The Lofted Bend PropertyManager has a Manufacturing Method dropdown with two options: Bent and Formed. When the dropdown shows only Formed — or you select Bent and get a flat pattern with no bend lines — the root cause is almost always one of three things: sketch planes that aren’t parallel, profile geometry that has sharp corners, or connector points placed on the wrong part of the sketch entities.
None of these are obvious from the error message, and the official documentation buries the parallel-plane requirement. Here’s what’s actually going on.
What Bent and Formed Actually Mean
Bent treats the loft as a sequence of discrete press-brake bends separated by flat sections. SolidWorks approximates the curved transition by folding the geometry into a faceted shape — a series of small planar flats connected by defined bend lines. The flat pattern shows individual bend lines that a press brake operator can use directly. K-factor, bend allowance, and gauge table parameters apply.
Formed treats the loft as a smoothly curved surface produced by a non-traditional process (stamping, hydroforming, roll forming). There are no discrete bend lines in the flat pattern — instead, the flat pattern is a developable approximation of the curved surface with a specified maximum deviation tolerance. The sheet metal parameters (K-factor, bend radius) are irrelevant because the process doesn’t use them.
The practical difference: if your part goes to a press brake, you need Bent and usable bend lines. If it goes to a roll former or is being stamped, Formed is appropriate. If you’re modeling a duct transition that goes to plasma or waterjet (cut flat and welded), either can work, but Bent gives you explicit bend geometry to check against your forming method.
The Parallel Planes Requirement
This is the single most common reason Bent is unavailable or produces a flat pattern with no bend lines.
The Bent manufacturing method requires that the two sketch planes be parallel to each other. SolidWorks needs parallel planes to compute where the bend lines run — they’re geometrically perpendicular to the direction connecting the two profiles, and that direction only exists unambiguously when the planes don’t tilt relative to each other.
Prior to SolidWorks 2015, both sketch planes had to be parallel for the Lofted Bend feature to work at all. Non-parallel planes simply errored out.
SolidWorks 2015 introduced non-parallel support, but only for the Formed method. If your planes are at any angle to each other, SolidWorks silently makes the Bent option either unavailable or non-functional — it won’t tell you why. You select Bent, the preview generates, but when you look at the flat pattern there are no bend lines. Or the dropdown shows only Formed.
Diagnosis: Check whether your two sketch planes are truly parallel. Open the first plane’s properties and note the normal vector. Open the second and compare. Even a 0.1° difference from the imported geometry or from a misclick when creating the plane is enough to trigger this.
Fix: If your design intent requires Bent, rebuild one plane as an offset of the other using Insert > Reference Geometry > Plane > Offset Distance. This guarantees parallelism. Then re-sketch the profile on the new parallel plane.
Profile Geometry: Sharp Corners Block Formed, Open Profiles Block Both
The two methods have different profile requirements that are not stated together anywhere in the documentation.
For Bent: The profile sketch must be an open contour — a line, arc, or chain of segments with two free endpoints. A closed loop (like a full rectangle or circle) cannot be used with Bent. Open the sketch where you want the fold to start and end.
For Formed: The profile must also be open, but additionally cannot include sharp corners. If your sketch has a 90° vertex where two lines meet at a point, Formed either rejects the input or produces degenerate geometry. Add sketch fillets to all corners — even a 0.001" fillet satisfies the constraint — before switching to Formed.
This creates an asymmetry: if you want Bent but your profile has fillets throughout, it will work. If you want Formed but your profile has any sharp vertex, it won’t. In practice, transition pieces (square-to-round, rectangle-to-circle duct fittings) typically have one sketched profile that is a rectangle with sharp corners and another that is a circle. You can use Formed if you add fillets to the rectangle profile, or you can use Bent if the planes are parallel.
Connector Points: Why the Surface Twists
Both methods use connector points to determine how the loft surface is constructed between the two profiles. Connector points are the vertices or anchor points on each sketch that SolidWorks maps to each other when building the transition surface.
If the connector points align in a way that causes a twist — imagine connecting the top-left corner of a square to the bottom-right of a circle — you get a helical surface instead of a clean transition. The flat pattern will be unusable or fail entirely.
