Skip to content

Contour Cutting

Contour cutting traces the outline of vector shapes to cut them free from material. It's the most common laser operation for creating parts, signs, and decorative pieces.

Overview

Contour operations:

  • Follow vector paths (lines, curves, shapes)
  • Cut along the perimeter of objects
  • Support single or multiple passes for thick materials
  • Can use inside, outside, or on-line cutting paths
  • Work with any closed or open vector shape

When to Use Contour

Use contour cutting for:

  • Cutting parts free from stock material
  • Creating outlines and borders
  • Cutting shapes from wood, acrylic, cardboard
  • Perforating or scoring (with reduced power)
  • Creating stencils and templates

Don't use contour for: - L Filling areas (use Raster instead) - L Creating 3D depth effects (use Depth Engraving instead) - L Bitmap images (convert to vectors first)

Creating a Contour Operation

Step 1: Select Objects

  1. Import or draw vector shapes on the canvas
  2. Select the objects you want to cut
  3. Ensure shapes are closed paths for complete cuts

Step 2: Add Contour Operation

  • Menu: Operations Add Contour
  • Shortcut: Ctrl+Shift+C
  • Right-click: Context menu Add Operation Contour

Step 3: Configure Settings

Key Settings

Power & Speed

Power (%): - Laser intensity from 0-100% - Higher power for thicker materials - Lower power for scoring or marking

Speed (mm/min): - How fast the laser moves - Slower = more energy = deeper cut - Faster = less energy = lighter cut

Starting values (3mm plywood): - Power: 70-90% - Speed: 300-600 mm/min - Always test on scrap material first!

Multi-Pass Cutting

For materials thicker than a single pass can cut:

Passes: - Number of times to repeat the cut - Each pass cuts deeper - Typical: 1-3 passes for 3mm material

Pass Depth (Z-step): - How much to lower Z-axis per pass (if supported) - Requires Z-axis control on your machine - Creates true 2.5D cutting - Set to 0 for same-depth multiple passes

Example for 6mm plywood: - Passes: 3 - Pass depth: 2mm per pass - Result: Cuts 6mm total depth

Z-Axis Required

Pass depth only works if your machine has Z-axis control. For machines without Z-axis, use multiple passes at the same depth.

Path Offset

Controls where the laser cuts relative to the vector path:

Offset Description Use For
On Line Cuts directly on the path Centerline cuts, scoring
Inside Cuts inside the shape Parts that must fit exact size
Outside Cuts outside the shape Holes that parts fit into

Offset Distance: - How far inside/outside to offset (mm) - Typically set to half your kerf width - Kerf = width of material removed by laser - Example: 0.15mm offset for 0.3mm kerf

Cut Direction

Clockwise vs Counter-Clockwise: - Affects which side of the cut gets more heat - Usually clockwise for right-hand rule - Change if one side burns more than the other

Optimize Order: - Automatically sorts paths for minimum travel - Reduces job time - Prevents missed cuts

Advanced Features

Holding Tabs

Tabs keep cut pieces attached to stock material during cutting:

  • Add tabs to prevent pieces from falling
  • Tabs are small uncut sections
  • Break tabs after job completes
  • See Holding Tabs for details

Kerf Compensation

Kerf is the width of material removed by the laser beam:

Why it matters: - A circle cut "on line" will be slightly smaller than designed - The laser removes ~0.2-0.4mm of material (depending on beam width)

How to compensate: 1. Measure your kerf on test cuts 2. Use path offset = kerf/2 3. For parts: offset inside by kerf/2 4. For holes: offset outside by kerf/2

See Kerf for detailed guide.

Lead-In/Lead-Out

Lead-ins and lead-outs control where cuts start and end:

Lead-in: - Gradual entry to the cut - Prevents burn marks at start point - Moves laser to full speed before hitting the material edge

Lead-out: - Gradual exit from the cut - Prevents damage at end point - Common for metals and acrylics

Configuration: - Length: How far the lead extends (mm) - Angle: Direction of the lead path - Type: Straight line, arc, or spiral

Tips & Best Practices

Material Testing

Always test first: 1. Cut small test shapes on scrap 2. Start with conservative settings (lower power, slower speed) 3. Gradually increase power or decrease speed 4. Record successful settings

Cutting Order

Best practices: - Engrave before cutting (keeps material secured) - Cut inside features before outside perimeter - Use holding tabs for parts that might move - Cut smallest parts first (less vibration)

Quality Cutting

For clean cuts: - Use air assist (blows debris away) - Ensure proper focus (sharp beam = clean cut) - Multiple faster passes often better than one slow pass - Keep material flat and secured

 Avoid: - Cutting at maximum power (creates excessive charring) - Single slow pass (more heat = more burning) - Skipping material tests - Cutting warped or unsecured material

Common Materials

Material Thickness Power Speed Passes Notes
Paper 0.2mm 10-20% 3000+ mm/min 1 Very fast
Cardboard 3mm 40-60% 1500-2500 mm/min 1 Test for char
Plywood 3mm 70-90% 300-600 mm/min 1-2 Use air assist
Acrylic 3mm 80-95% 200-400 mm/min 1-2 Slow for clean edges
MDF 3mm 70-85% 400-700 mm/min 1-2 Very dusty

Settings vary by laser type, power, and beam quality. Always test!

Troubleshooting

Cuts not going through material

  • Increase: Power setting
  • Decrease: Speed setting
  • Add: More passes
  • Check: Focus is correct
  • Check: Beam is clean (dirty lens)

Excessive charring or burning

  • Decrease: Power setting
  • Increase: Speed setting
  • Use: Air assist
  • Try: Multiple faster passes instead of one slow
  • Check: Material is appropriate for laser cutting

Parts fall out during cutting

  • Add: Holding tabs
  • Use: Cutting order optimization
  • Cut: Inside features before outside
  • Ensure: Material is flat and secured

Inconsistent cut depth

  • Check: Material thickness is uniform
  • Check: Material is flat (not warped)
  • Check: Focus distance is consistent
  • Verify: Laser power is stable

Missed corners or curves

  • Decrease: Speed (especially on corners)
  • Check: Machine acceleration settings
  • Verify: Belts are tight
  • Reduce: Path complexity (simplify curves)

Technical Details

Coordinate System

Contour operations work in: - Units: Millimeters (mm) - Origin: Depends on machine and job setup - Coordinates: X/Y plane (Z for multi-pass depth)

Path Generation

Rayforge converts vector shapes to G-code:

  1. Offset path (if inside/outside cutting)
  2. Optimize path order (minimize travel)
  3. Insert lead-in/lead-out (if configured)
  4. Add holding tabs (if configured)
  5. Generate G-code commands

G-code Commands

Typical contour G-code: 

G0 X10 Y10          ; Rapid move to start
M3 S204             ; Laser on at 80% power
G1 X50 Y10 F500     ; Cut to point at 500 mm/min
G1 X50 Y50 F500     ; Cut to next point
G1 X10 Y50 F500     ; Continue cutting
G1 X10 Y10 F500     ; Complete the square
M5                  ; Laser off