How do I fix open contours in DXF files for nesting?

Open contours cause nesting failures because the software cannot determine inside vs outside. Fix by: (1) Use PEDIT > Join in AutoCAD to connect near-endpoints within 0.01mm tolerance, (2) Check for duplicate overlapping lines that prevent joining, (3) Convert splines to polylines for better compatibility, (4) Use the AUDIT and OVERKILL commands to clean geometry before export.

What is the optimal gap between parts for common-line cutting?

For common-line cutting, the optimal gap is 0-0.3mm depending on material. For standard nesting without shared edges: use 2-5mm gap for thin sheet ( 6mm). The gap must account for kerf width (typically 0.15-0.5mm for fiber laser) plus a safety margin to prevent heat-affected zone overlap.

How do small features in DXF affect nesting efficiency?

Small features (text engravings, tiny holes <1mm, decorative details) significantly impact nesting because nesting software must maintain minimum spacing around these features. Simplify or remove unnecessary small features before nesting. For holes smaller than material thickness, consider post-processing (drilling) instead of laser cutting to improve nesting density.

DXF Nesting Best Practices: 10 Rules for Maximum Material Utilization

Q: What DXF version is best for laser cutting nesting?

DXF R14 (AutoCAD 2000) is the most compatible version for laser cutting nesting software. It supports all necessary geometry types while maintaining maximum compatibility across SigmaNEST, ProNest, Lantek, and other major nesting platforms. Avoid DXF 2018+ formats as some nesting software may not fully support newer entity types.

Q: Should I nest parts in CAD or use dedicated nesting software?

Always use dedicated nesting software for production. Manual CAD nesting typically achieves 60-70% utilization while automated nesting software (SigmaNEST, ProNest, Lantek) achieves 75-90%+ through advanced algorithms including true-shape nesting, common-line optimization, and remnant management. The 10-20% utilization improvement easily justifies the software investment.

⚡ Key Takeaway

Proper DXF file preparation can improve nesting utilization by 5-15% — saving thousands of dollars annually in material costs. The most impactful practices: close all contours, remove duplicate entities, convert splines to polylines, and set layer-based cut parameters.

DXF file quality directly determines nesting efficiency. Poorly prepared files cause import errors, reduce utilization rates, and increase scrap. This guide covers the 10 most critical DXF preparation rules used by production facilities running 10,000+ sheets per year. For the broader nesting strategy, see our Nesting Optimization Guide.

Published: February 11, 2026

Last Updated: February 11, 2026

Skill Level: Intermediate to Expert

1. Close All Contours — The #1 Rule

Open contours are the single most common cause of nesting failures. Nesting software must identify closed boundaries to determine part geometry. Even a 0.01mm gap between endpoints will cause the part to be rejected or incorrectly nested.

❌ Common Problems

• Lines not joined at endpoints (gap > 0.001mm)

• Arcs converted from circles with open segments

• Imported geometry with broken polylines

• Splines that don't close properly

✅ Solutions

• AutoCAD: PEDIT → Join (tolerance 0.01mm)

• SolidWorks: Check Sketch → Find Open Contours

• Fusion 360: Inspect → Validate Sketch

• Any CAD: Zoom to 1000x on each corner to verify

Pro Tip: Run AutoCAD's AUDIT command followed by OVERKILL before every DXF export. This catches 90% of geometry issues automatically.

2. Remove Duplicate and Overlapping Entities

Duplicate lines cause the laser to cut the same path twice, wasting time and potentially damaging edges. Overlapping entities also confuse nesting software contour detection, resulting in incorrect part boundaries.

Detection & Removal Methods:

• AutoCAD: OVERKILL command (tolerance 0.001mm)

• Manual: Select all → Properties → check for multiple entities on same coordinates

• Nesting QC: If part perimeter in nesting differs from CAD by > 5%, suspect duplicates

• Prevention: Avoid Copy/Paste in place — use MOVE instead when repositioning

3. Convert Splines to Polylines

Splines (NURBS curves) are mathematically complex and many nesting and CNC controllers handle them poorly. Converting to polylines with appropriate chord tolerance ensures consistent results across all platforms.

Recommended Chord Tolerance by Application:

Standard Parts

Tolerance: 0.05-0.1mm

Good balance of accuracy and file size

Precision Parts

Tolerance: 0.01-0.02mm

Medical/aerospace — larger file, higher accuracy

Decorative/Sign

Tolerance: 0.1-0.5mm

Visual accuracy sufficient, smaller files

4. Use Layer-Based Cut Parameter Assignment

Organize your DXF by layers to separate different cutting operations. Most nesting software maps layers to cutting parameters automatically, enabling mixed operations (cutting, engraving, marking) in a single nest.

Layer Name	Color	Operation	Typical Settings
CUT	Red (1)	Through cut (external)	Full power, standard speed
CUT_INTERNAL	Yellow (2)	Internal holes and cutouts	Same as CUT, processed first
ENGRAVE	Green (3)	Surface engraving	Reduced power, higher speed
MARK	Cyan (4)	Part ID marking	Low power, fast scan
BEND	Magenta (6)	Bend line reference (no cut)	Not processed — reference only

5. Optimize Small Features for Nesting Density

Small features (tiny holes, text, decorative details) create "exclusion zones" around parts that reduce nesting density. The nesting software must maintain minimum spacing around these features, effectively making each part occupy more sheet area than its actual boundary.

Minimum Hole Diameter Rule: Holes should be ≥ material thickness. For 3mm steel, minimum hole is 3mm diameter. Smaller holes require drilling or EDM — remove them from the DXF cutting file to improve nesting. See Material Thickness Parameters for detailed minimum feature sizes by material.

