.
15. Draw the unfold symbol for the opposite face.
16. Turn layer 0 back on, turn off both unfold layers, set layer 0 current, and save the drawing.

Creating a Custom Parametric Form Feature

Continuing the custom form feature above, we’ll parametrize a conical hole using two parameters: D (the diameter of the cone’s larger edge) and A (the angle of the conical face). The built-in _SM_THICKNESS parameter already controls the sheet metal part’s thickness.

1. Create an auxiliary body for constraining on a new CONSTRUCTION layer (make it current, switching off all others).
2. Create a Region in the WCS’s XY plane on that CONSTRUCTION layer.
3. Apply a DMFIX3D constraint to the region.
4. Switch layer 0 back on.
5. Apply a DMCOINCIDENT3D constraint between the region’s face and the flange’s top face.
6. Apply a DMDISTANCE3D constraint between the flange’s top and bottom faces (select the top face, then press Tab to select the bottom, accepting the default dynamic dimension value).
7. Type _SM_THICKNESS into that Distance_3 constraint’s Expression field.
8. Since the form feature is conical, modify the flange from a parallelepiped into a cylinder.
9. In the Mechanical Browser, right-click the feature name and choose Add new parameter; name it D, set its units to mm, and type 16 in its Expression field.
10. Apply a DMRADIUS3D constraint to the conical face’s top edge (accept the default value).
11. Type D/2 into that Radius_5 constraint’s Expression field.
12. Add another new parameter named A (leave units empty), typing 45 in its Expression field.
13. Create a Cone Angle constraint on the conical face, either via DMANGLE3D‘s Cone Angle option, or by hovering the face and choosing Cone Angle constraint in the Quad menu’s Constraints group (accept the default value).
14. Type A into that ObjectAngle_6 constraint’s Expression field.
15. Turn the flange into a cylinder: draw a 9 mm radius circle on top of it, enable Enable Boundary Detection in the Settings panel of the Home ribbon tab, then hover between the circle and the flange’s square edge, choose Extrude from the Quad menu, and drag downward.
16. Apply a DMCONCENTRIC3D constraint between the region’s circular edge and the new cylindrical face.
17. Apply a DMRADIUS3D constraint to that cylindrical face (accept the default value).
18. Type D/2+0.1*_SM_THICKNESS into that Radius_8 constraint’s Expression field.
19. Set both parameters A and D’s Exposed field to On.

Now build the unfold symbols’ 2D constraints:

20. Make UNFOLD_SYMBOL_UP current, switching off every other layer.
21. Apply GCFIX to both crossing lines marking the circle centers.
22. Apply GCHORIZONTAL to the horizontal center line.
23. Apply GCVERTICAL to the vertical center line.
24. Apply GCCONCENTRIC between the two circles.
25. Apply DCLINEAR between the center lines’ endpoints (accept the default value).
26. Apply DCDIAMETER to both circles (accept the defaults for dia1, the inner circle, and dia2, the outer circle).
27. Adjust the resulting 2D constraint expressions: d1 = 1; d2 = d1; dia1 = D - 2*_SM_THICKNESS/tan(A); dia2 = D.
28. Switch off every layer except layer 0, and save the file.

This form feature can now create conical parametric openings in a sheet metal flange, insertable via the Insert Form Feature tool (BMINSERT), and optionally added as a component to a tool palette.

Creating a Bead Feature

SMBEAD creates bead features from a 2D curve drawn on a flange face.

1. Launch SMBEAD via the Create Bead Feature tool button on the Sheet Metal toolbar or ribbon, or the command itself; you’re prompted to select a flange face.
2. Select the flange face; you’re prompted to select a curve, or choose Profile radius or Round radius.
3. Select a curve on that face (lines, polylines, circles, arcs, ellipses, elliptical arcs, and splines are all accepted; it can be open or closed, but can’t self-intersect or intersect other form features); the bead feature creates.

Modifying a Bead Feature

Modify the generatrix curve: select it (press Tab to select obscured entities hidden by the bead feature, or select it in the Structure panel), then grip-edit it; the bead feature updates automatically to match.

Edit properties in the Mechanical Browser: select the bead feature there (it highlights in the model), select a property in the Bead properties grid, and type a new value; the feature updates accordingly.

Understanding the Difference Between Control and Trajectory Curves

When creating a rectangular bead feature, you first draw a rectangle, which SMBEAD uses as the control curve; grip-editing this control curve updates the bead feature accordingly. On the production side, though, this rectangular control curve gets replaced by a filleted trajectory curve, reflecting the physical limitations of the wheel tool, which is accurate but hard to manipulate directly (moving a single corner, for example).

During design, you work with the control curve instead. When SMBEAD creates the feature, it adds fillets according to the Bead fillet radius parameter in the Mechanical Browser, a property that isn’t controlled per feature, since it reflects the physical wheel tool’s own properties rather than any individual bead. Grip-editing the control curve (a polyline, for example) adjusts the bead feature accordingly, illustrating the associativity between the 2D curve and the 3D bead feature. SMCONVERTRECOGNIZERIBCONTROLCURVES controls whether SMCONVERT recognizes bead features via their control curves.

When the part unfolds with SMUNFOLD, its curves follow the 3D design and include the fillets; the middle curve in that result is called the Trajectory Curve.

Frequently Asked Questions

What’s the difference between a form feature’s control curve and its trajectory curve? The control curve is what you draw and grip-edit during design (a plain rectangle, for example); the trajectory curve is the filleted, production-accurate version reflecting the physical wheel tool’s limitations, harder to manipulate directly.

Can I use a spline as the profile for a bead feature? Yes, lines, polylines, circles, arcs, ellipses, elliptical arcs, and splines are all accepted, whether open or closed, as long as the curve doesn’t self-intersect or intersect other form features.

How do I make BricsCAD recognize form features from imported geometry as a specific library type? Use SMCONVERT to recognize them generally, then SMREPLACE to swap recognized features for ones from your built-in or user library.

What does setting a parameter’s Exposed field to On actually control? It makes that parameter (D and A in the conical hole example, for instance) available for editing when the form feature is used or inserted elsewhere.