SOLIDWORKS 2026 SP3.2 introduced a regression specific to the flat-pattern DXF export path: bend lines appear in the cleanup window preview, the Bend lines checkbox in the DXF/DWG Output PropertyManager is checked, yet the written DXF has no bend line entities whatsoever. The geometry exports fine. Layers are correct. But the press brake operators get a DXF with no fold marks.

This is a distinct failure mode from the SP3 regression documented in the general bend lines troubleshooting guide. That post covers the mapping file regression (enable-flag rows silently cleared) and per-user registry mismatches. The SP3.2 bug is different: the mapping file is intact, the registry value is correct, the entity bitmask is correct — and the export still omits bend lines.

What the cleanup window is actually doing

When you right-click a Flat-Pattern feature and choose Export to DXF/DWG, SOLIDWORKS opens the DXF/DWG Output PropertyManager. At the top is a preview rendering of the flat pattern — the “cleanup window” — where you can remove unwanted entities before committing the export.

This preview is generated by an internal hidden drawing SOLIDWORKS creates in memory. It renders the flat pattern with all entity types visible, including bend lines. The bend lines you see in the cleanup preview are drawn from this in-memory drawing, not from the bitmask that controls what the export engine writes.

Therein lies the SP3.2 bug: the preview and the writer read from different sources. The cleanup preview always shows bend lines. The export engine, in SP3.2, was changed to honor the active drawing template’s bend line visibility state instead of relying purely on the PropertyManager bitmask. If the drawing template — the .drwdot file configured under Tools > Options > System Options > Default Templates — was saved without bend lines visible, the export engine suppresses them regardless of what the PropertyManager says.

You check the box. The preview confirms it. You export. No bend lines.

Confirming this is the SP3.2 issue

Before applying the workaround, rule out the other causes:

  1. Not a mapping file issue. Go to Tools > Options > System Options > Export > DXF/DWG. If Custom Map SOLIDWORKS to DXF/DWG is enabled, click Map Entities. Under the Sheet Metal category, verify the enable checkboxes for Bend Lines – Up Direction and Bend Lines – Down Direction are checked. If they are unchecked, that is the SP3 mapping file regression — re-enable and re-save. If they are checked and you still get no bend lines, continue.

  2. Not a per-user registry mismatch. Open regedit.exe, navigate to HKCU\SOFTWARE\SolidWorks\SOLIDWORKS 2026\General\Export, and read the decimal value of FlatPatternOption. Bit value 4 must be set for bend lines. A value of 5 (1 + 4) means geometry + bend lines; 13 (1 + 4 + 8) adds sketches. If bit 4 is absent, fix the registry — that is the per-user issue covered in the troubleshooting guide. If bit 4 is set and you still see no bend lines in the output, you are hitting the SP3.2 bug.

  3. Drawing template visibility. This is the root cause. Open your default drawing template (draw.drwdot or equivalent). Insert any sheet metal part with a flat pattern view. Check whether bend lines are visible in that view: View > Hide/Show > Bend Lines. If they are hidden, that is exactly the condition the SP3.2 export engine is reading. Fix the template (instructions below) or use the annotation view workaround.

Workaround: convert bend lines to sketch + export via Annotation Views

This is the reliable fix. It sidesteps the SP3.2 bug entirely because it routes bend line geometry through a different emit path — one the regression does not affect.

Step 1 — Convert bend lines to sketch geometry

Open your sheet metal part. In the FeatureManager tree, find the Flat-Pattern feature and confirm it is unsuppressed (it should be active if you are trying to export it).

Start a new sketch. In the Sketch toolbar, use Insert > Sketch. The sketch plane should be the flat-pattern face — click the flat top face of the unsuppressed flat pattern to set the plane.

Inside the sketch, go to Tools > Sketch Tools > Convert Entities (or click the Convert Entities icon in the Sketch toolbar). Select all bend line edges from the flat pattern. You can window-select the entire flat pattern and the bend lines will be among the selected edges, or select them individually if you prefer.

Click OK. The bend line segments appear in the sketch as regular 2D lines, fully parametrically linked to the flat pattern geometry — if the part changes and bend positions shift, the sketch updates automatically.

Exit the sketch. Rename it to something identifiable: right-click in the tree and choose Rename Feature. “BendLines-Sketch” or similar. The sketch appears as a child feature under Flat-Pattern.

