SolidWorks DXF Export — Why Bend Lines Disappear and How to Get Them Back

If bend lines stopped appearing in your DXF exports after a SolidWorks service pack update, you are not alone. The r/SolidWorks threads from August 2026 show multiple engineers hitting this after 2025 SP5 and 2026 SP3. Some had working configurations for years. They installed the update, exported a flat pattern, and the bend lines were gone.

The problem is fixable — but only if you understand that bend lines disappear for fundamentally different reasons depending on how you export. Applying the wrong fix wastes time and leaves you thinking the issue is deeper than it is.

Two export paths, two root causes

SolidWorks has two distinct paths for getting a flat pattern into a DXF file:

Path A — Part-level export: Right-click the Flat-Pattern feature in the FeatureManager tree → Export to DXF/DWG. Or open a sheet metal part and use File → Save As → DXF. This path gives you the flat pattern options dialog with checkboxes for Geometry, Bend lines, Sketches, and so on.

Path B — Drawing-level export: Create a drawing with a flat pattern view inserted, then File → Save As → DXF on the drawing. This path exports the drawing sheet as DXF. The bend line visibility in the output comes from whether bend lines are visible in the drawing view.

These paths produce different behavior because they use different engines. Path A reads the solid geometry and uses the entity checkboxes (stored as a bitmask) to decide what to emit. Path B reads the drawing view’s display settings — whatever is visible in the drawing is what goes into the DXF.

If you are on Path A and bend lines are missing, the cause is the entity checkbox (or mapping file). If you are on Path B, the cause is the drawing template. Confirming which path you use takes thirty seconds and determines which fix applies.

Diagnosing Path A (part-level export)

Open a sheet metal part. Right-click the Flat-Pattern feature. If you see Export to DXF/DWG in the context menu, you are on Path A.

When you get to the export dialog, look for an Options button. Click it. You will see a tab called Sheet Metal (or similar, depending on version). The relevant checkboxes are:

• Export flat pattern geometry — must be checked or the output is empty
• Include sheet metal bend lines — this is the one controlling bend line output

If that checkbox is unchecked, that is your immediate fix. Check it and export again.

The deeper problem: this checkbox is not persisted between SolidWorks sessions. As documented in the SolidWorks DXF entity export settings internals, the entity checkboxes in the flat pattern export dialog reset to their internal defaults every time SolidWorks restarts. The only thing the dialog persists is the active layer mapping file. If you had a working workflow and bend lines suddenly stopped appearing, a restart or update likely reset the checkbox.

Diagnosing Path B (drawing-level export)

Open your drawing. Look at the flat pattern view. Go to View → Hide/Show and check whether Bend Lines is in the visible list. If bend lines are hidden in the drawing view, they will be absent from the DXF.

The underlying mechanism: SOLIDWORKS uses the active drawing template (.drwdot file) as the baseline for view display settings when a new drawing is created. If the template was saved without bend line visibility enabled, every drawing created from it will have bend lines hidden by default.

Fix for Path B:

1. Find your default drawing template. Tools → Options → System Options → Default Templates shows the path. It ends in something like draw.drwdot.
2. Open a new drawing from that template. File → New → Drawing.
3. Insert any sheet metal part with a flat pattern view.
4. In the drawing view, right-click → View (Properties), or use View → Hide/Show → Bend Lines to enable them.
5. Save the drawing as a template: File → Save As → file type Drawing Template (*.drwdot), overwriting the original.
6. Future drawings created from this template will have bend lines visible by default.

Why the 2025 SP5 and 2026 SP3 service packs are causing recurrence

The regression that multiple engineers hit in mid-2026 is specific to Path A users who had a custom DXF mapping file configured. Here is what happens:

Before SolidWorks 2022, bend lines were assigned to a layer named BEND by default. In 2022, that default was removed. To get bend lines on a named layer in the output DXF, you need to explicitly map them in the mapping file — the .swmapfile format described in detail in SolidWorks DXF layer mapping for laser cutting.

