CNC Router Toolpath Generation

Automatic Toolpath Generation: Convert vector paths to G-code with climb/conventional selection and offset compensation.

Tab Placement Preview: Visualize where tabs hold parts in place before cutting.

Feed Rate Calculator: Optimize speed and RPM per material and bit diameter.

1. Input Format: Vector paths (DXF, SVG, AI) for 2D profiles, STL or STEP for 3D carving.
2. Output Format: G-code (machine instructions) or tool-specific format (e.g., .sbp for ShopBot, .nc for generic CNC).
3. Tool Library: End mill diameter, flute count, material (HSS, carbide, compression).
4. Material Thickness: Exact measurement for depth calculations and tab placement.

The direction the bit rotates relative to feed direction affects surface finish and tool life

Climb Milling (Down-Cut): Bit rotates in same direction as feed. Chip load starts thick, ends thin.

• Pros: Smoother finish, less chipout on top edge, less tool deflection.
• Cons: Can pull part loose if not secured, requires rigid machine.
• Use for: Final pass on visible edges, hardwoods, aluminum.

Conventional Milling (Up-Cut): Bit rotates opposite to feed direction. Chip load starts thin, ends thick.

• Pros: Better chip evacuation, less likely to pull part loose.
• Cons: Rougher finish, more chipout on top edge.
• Use for: Roughing passes, softwoods, plastics.

Best Practice: Rough cuts in conventional, final pass in climb for best finish.

Step-Over: Overlap percentage between adjacent tool passes. Smaller step-over = smoother finish but longer cut time.

• Roughing: 40-60% of bit diameter (faster, rougher).
• Finishing: 10-30% of bit diameter (slower, smoother).
• 3D Carving: 5-15% for fine detail.

Depth of Cut: How deep the bit plunges per pass. Depends on material hardness and bit diameter.

• Softwood (pine, poplar): 50-100% of bit diameter per pass.
• Hardwood (oak, maple): 25-50% of bit diameter per pass.
• MDF: 50-75% of bit diameter per pass.
• Aluminum: 10-30% of bit diameter per pass, use cutting fluid.
• Acrylic: 30-50% of bit diameter, single-flute bit to prevent melting.

Tabs are small uncut sections that hold parts in place during cutting

Tab Size: 3-6mm wide, 50-75% of material thickness. Larger parts need bigger tabs.

Tab Count: Minimum 3 tabs per part, 4+ for parts over 300mm. Space evenly around perimeter.

Tab Location: Place on straight edges or gentle curves, never on tight inside corners (stress concentrator). Avoid placing tabs where surface finish matters.

Tab Cleanup: Sand, chisel, or router after cutting. Leave 1-2mm tab material and sand flush.

Z-zero sets the vertical reference point for depth calculations

Material Top: Zero probe touches material surface. Use for through-cuts and profiles. Easy to reset between parts.

Spoilboard Top: Zero probe touches waste board under material. Use for pocketing and engraving where material thickness varies. Requires precise material thickness measurement.

Tool Length Offset: Machine stores tool lengths, auto-adjusts Z-zero when changing bits. Professional machines only.

Always re-zero Z after changing bits or material.

Feed Rate: How fast the bit moves through material (mm/min or in/min). Too fast = rough finish and bit breakage. Too slow = burning and dull bit.

RPM: Spindle rotation speed. Higher RPM for small bits and soft materials, lower RPM for large bits and hard materials.

Chip Load: Amount of material removed per tooth per revolution. Optimal chip load depends on material and bit type.

### General Feed Rate Formula

Feed Rate (mm/min) = RPM × Number of Flutes × Chip Load (mm)

Example: 1/4" 2-flute carbide in MDF

• RPM: 18,000
• Flutes: 2
• Chip Load: 0.1mm
• Feed Rate: 18,000 × 2 × 0.1 = 3,600 mm/min (141 in/min)

### Common Material Settings (1/4" carbide bit)

MDF/Plywood: 18,000 RPM, 3,000-4,500 mm/min feed, 6mm depth of cut.

Hardwood: 16,000 RPM, 2,000-3,000 mm/min feed, 4mm depth of cut.

Softwood: 18,000 RPM, 4,000-6,000 mm/min feed, 8mm depth of cut.

Aluminum: 12,000 RPM, 800-1,500 mm/min feed, 2mm depth of cut, flood coolant.

Acrylic: 10,000 RPM, 2,000-3,000 mm/min feed, 5mm depth of cut, single-flute bit.

Straight Bit: Flat end, used for profiles, pockets, dados. Most common.

Ball Nose: Rounded end, used for 3D carving and contoured surfaces.

V-Bit: Angled tip, used for engraving text, V-carve inlays, chamfers.

Compression Bit: Up-cut flutes at bottom, down-cut at top. Clean edges on both surfaces. Best for plywood.

Downcut Bit: Pushes chips down, clean top edge. Use for through-cuts where top surface matters.

Upcut Bit: Pulls chips up, clean bottom edge. Better chip evacuation for deep cuts.

Bit Breakage: Feed rate too high, depth of cut too deep, or bit dull. Reduce feed rate 20-30%, shallow depth of cut, replace bit.

Rough Finish: Wrong milling direction (use climb for final pass), dull bit, or excessive step-over. Use sharp carbide bit, reduce step-over to 25%.

Part Pulled Loose: Insufficient tabs, climb milling on unsecured part, or tabs too small. Add more tabs, increase tab size, use conventional milling.

Burning: Feed rate too slow or RPM too high. Increase feed rate 20-30%, reduce RPM 10-20%.

Chipout on Top Edge: Conventional milling on final pass, or dull bit. Use climb milling for final pass, use compression bit for plywood.