Step 2 — Export using Annotation Views

Right-click the Flat-Pattern feature and choose Export to DXF/DWG. The DXF/DWG Output PropertyManager opens with the cleanup preview.

At the top of the PropertyManager, find Export selection set. Change this from Sheet Metal to Annotation Views.

With Annotation Views selected, SOLIDWORKS exports the visible content of the named annotation views rather than reading the entity bitmask. The converted bend line sketch is now ordinary sketch geometry — SOLIDWORKS treats it as visible sketch entities in the flat pattern view, and they are emitted to the DXF correctly.

Verify the output layer assignment before finalizing: if your shop uses a named BEND layer for press brake operators, your mapping file layer assignment for Sketch entities should include that layer, or add the converted sketch to a separate layer via the mapping file. The converted sketch lines are class ISketchLine, not IBendLine — they will not appear in the bend-line-specific mapping file rows. Assign them through the Sketches category in Map Entities, or accept them on layer 0 and let the press brake operator identify them by linetype (assign a center-dashed or phantom linetype to the sketch).

Fixing the drawing template (prevents recurrence)

The root cause is a drawing template with bend lines hidden. Fixing the template means the SP3.2 export engine’s template-visibility check passes, and the Sheet Metal export path works again without the sketch workaround.

  1. Open your default drawing template: File > New > Drawing, then select the template you use.
  2. Insert a sheet metal part with a flat pattern view: Insert > Drawing View > Flat Pattern, or drag from the View Palette.
  3. Right-click the flat pattern view in the drawing and choose View (Properties), or go to View > Hide/Show > Bend Lines to enable bend line visibility.
  4. Confirm bend lines are now visible in the view.
  5. File > Save As > file type: Drawing Template (*.drwdot), overwriting the original. Accept the dialog warning about re-saving a template.

After saving, new exports via the Sheet Metal path should include bend lines again without the sketch workaround — the export engine’s template visibility check now finds them visible.

Note: if your team shares drawing templates via a central network location, update that copy. Individual users with local cached templates may need to re-download.

API path: immune to the SP3.2 bug

If you run batch exports via macro or a tool like CadShift, the API path bypasses the bug entirely. The key is which export action you specify in ExportToDWG2:

' VBA: Sheet Metal path - uses entity bitmask. Affected by SP3.2 bug.
bRet = swPart.ExportToDWG2(sOutPath, sPartPath, _
    swExportToDWG_e.swExportToDWG_ExportPropertyManager, _
    True, vAlignmentData, False, False, lOptions, vNull)

' VBA: Annotation Views path - immune to the SP3.2 bug.
' Requires annotation view to exist in the part with bend lines visible.
bRet = swPart.ExportToDWG2(sOutPath, sPartPath, _
    swExportToDWG_e.swExportToDWG_ExportAnnotationViews, _
    True, vAlignmentData, False, False, lOptions, vNull)

swExportToDWG_ExportAnnotationViews (value 2) tells the engine to export from annotation views rather than the bitmask-driven Sheet Metal path. With the converted sketch in place and this export action specified, bend lines are included regardless of drawing template state. This is the same mechanism as the manual workaround above, expressed via the API.

For a complete reference on the ExportToDWG2 bitmask options and how the API diverges from manual export, see the DXF export entity settings reference.

SP3.2 and the broader bend-line landscape

This regression sits alongside two earlier issues that remain unresolved for some users:

SP3 mapping file reset (mid-2026): The SP3 installer cleared the enable-flag rows in Map Entities for some configurations. If your mapping file had bend line rows configured, they silently stopped emitting after the update. Fix: re-enable the rows in Map Entities dialog and re-save the .swmapfile.

SP3.2 template visibility (this post): The Sheet Metal export path reads drawing template display state. If bend lines are hidden in the template, they are suppressed in the output despite the PropertyManager checkbox. Fix: repair the template, or use the annotation view + converted sketch path.

Both issues compound: a user who hit the SP3 mapping file regression, fixed it by reconfiguring Map Entities, then updated to SP3.2 may find bend lines missing again — but now the template is the cause, not the mapping file. Applying the SP3 fix a second time won’t help.

If you have batch export workflows across large part lists, the annotation view path in the API is the most durable approach: it is not affected by either the SP3 or SP3.2 regressions, and the converted bend line sketch updates parametrically when the model changes. The DXF layer mapping guide covers how to ensure the sketch entities land on the correct layer in the output DXF so CAM software reads them without confusion.