When you configure a mapping file correctly, the Sheet Metal entity category contains two mappable types: Bend Lines – Up Direction and Bend Lines – Down Direction. You assign each to a layer (typically BEND-UP and BEND-DOWN, or a single BEND layer for shops that don’t need direction). Save the map file, and SOLIDWORKS remembers which map file to use between sessions (it persists the file path in the registry, unlike the entity checkboxes).

The problem introduced by 2025 SP5 and 2026 SP3: the service pack installer modifies the system-level default mapping file settings. In some configurations, this clears the entity checkbox state for the Sheet Metal category within the mapping file dialog — specifically, the checkmark that tells SOLIDWORKS to include bend line entities in the export at all. Your map file still exists on disk. SOLIDWORKS still loads it. But it now ignores the bend line rows because the enable flag was reset.

The result: geometry exports correctly, layers look right for other entity types, but bend lines are simply absent. Engineers who had working configurations for years suddenly see the regression after a routine update.

Fixing the mapping file regression

Go to Tools → Options → System Options → Export → DXF/DWG. Confirm that Custom Map SOLIDWORKS to DXF/DWG is checked. If not, enable it and reload your .swmapfile.

Click Map Entities. In the left column, find the Sheet Metal category. Expand it. You should see:

• Bend Lines – Up Direction
• Bend Lines – Down Direction
• (possibly) Bounding Box

Check whether the enable checkbox on the left of each bend line row is checked. After the regression, these are often unchecked even though the row exists and has a layer assignment. Check them.

Assign the bend line types to their destination layers (BEND-UP and BEND-DOWN, or a single BEND layer per your shop’s convention). Set linetype to a dashed or centerline style — center-dashed is the most widely readable convention for press brake operators.

Click Save Map File to write the updated configuration back to disk.

Export a test part and verify bend lines appear on the correct layer before returning this to production.

Separating entity selection from layer mapping

A common point of confusion: the entity checkbox and the mapping file work together, not independently.

The entity checkbox (Path A dialog) is a gate: it decides whether bend lines are included in the export at all. If unchecked, no mapping file configuration will make bend lines appear — the exporter simply does not emit them.

The mapping file controls which DXF layer those bend lines land on and what linetype they carry. If you have no mapping file, bend lines still appear in the export (assuming the checkbox is set), but they land on the default layer 0 with whatever linetype the exporter defaults to.

After 2022, the default layer for bend lines changed and many users saw them “disappear” — they were present in the DXF but on a different layer than the CAM software expected, so the software ignored them. This is a different failure mode from the regression above.

To diagnose: open the exported DXF in a viewer (DraftSight, eDrawings, or Notepad). Search for BEND in the layer table. If the layer exists with entities, the lines are there but on an unexpected layer. If no bend entities exist anywhere, the entity checkbox was off.

When your coworker’s export includes bend lines but yours does not

If you have verified the entity checkbox and the mapping file, and both look correct, but a coworker running the same export from the same file still gets bend lines while you do not — the problem is per-user registry settings.

SolidWorks stores the flat pattern export entity checkboxes as a DWORD bitmask in the Windows registry under each user’s profile, not in the document and not in a shared location. Two users on the same workstation (or two Windows accounts across different machines) can have different values for this key, producing different output from identical part files.

Registry location (substitute your SolidWorks year):

HKEY_CURRENT_USER\SOFTWARE\SolidWorks\SOLIDWORKS 2026\General\Export

Value name: FlatPatternOption (DWORD, read as decimal)

The bitmask breaks down as follows:

A value of 1 exports geometry only. A value of 5 (1 + 4) exports geometry plus bend lines. A value of 13 (1 + 4 + 8) exports geometry, bend lines, and sketches. If your registry shows 1 and your coworker’s shows 5 or higher, that is the discrepancy.

To check your value: Open regedit.exe, navigate to the path above (adjusting the year for your installed version), and read the decimal value of FlatPatternOption. Compare it with what your coworker has.

