A SOLIDWORKS forum question asked this week: how do you model a curved sheet metal part, and do stamping structures require forming tools? The answer depends entirely on what “curved” means, because SOLIDWORKS handles three fundamentally different curved-sheet-metal scenarios with three different tools — and forming tools are a separate concern from the geometry of the base body.

This post maps the decision tree.

The Three Curved Sheet Metal Scenarios

SOLIDWORKS sheet metal works by tracking a flat-pattern state for every feature. Every bend is stored with a radius, K-factor, and bend allowance so the flat pattern can be computed by unfolding. Curved geometry complicates this in three distinct ways:

Cylindrical body: A tube or curved-profile part whose cross-section curves in one direction. The flat pattern is a simple rectangle or parallelogram. Every straight-sided cylinder is a developable surface — it can be unrolled flat with zero distortion. SOLIDWORKS handles this natively with the Base Flange or Convert to Sheet Metal tool.

Conical body: A cone or tapered transition where the cross-section changes diameter. The flat pattern is a sector (pie slice) or annular sector. Cones are also developable and SOLIDWORKS handles them with the Lofted Bend feature.

Doubly-curved (compound-curved) body: A saddle, dome, or any surface that curves simultaneously in two directions. These are non-developable — their Gaussian curvature is nonzero, and no flat pattern exists that preserves both distances and angles. SOLIDWORKS cannot produce an exact flat pattern for these. The Surface Flatten tool (SOLIDWORKS Premium) provides an approximation with user-controlled tear lines.

Cylindrical Sheet Metal: Base Flange

A cylindrical tube is the simplest case. Create a Base Flange with an arc sketch — not a full circle (closed sketches aren’t valid for sheet metal), but an arc that leaves a gap. Set the thickness, bend radius, and K-factor. SOLIDWORKS produces a flat pattern that is a rectangle with length equal to the arc length.

The common error: sketching a full 360-degree circle and wondering why the Flat Pattern feature won’t unsuppress. Sheet metal requires at least one open edge to unfold through. For a complete cylinder, you need a gap — even 0.01mm — or use the Rip feature after creation to add it.

For parts that start as cylindrical solids (imported geometry, for example), Convert to Sheet Metal handles the same scenario. Select the cylindrical face as the base, mark the seam edge as a rip, and SOLIDWORKS reverse-engineers the sheet metal parameters from the geometry.

Conical Sheet Metal: Lofted Bend

The Lofted Bend is the correct tool for conical transitions, reducers, and any sheet metal part defined by two parallel open profiles of different geometry. It behaves like the Loft feature but operates in the sheet metal environment, adding flat-pattern tracking.

Bent vs. Formed methods

The choice of method controls both the manufacturing assumption and the flat-pattern output:

Bent (default): SOLIDWORKS approximates the cone with a series of planar bends. The flat pattern contains discrete bend lines. The number of bend lines is controlled by the faceting parameters — chord tolerance, number of bends per transition segment, segment length, or segment angle. The K-factor and bend radius apply to each bend, so the flat pattern accurately models what a press brake with multiple setups would produce.

Formed: SOLIDWORKS treats the part as being shaped by a specialized die that produces smooth geometry rather than discrete bends. The flat pattern has no bend lines — just a single curved surface. K-factor doesn’t apply. The model looks correct for a spinning or roll-forming operation, but the flat pattern is an approximation computed by geometric unrolling rather than bend allowance calculation.

The API exposes this distinction directly through ILoftedBendsFeatureData. Decompiling the SolidWorks interop reveals that FormedMethod is a boolean: True for formed, False for bent. The InsertSheetMetalLoftedBend2 method signature shows how faceting is controlled:

' Insert a bent lofted bend with chord-tolerance faceting
Dim swFeat As Feature
swFeat = swFeatMgr.InsertSheetMetalLoftedBend2( _
    1,          ' ThickDirType: 1 = inside (default)
    0.002,      ' Thickness in meters (2mm)
    False,      ' BFormed: False = bent method
    0.001,      ' DRadius: 1mm bend radius
    False,      ' BReferToEndPoint: use smallest arcs (not theoretical vertexes)
    0,          ' EFacetOption: 0 = chord tolerance
    0.00127,    ' DChordTol: 0.05" max chord deviation
    0,          ' INumBends: not used when EFacetOption = 0
    0,          ' DSegLength: not used
    0 _         ' DSegAngle: not used
)

The EFacetOption parameter maps to swLoftedBendFacetOptions_e:

  • 0 = chord tolerance (distance between arc and linear segment)
  • 1 = bends per transition segment
  • 2 = segment length
  • 3 = segment angle

For manufacturing, chord tolerance is usually the right choice — it directly controls how closely the approximated bends match the true conical geometry.

The flat pattern difference is significant. With the Bent method, every bend line appears in the DXF flat pattern as a separate line entity, typically on its own layer. With the Formed method, the flat pattern is a single body outline with no bend lines — which is correct if the part is roll-formed, but misleading if the fabricator expects bend-line guidance.

Prerequisites before calling InsertSheetMetalLoftedBend2

Before calling InsertSheetMetalLoftedBend2, you must select at least two sketch profiles on parallel planes. The profiles must be open sketches (not closed loops). Pre-select them using IModelDocExtension.SelectByID2 with Mark = 1 for each profile. If the profiles are closed, the feature creation fails silently — no error dialog, just Nothing returned.