Text Simplification: Convert text to single-line fonts or outlines. Multi-stroke fonts create excessive small segments. For part identification, use dot-peen marking post-processing instead of laser engraved text when possible.

Feature Consolidation: Group mounting holes at standard spacings (e.g., 25mm grid). Standard patterns nest more efficiently than random hole placements.

6. Set Correct Units and Scale

DXF files are unit-agnostic — geometry is stored as dimensionless numbers. This causes frequent scale errors when files are created in inches but imported in millimeters (or vice versa). A part designed at 100mm will appear at 100 inches if units are mismatched — a 25.4× error.

Prevention Checklist:

Set AutoCAD INSUNITS to 4 (millimeters) before drawing
Include a reference dimension (e.g., 100mm square) on a separate layer for verification
Always verify part dimensions in nesting software after import
Standardize your shop on one unit system (mm is industry standard)

7. Include Kerf Compensation in Design

The laser beam removes material (kerf width typically 0.15-0.5mm for fiber lasers). For precision parts, you must decide whether kerf compensation is applied in CAD or by the nesting/controller software. Double compensation is a common error. Use our Kerf Calculator to determine the correct compensation for your setup.

Method A: CAD Compensation

• Offset contours in CAD by half-kerf

• Set nesting software kerf to 0

• Best for: Single-material shops

• Risk: Wrong if material/power changes

Method B: Software Compensation (Recommended)

• Draw parts at nominal dimensions

• Set kerf in nesting/controller software

• Best for: Multi-material, production shops

• Advantage: Change kerf per material/power

8. Clean Up Non-Geometry Entities

Dimensions, text annotations, hatching, viewport boundaries, and block references can interfere with nesting import. Even if they don't cause errors, they increase file size and processing time.

Pre-Export Cleanup Sequence:

Delete all dimensions (DIMSTYLE → Purge → Delete objects)
Explode all blocks to base geometry
Remove all hatching and fills
Flatten 3D geometry to 2D (FLATTEN command)
Delete all text on cutting layers (keep on MARK layer if needed)
Run PURGE → All to remove unused definitions
Run AUDIT → Fix all errors

9. Export in the Right DXF Version

Not all DXF versions are created equal. Newer versions support more entity types but have lower compatibility with CNC controllers and nesting software.

DXF Version	Compatibility	Recommendation
R14 / 2000	Universal (99%+ software)	✅ Best for production
2007 / 2010	High (90%+ software)	Good if you need mesh/solid support
2013 / 2018+	Limited (70% software)	⚠️ May cause import errors

10. Validate Before Sending to Production

Establish a validation checklist that every DXF file must pass before it enters the nesting queue. Catching errors at the design stage saves 10-50× the time compared to fixing problems on the shop floor.

Production-Ready DXF Checklist:

☐ All contours closed (zero open endpoints)

☐ No duplicate/overlapping entities

☐ Splines converted to polylines

☐ Layers correctly assigned (CUT, ENGRAVE, etc.)

☐ Units verified (mm, dimensions correct)

☐ Kerf compensation method documented

☐ Non-geometry entities removed

☐ Minimum feature size ≥ material thickness

☐ DXF version: R14 or 2000

☐ AUDIT + PURGE completed

Frequently Asked Questions

What DXF version is best for laser cutting nesting?

DXF R14 (AutoCAD 2000) offers the best compatibility across all major nesting platforms (SigmaNEST, ProNest, Lantek, FastCAM). It supports all necessary 2D geometry types while avoiding compatibility issues with newer entity formats. Set SAVEAS → AutoCAD 2000 DXF in your CAD software.

How do I fix open contours in DXF files?

In AutoCAD: Select the lines → PEDIT → Yes → Join → set tolerance to 0.01mm. This joins all endpoints within the tolerance. If join fails, check for duplicate overlapping lines (use OVERKILL) or tiny gaps (zoom to 1000× on each corner). In SolidWorks: Tools → Sketch Tools → Check Sketch for Errors.

What gap should I use between parts in nesting?

Standard part spacing: 2-5mm for thin sheet (<3mm), 5-10mm for thick plate (> 6mm). For common-line cutting, spacing is 0-0.3mm (parts share a cut edge). This gap must account for kerf width plus heat-affected zone to prevent part distortion.

Should I nest parts in CAD or use dedicated nesting software?

Always use dedicated nesting software for production volumes. Manual CAD nesting achieves 60-70% utilization vs 75-90%+ with automated software. The 10-20% improvement on a shop running $50,000/month in material costs saves $60,000-120,000 annually — far exceeding software costs. See our nesting ROI analysis for detailed calculations.

How do small features affect nesting efficiency?

Small features create larger exclusion zones around parts, reducing nesting density. Remove holes smaller than material thickness from cutting DXFs and use post-processing (drilling, punching) instead. Simplify text engravings to single-line fonts. These optimizations typically recover 2-5% utilization.

Related Tools & Guides

Nesting Optimization Guide

Complete nesting strategy with ROI analysis

Nesting Efficiency Calculator

Calculate material utilization and savings

Kerf Calculator

Determine kerf width for accurate compensation

Cutting Time Calculator

Estimate cycle time from part geometry

Cutting Speed Chart

Speed data for nesting time estimates

Cost Estimator

Calculate material waste cost impact

This guide is based on production best practices from facilities using SigmaNEST, ProNest, Lantek, and Radan nesting software. Specific commands reference AutoCAD 2024+ but equivalent functions exist in all major CAD platforms. Always verify your specific nesting software documentation for import requirements.