To fix it, choose one of three approaches:

1. Through the dialog: Right-click the Flat-Pattern feature → Export to DXF/DWG → Options. Check the entities you want, including bend lines. Click OK. This writes the correct bitmask to your registry for your user session without touching regedit directly.
2. Direct registry edit: Change FlatPatternOption to 5 (geometry + bend lines) or the correct combined value. Requires admin rights on some machines.
3. Team-wide deployment: For organizations where per-user inconsistency is a recurring problem, push a standardized registry value via Group Policy, a .reg file deployed through IT onboarding, or a PowerShell script. This eliminates the “works on my machine” variance permanently:

# Set FlatPatternOption to geometry + bend lines + sketches (value 13)
# Run once per user session or deploy via GPO
$regPath = "HKCU:\SOFTWARE\SolidWorks\SOLIDWORKS 2026\General\Export"
Set-ItemProperty -Path $regPath -Name "FlatPatternOption" -Value 13 -Type DWord

Second per-user variable: the mapping file path. The active DXF mapping file path is also stored per-user:

HKEY_CURRENT_USER\SOFTWARE\SolidWorks\SOLIDWORKS 2026\General\Export

Value name: DXFCustomMapping (string). Your coworker may have a .swmapfile configured that includes bend lines, while your session points to a different file or none at all. When diagnosing a coworker discrepancy, always check both FlatPatternOption and the DXFCustomMapping path. If the paths differ, the active mapping file configuration differs — and a mapping file that omits bend line layer assignments will suppress them even when the entity checkbox is set.

Locking it in with the API

If you run batch exports via VBA or C# — whether via a custom macro or a tool like CadShift — you bypass the dialog entirely and pass the options as a bitmask. The relevant flag is swExportFlatPatternOption_e.swExportFlatPatternGeometry combined with swExportFlatPatternOption_e.swExportFlatPatternBendLines:

' VBA: export with geometry + bend lines + sketches
Dim lOptions As Long
lOptions = 1 Or 4 Or 8   ' geometry=1, bend lines=4, sketches=8

Dim bRet As Boolean
bRet = swPart.ExportToDWG2(sOutPath, sPartPath, _
    swExportToDWG_e.swExportToDWG_ExportAnnotationViews, _
    True, vAlignmentData, False, False, lOptions, vNull)

Using value 4 in the bitmask guarantees bend lines in every export regardless of what the dialog checkbox says. This is the only way to make the setting immune to SP updates and user sessions. The complete VBA export walkthrough covers the full ExportToDWG2 signature including the face selection prerequisites.

For bend line layer assignment in API-driven exports, you still need the mapping file to be configured — the API uses whatever mapping file is currently active in System Options. Setting the mapping file path via ISldWorks.SetUserPreferenceStringValue with swUserPreferenceStringValue_e.swDxfMappingFile allows you to programmatically select a specific map file before each export, which is how batch tools handle multi-fabricator workflows without manual switching.

Summary diagnostic flow

1. Are you exporting from the part (right-click Flat-Pattern) or from a drawing?
2. From part: Check Options → Sheet Metal → Include bend lines. If unchecked, check it. If it resets after restart, use the API bitmask or a tool that hardcodes it.
3. From drawing: Enable bend lines in the drawing view, then re-save the drawing template.
4. Had a mapping file and it stopped working after an SP update: Open Map Entities → Sheet Metal category → re-enable the bend line rows → re-save the map file.
5. Bend lines appear in the DXF but CAM software ignores them: They are on the wrong layer. Open the DXF in a text editor and check the layer table. Configure the mapping file so bend lines land on the layer your CAM software reads.
6. Coworker gets bend lines from the same file but you do not: Per-user registry mismatch. Check HKCU\SOFTWARE\SolidWorks\SOLIDWORKS <year>\General\Export → FlatPatternOption. Must include bit value 4 (bend lines). Also check DXFCustomMapping — different users may have different active mapping files.

The regression in 2025 SP5 and 2026 SP3 is specifically case 4. The coworker mismatch (case 6) is a per-user configuration issue unrelated to SP updates — both users need the same registry values and the same mapping file. Using the API bitmask (case 2) is immune to both because it bypasses the per-user settings entirely.