How to see and move connector points: After the loft preview generates, right-click on the surface mesh in the graphics area and select Show All Connectors. Small colored points appear on the sketch profiles. These show the current mapping. Drag a connector point to a different location on the sketch to change how the profiles connect.
The key rule is that connector points must land at the endpoint of a sketch entity, not on a curve midpoint. If your profile is an arc, the connector point can only sit at one of the arc’s endpoints. Trying to drag it onto the arc body snaps it back to the nearest endpoint. This is the source of the Reddit question that motivated this post — users see the connector handle and try to drag it to a specific point on a smooth curve, find it won’t stay, and assume the feature is broken.
For a square-to-circle transition:
- On the square: put one connector at a corner (the endpoint where two lines meet)
- On the circle: put the corresponding connector at the point on the circle that is geometrically closest to where you want the seam line to run
- Make sure you don’t inadvertently create a twist by mapping diagonally opposite corners
If the surface still twists after setting connector points manually, check whether the two profiles have the same winding direction. A square sketched clockwise and a circle sketched counterclockwise will twist regardless of connector positions. Use Sketch > Tools > Flip Direction to change the winding on one profile.
What the Flat Pattern Shows
The flat pattern differences between Bent and Formed are significant for downstream use.
Bent flat pattern: Produces a flat geometry where the curved transition is represented by a series of flat facets separated by explicit bend lines. The number of bend lines is controlled by the Facet Count setting in the Lofted Bend PropertyManager — more facets means a smoother approximation but more bend lines for the press brake operator to hit. The flat area of each facet is exactly the flat you need to form. Bend line annotations show up in drawings and can drive a bending program directly.
Formed flat pattern: Produces a flat geometry with no bend lines, derived from developable surface mathematics. The flat pattern is the best planar approximation of the curved surface, governed by a Maximum Deviation tolerance (default 0.050"). Tighter deviation means more intermediate geometry. Because there are no discrete bend lines, you can’t use this with a press brake in the conventional way — the fabricator needs a form die or roll-forming tooling to produce the surface as modeled.
For batch DXF export, Bent-derived flat patterns export as closed polylines with bend line entities on separate layers. Formed-derived flat patterns export as smooth closed profiles with no internal geometry — which is fine for plasma or waterjet cutting the flat blank, but tells the operator nothing about how to form it.
When to Use Each
Use Bent when:
- The part goes to a press brake
- You need defined bend lines on the drawing
- Both profiles are on parallel planes
- You need accurate developed length for material ordering
Use Formed when:
- The part is stamped, hydroformed, or roll-formed
- The profiles are on non-parallel planes (unavoidable in some duct transitions)
- You only need the flat blank for cutting, not for bending to a program
- The profile has smooth curves that can’t be approximated as facets
Use neither — redesign — when:
- The transition is too complex for SolidWorks lofted bend to flatten (compound curvature that isn’t developable). In that case, see flat wrap vs developable surfaces for the Rhino Squish path.
Checking the Flat Pattern K-Factor
When Bent produces a flat pattern with valid bend lines, the developed length of each flat section is computed using the K-factor from the sheet metal feature. If your lofted bend part inherits the default K-factor (0.50 for most materials) but your shop presses aluminum to a K of 0.40, the flat pattern dimensions will be wrong.
Check the K-factor by right-clicking the Sheet-Metal feature in the FeatureManager and selecting Edit Feature. The K-factor, bend allowance, and gauge table settings are all here. The Lofted Bend feature uses whatever values are set at the sheet metal level, same as any other bend in the part.
For press-formed transitions where bend allowance accuracy matters, understanding what goes into flat pattern calculations makes it clear why the K-factor setting at the part level propagates to every feature — lofted bends included.
Quick Diagnostic Checklist
When your lofted bend won’t show Bent, or Bent produces no flat pattern bend lines:
- Are the sketch planes parallel? Check normal vectors. If not, rebuild one as an offset of the other.
- Are the profiles open contours? Both must be open (not closed loops).
- Does the Formed-method profile have sharp corners? Add fillets if using Formed.
- Are connector points at sketch entity endpoints, not midpoints? Right-click > Show All Connectors to verify.
- Do both profiles have the same winding direction? Flip one if the surface twists.
- Are you on SolidWorks 2015 or later? Pre-2015, non-parallel planes simply don’t work with any Lofted Bend option.