Doubly-Curved Parts: When Sheet Metal Tools Can’t Help

If the part curves in both principal directions — think a dome, a saddle, or a compound-curve body panel — it isn’t developable. No combination of Base Flange, Lofted Bend, or Convert to Sheet Metal will produce a geometrically correct flat pattern, because one doesn’t exist.

SOLIDWORKS Premium includes Surface Flatten, which approximates the flat pattern for non-developable surfaces. The ISurfaceFlattenFeatureData interface exposes the key parameters:

  • ShouldMakeTears — when True, SOLIDWORKS adds user-defined tear lines (from TearEdges) to relieve the Gaussian curvature before unrolling. Without tears, the flattened mesh distorts.
  • AccuracyFactor — controls the mesh density used in the finite-element unrolling computation.
  • MapEdges — maps specific 3D edges to their 2D positions in the flat pattern, useful for aligning hole positions.

The flat pattern from Surface Flatten is an engineering approximation. The area and perimeter are preserved as well as the mesh resolution allows, but corner angles and distances between non-adjacent points will be slightly wrong. For most formed or hydroformed sheet metal where the part is stretched and thinned during forming, the approximation is sufficient. For tight-tolerance work, validate against actual formed blanks.

The other option is to export the surface to Rhino and use Squish, which runs a different unrolling algorithm. The flat wrap vs. developable surfaces guide covers when Squish is worth the export overhead.

Forming Tools: A Separate Question

The original forum question asked whether “stamping structures require forming tools.” This is where the terminology gets muddled — forming tools in SOLIDWORKS are a specific feature type that is completely separate from the geometry of the base sheet metal body.

A forming tool is a part file (.sldprt) saved in the Forming Tools folder and used as a die to indent, lance, or otherwise deform sheet metal. Built-in forming tools include:

  • Louvers — a combination of lance and form that creates a ventilation slot
  • Lances — a cut-and-bend that tabs a flap from the sheet
  • Dimples — a circular indentation
  • Ribs — a stiffening bead pressed into the sheet
  • Flanges — an extruded hole with a surrounding flange (for fasteners)

These features appear in the feature tree as Forming Tool feature types. In the flat pattern, they’re represented as their footprint outline — the 3D deformed geometry suppresses, showing only the flattened boundary. This is what the fabrication receives: the flat blank outline plus cut lines for lances, with the stamping depths called out on the drawing.

When are forming tools required for stamped structures? If you want SOLIDWORKS to recognize the stamped feature as a proper sheet metal feature — with the correct flat-pattern footprint, no interference with bend lines, and propagation through configurations — then yes, you need a forming tool. If you just need the geometry (a dimple modeled as a shell feature, for example), you can use a surface tool and no forming tool library entry is needed, but you lose flat-pattern integration.

On a curved base body (a conical lofted bend, for example), forming tools can be placed on the curved surface. SOLIDWORKS positions the tool normal to the surface at the placement point. The constraint is that the tool must not intersect any bend line from the underlying lofted bend.

Flat Pattern DXF Export for Lofted Bend Parts

Lofted bend parts export flat patterns via the same IPartDoc.ExportToDWG2 path used for standard sheet metal, but the behavior differs depending on the method used.

For a Bent lofted bend, the flat pattern contains the outline, bend lines (on their own layer by default), and any cut features. Export via the flat pattern view in a drawing, or use ExportToDWG2 with Action = 1 (drawing view export) rather than Action = 0 (face-selection geometry):

Sub ExportLoftedBendFlat()
    Dim swApp As SldWorks.SldWorks
    Dim swModel As ModelDoc2
    Dim swPart As PartDoc
    Dim exportData As ExportPDFData
    
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    Set swPart = swModel
    
    ' Unsuppress the flat pattern before export
    Dim swFlatFeat As Feature
    Dim swFeat As Feature
    Set swFeat = swModel.FirstFeature
    Do While Not swFeat Is Nothing
        If swFeat.GetTypeName2 = "FlatPattern" Then
            Set swFlatFeat = swFeat
        End If
        Set swFeat = swFeat.GetNextFeature
    Loop
    
    If Not swFlatFeat Is Nothing Then
        swFlatFeat.Select2 False, 0
        swModel.EditUnsuppress2
    End If
    
    Dim outputPath As String
    outputPath = Left(swModel.GetPathName, Len(swModel.GetPathName) - 7) & "_flat.dxf"
    
    Dim bRet As Boolean
    bRet = swPart.ExportFlatPatternView(outputPath, 1)  ' 1 = flat pattern view
    
    If Not bRet Then
        MsgBox "Export failed — check that the flat pattern is unsuppressed"
    End If
End Sub

For a Formed lofted bend, the flat pattern geometry is computed differently — there are no bend lines, and the outline is a single curved boundary. The export works the same way via ExportFlatPatternView, but the output DXF will contain only the outline without any bend line entities.

The API vs. manual DXF export differences guide covers why ExportToDWG2 Action=0 (face selection) produces different geometry from the flat pattern view for standard parts — the same distinction applies to lofted bends. Always use Action=1 or ExportFlatPatternView when the output needs to match what the flat pattern view shows in a drawing.

For assembling a K-factor and bend allowance that matches your press brake, the Bent method’s flat pattern is the right starting point — you’re working with the same bend allowance math used for standard flanges. The Formed method’s flat pattern requires calibration against actual roll-formed or spun blanks.

If you’re processing multiple conical lofted-bend parts in a batch, CadShift handles flat-pattern extraction from assemblies with mixed standard and lofted-bend bodies — each body’s flat pattern exports separately with the correct metadata layers. See batch DXF export from a SolidWorks assembly for the workflow.