How to V-Carve Inlays and Precision Signs on a Desktop CNC Router

Introduction

V-carving uses a V-shaped bit to cut tapered grooves into material. Unlike flat end mills, a V-bit cuts deeper for wide areas and shallower for narrow areas, producing crisp variable-width lines with sharp corners. This is the standard method for professional signage, inlay work, and decorative engraving in wood, acrylic, and soft metals.

V-Bit Selection

• 60 degree V-bit: Sharper angle, finer detail, deeper cuts — best for text and fine lines
• 90 degree V-bit: Wider angle, shallower cuts, bolder appearance — best for larger signs
• 30 degree V-bit: Very fine detail — for jewelry, small text
• 120 degree V-bit: Very wide, shallow — for large area clearing

Step 1: Design Setup in Vectric VCarve

1. File > New > Create New File
2. Set job dimensions (e.g., 200mm x 100mm x 12mm)
3. Set XY origin to bottom-left or center
4. Set Z origin to top surface of material

Create Vectors

1. Use the Text tool to add your sign text
2. Choose a bold font with clean lines (Arial Black, Impact, stencil fonts)
3. Convert text to curves (Ctrl+Q)
4. Import logos as DXF/SVG

Step 2: Create V-Carve Toolpath

1. In the Toolpath panel, click V-Carve/Router Toolpath
2. Select your V-bit from the tool database
3. Start depth: 0 (top of material)
4. Flat depth (optional): limits maximum depth for shallow engravings
5. Enable Flat Area Clearance for wide areas — clears center with end mill first
6. Click Calculate and preview in 3D

Material-Specific Settings

Hardwood (Maple, Cherry, Walnut)

• 60 degree V-bit: 800-1200mm/min feed, 300mm/min plunge, 18,000 RPM
• 90 degree V-bit: 1000-1500mm/min feed, 400mm/min plunge, 18,000 RPM

MDF

• 60 degree: 1500-2000mm/min feed, 500mm/min plunge, 18,000 RPM
• 90 degree: 1800-2500mm/min feed, 600mm/min plunge, 16,000 RPM

Acrylic

• 60 degree: 800-1200mm/min feed, 300mm/min plunge, 20,000 RPM
• Use air blast or mist coolant to prevent melting

Two-Color Inlay Technique

1. V-carve the design into your base material (e.g., walnut)
2. Use Vectric's Inlay Toolpath to create the male profile
3. Cut inlay material (e.g., maple) 0.2mm proud of pocket depth
4. Test fit dry — should slide in with light pressure
5. Apply Titebond III glue, press in place, wipe excess
6. Clamp with wax paper and cauls, cure 24 hours
7. Sand flush starting with 120 grit, progress to 220

Finishing

• Remove dust with compressed air
• Sand lightly with 220 grit if surface is rough
• Apply Danish oil for natural grain enhancement
• Or apply polyurethane for outdoor durability
• For painted contrast: fill V-carved areas with acrylic paint, sand off excess

Troubleshooting

• Fuzzy edges: Reduce feed rate by 20%, increase spindle speed, or use sharper bit
• Chipped corners: Reduce plunge rate, check for knots in material
• Uneven depth: Tram/square your spindle, ensure material is flat

Pro Tips

• Always use a sharp V-bit — dull bits produce ragged edges
• Two-stage cutting (clearance + V-carve) is 3-5x faster than V-carve alone
• Test fonts at small size before committing — thin fonts do not V-carve well
• Use a Z-probe before every job — V-carving requires precise Z-zero

Conclusion

V-carving transforms a desktop CNC from a cutting tool into an engraving instrument. The tapered cuts produce professional-quality text and graphics that flat end mills cannot match. For signage, V-carved text with painted inlay creates high-contrast durable results. The keys are sharp V-bits, precise Z-zero, appropriate feeds and speeds, and two-stage cutting for efficiency.