You export a flat pattern from SolidWorks, send the DXF to the laser cutter, and get a phone call: “There are open loops in your file. The machine can’t run it.” You open the DXF back in SolidWorks, zoom in, and the outline looks fine. Zoom in further. There’s a 0.003 mm gap between two arc endpoints at a spline junction.
This problem has two distinct root causes that require different fixes. Conflating them wastes time. Here is what is actually happening in each case.
Two Different Problems, Often Called the Same Thing
When a CNC operator says “disconnected curves,” they usually mean one of two things:
Open contours — the cutting path is not a closed loop. There is a true geometric gap between the endpoint of one entity and the start of the next. The machine controller cannot determine which side of the cut is inside and which is outside, so it refuses to run.
Over-tessellated splines — the spline was converted to a polyline with too few segments. The path is technically closed, but the edges look faceted. At tight tolerances, the faceting introduces scalloping that affects cut quality on engraved text, organic shapes, or tight curves.
SolidWorks produces both types of output depending on which export path you use and which options are set. The fix for one does not fix the other.
Why Splines Are Problematic in DXF
The DXF format has carried the SPLINE entity type since AutoCAD R13 (AC1012) in 1994. Before that, the R12 format (AC1009) had no spline entity — every curved path had to be expressed as a series of ARC and LINE segments stitched into a POLYLINE.
SolidWorks defaults to exporting in R2013 format when you use Save As → DXF from a part or flat pattern. R2013 fully supports SPLINE entities, so a SolidWorks B-spline can be written directly into the file without any approximation.
The problem is that many CNC controller softwares — plasma, waterjet, and older laser software — do not correctly parse DXF SPLINE entities. They either ignore them entirely (silent failure: the entity disappears), convert them internally with a coarse chord tolerance, or crash. So SolidWorks gives you an option to pre-convert splines to polylines at a tolerance you control, rather than leaving the conversion to the machine controller.
The Chord Tolerance Setting
When SolidWorks converts a spline to a polyline, it uses chord tolerance to decide how many segments the polyline needs. Chord tolerance is the maximum allowable distance between the true spline curve and the straight-line segment that approximates it.
- Tight tolerance (e.g., 0.01 mm): many short segments, smooth output, large file size
- Loose tolerance (e.g., 0.5 mm): few long segments, faceted appearance, small file size
The option is in Tools → Options → System Options → Export, under the DXF/DWG section: “Splines” dropdown with two options — Export splines as splines and Export splines as polylines. When you select polylines, a tolerance field appears.
A common default is 0.1 mm. For visible curves on parts wider than 100 mm, 0.1 mm chord deviation is usually invisible. For CNC engraving on small text or tight radii, 0.1 mm is coarse enough to produce visible faceting.
Working tolerance values:
| Use case | Chord tolerance |
|---|---|
| Laser cutting, sheet metal flat patterns | 0.05–0.1 mm |
| CNC engraving, small text, organic curves | 0.01–0.02 mm |
| Plasma cutting, waterjet (rough profiles) | 0.1–0.25 mm |
If your CNC controller accepts DXF splines natively (most modern FANUC, Siemens, and Beckhoff-based systems do), leave the setting on Export splines as splines. Let the controller handle it — it knows its own interpolation tolerance.
Why Open Contours Happen
Open contours are a different failure mode. The spline setting above does not cause them — they come from the geometry itself.
Cause 1: Sketch Has Gaps
SolidWorks sketches are not required to be fully closed for the purpose of creating features. A sketch used for a base flange or thin feature can have intentional openings. When you export that sketch or the flat pattern derived from it, the DXF inherits those gaps.
The easiest check: with the sketch open, run Tools → Sketch Tools → Check Sketch for Feature. Set the feature type to No Check (or the relevant feature). Any open contours are highlighted in the sketch.
For existing parts, Tools → Sketch Tools → Repair Sketch will identify and optionally close gaps below a threshold you set (default: 0.00254 mm). Gaps wider than the threshold are flagged but not auto-closed — you need to manually add a line or merge the endpoints.
Cause 2: Spline-to-Polyline Conversion Introduces Rounding Gaps
This is the subtle one. When SolidWorks converts a spline to a polyline, it evaluates points along the spline at the chord tolerance interval. If two splines meet at a shared control point, the endpoint of one converted polyline and the start of the next should coincide exactly. In practice, floating-point rounding during the arc-segment computation can produce endpoints that differ by 10⁻⁷ to 10⁻⁵ mm.
Most laser cutting software has a snap tolerance that closes gaps below 0.01 mm automatically. But some controllers — especially older ones with stricter validation — treat even a 0.001 mm gap as an open contour.
The fix: in the DXF export options, enable “Merge points” (also called “Endpoint merging”). This pass-through step collapses endpoint pairs within a tight distance threshold (typically 0.001 mm) into a single shared vertex, eliminating the rounding artifacts.
Cause 3: Overlapping Entities at Sketch Junctions
When a profile is built from multiple sketch segments that meet at a shared point, the endpoint-matching is done by the SolidWorks sketch engine. If the user placed two separate endpoints near each other but did not use a Coincident relation, they look merged in the sketch view but export as two distinct points with a gap.
Zoom in to 1:1 scale in the sketch at every spline junction. Any visible gap, however small, will become an open contour in the DXF.
The Export Method Matters
SolidWorks has three distinct paths for getting a flat profile into a DXF, and they do not all produce the same output.
1. Save As → DXF from the Part
Opens the flat pattern DXF export dialog. This path exports the sheet metal flat pattern geometry computed by the CGM unfold kernel. The geometry reflects the actual manufactured shape. This is the path CadShift uses for batch DXF export — it operates on the flat pattern view directly via IExportToDWG2.
2. Insert → Drawing View, then Save As DXF from the Drawing
Exports the drawing view as DXF. The critical setting here is the view quality. Draft Quality views use a coarse approximation of curved edges for display performance — they are fast to render but produce faceted splines when exported. High Quality views compute exact edge geometry. Right-click the drawing view → Properties → View Quality → High Quality before exporting.
When using a drawing export, the DXF version is also significant. Exporting as DXF R12 forces all splines to polylines regardless of your system option setting — the format simply cannot represent SPLINE entities. Switching to R2000 or later preserves SPLINE entities. For the tradeoffs between DXF versions, see DXF R12 vs R2000 vs R2010 in SolidWorks.
3. Sketch → Save As DXF
This exports the raw sketch geometry, not the computed flat pattern. It bypasses the sheet metal bend deduction and unfold entirely. Useful for 2D profiles that were never modeled as sheet metal, but it produces a different result than the flat pattern path for any part with bends.
The Re-Import Verification Step
The fastest way to confirm your DXF is valid is to re-import it into SolidWorks immediately after export:
- File → Open → DXF, set import type to 2D Sketch
- SolidWorks loads the geometry into a sketch
- Run Tools → Sketch Tools → Check Sketch for Feature — any open loops appear highlighted in red
If there are gaps, you know before the file leaves your machine. This is faster than waiting for the fabricator’s toolpath software to reject it.
For high-volume batch exports, CadShift validates the exported DXF geometry as part of the export pipeline, flagging open contours per-part in the export log rather than finding out at the machine.
Summary
| Symptom | Root cause | Fix |
|---|---|---|
| Faceted, jagged splines | Chord tolerance too loose | Tighten to 0.01–0.05 mm, or export as true SPLINE entities |
| Open contour at curve junction | Rounding during spline-to-polyline | Enable “Merge points” in export options |
| Open contour at sketch junction | No Coincident relation in sketch | Add relation or use Repair Sketch |
| Open contour in drawing export | Draft Quality view | Switch view to High Quality before exporting |
| All splines become line segments | Exporting as DXF R12 | Switch to R2000 or R2013 format |
The right default for sheet metal flat patterns sent to laser cutting: export from the part (not the drawing), set DXF version to R2013, set splines to Export as splines, enable Merge points. Verify by re-importing before sending. If your specific laser controller rejects SPLINE entities, switch to polylines at 0.05 mm chord tolerance — that is the cutoff where the difference becomes visually significant on typical sheet metal profiles.