CNC Router Bits for Woodworking: A Complete Guide to Choosing the Right Router Tooling

Choosing the right CNC router bit is one of the most practical decisions a woodworking or sign making business makes on a daily basis. The bit you select for a given material and operation has a direct impact on cut quality, edge finish, tool life, spindle load, and production efficiency.

Many CNC router owners — especially those new to the technology — underestimate the importance of tooling selection. They invest carefully in the right machine, configure their software correctly, and then use a general-purpose bit that produces rough edges, tears the surface of laminated panels, or wears out after a fraction of its expected life. The result is poor output quality, increased material waste, and higher production costs.

This guide covers everything woodworking and sign making businesses need to know about CNC router bits — the main types, what each one is designed to do, which materials they work best with, and how to select the right bit for each application. Whether you are cutting cabinet panels on a 1325 wood CNC router, carving dimensional signs on a 6090 CNC router, or profiling acrylic letters for a sign shop, this guide will help you get better results from every job.

How CNC Router Bits Work: Key Concepts

Before comparing specific bit types, it helps to understand the key concepts that determine how a router bit performs.

1.1. Flute Count and Chip Clearance

The flute is the cutting edge and the channel that carries chips away from the cutting zone. The number of flutes on a bit affects:

• Chip clearance — Fewer flutes mean larger chip channels and better chip evacuation, which is important for materials that produce large chips or require high feed rates

• Surface finish — More flutes produce a smoother surface finish because each flute takes a smaller chip per revolution

• Feed rate — More flutes allow higher feed rates at the same chip load per flute

For most woodworking applications, single-flute and two-flute bits are the most common choices. Single-flute bits are preferred for soft materials and plastics where chip clearance is critical. Two-flute bits are the standard for general woodworking.

1.2. Upcut, Downcut, and Compression Geometry

The helix direction of the flutes determines how the bit moves chips and how it affects the cut surfaces.

• Upcut spiral — Flutes spiral upward, pulling chips out of the cut and away from the workpiece. Produces clean cuts on the bottom face of the material but can cause slight tearout on the top surface of laminated panels. Excellent chip evacuation makes upcut bits the standard choice for deep pocketing and through-cutting in solid wood and MDF.

• Downcut spiral — Flutes spiral downward, pushing chips into the cut. Produces a clean, chip-free edge on the top surface of the material but can cause tearout on the bottom face and traps chips in the cut, generating more heat. Best used for shallow surface operations where top-face finish quality is the priority.

• Compression spiral — Combines an upcut section at the tip with a downcut section above it. The upcut tip cuts cleanly from the bottom face while the downcut section above cuts cleanly from the top face simultaneously. This geometry produces clean, chip-free edges on both faces of laminated panels in a single pass, making it the preferred choice for melamine-faced MDF and laminated particleboard in cabinet production.

Understanding this geometry is essential for anyone cutting laminated sheet materials. Using an upcut bit on melamine-faced board will chip the top surface. Using a compression bit eliminates this problem entirely.

1.3. Cutting Material: Carbide vs HSS

Almost all professional CNC router bits used in woodworking are made from solid carbide or have carbide cutting edges. Carbide is significantly harder and more wear-resistant than high-speed steel (HSS), which means:

• Longer tool life, especially in abrasive materials like MDF and particleboard

• Ability to run at higher spindle speeds without losing hardness

• Better edge retention for cleaner cuts over longer production runs

HSS bits are cheaper but wear much faster in CNC applications where the spindle runs continuously at high speed. For any serious production use, solid carbide bits are the correct choice.

1.4. Shank Diameter

The shank is the cylindrical portion of the bit that is held in the collet. Common shank diameters for CNC router bits include:

• 6mm — Common for smaller bits and fine detail work

• 8mm — Mid-range, used for general woodworking bits

• 12mm — Standard for larger diameter bits and heavy-duty cutting

• 1/4 inch (6.35mm) and 1/2 inch (12.7mm) — Common in North American markets

Always confirm that the bit shank diameter matches the collet size on your machine's spindle. Using an adapter to run a mismatched shank size reduces rigidity and can cause vibration and accuracy problems.

The Main Types of CNC Router Bits for Woodworking

2.1. Straight Upcut Spiral Bit

The straight upcut spiral bit is the most commonly used general-purpose CNC router bit for woodworking. It is the standard choice for through-cutting, pocketing, and profile operations in MDF, plywood, solid wood, and particleboard.

Best materials:

• MDF

• Plywood

• Solid wood

• Particleboard (non-laminated)

• Softwood and hardwood panels

Typical applications:

• Through-cutting panel shapes

• Pocket clearing for recessed features

• Profile routing on solid wood components

• General woodworking operations where top-face finish is not critical

Advantages:

• Excellent chip evacuation

• Versatile across a wide range of materials and operations

• Available in a wide range of diameters and cutting lengths

• Good tool life in MDF and plywood

Limitations:

• Can cause slight tearout on the top surface of laminated panels

• Not the best choice for melamine-faced board where top-face finish quality is critical

For cabinet shops and furniture factories cutting raw MDF and plywood, the straight upcut spiral bit is the workhorse of daily production. Machines like our 1325 wood CNC router running full production shifts will typically use upcut spiral bits for the majority of panel cutting operations.

Recommended starting parameters for MDF:

• Spindle speed: 18,000–22,000 RPM

• Feed rate: 4,000–8,000 mm/min depending on bit diameter and depth of cut

• Depth of cut per pass: 50–100% of bit diameter

2.2. Compression Spiral Bit

The compression spiral bit is the most important bit for cabinet making and furniture production involving laminated sheet materials. Its combined upcut/downcut geometry produces clean, chip-free edges on both the top and bottom faces of melamine-faced MDF, laminated particleboard, and HPL-faced panels in a single pass.

Best materials:

• Melamine-faced MDF

• Melamine-faced particleboard

• HPL (High Pressure Laminate) faced panels

• Veneer-faced plywood

• Any laminated sheet material where both faces must be chip-free

Typical applications:

• Cabinet panel cutting in furniture factories

• Wardrobe and kitchen cabinet carcass production

• Cutting laminated panels for retail display and interior fit-out

• Any through-cutting operation where both faces of the material are visible in the finished product

Advantages:

• Clean, chip-free edges on both faces in a single pass

• Eliminates the need for secondary edge finishing on laminated panels

• Reduces material waste from chipped panels

• Significantly improves production quality for cabinet and furniture work

Limitations:

• More expensive than standard upcut bits

• Requires correct cutting depth to engage both the upcut tip and downcut body simultaneously — too shallow a cut will not activate the compression geometry

• Not necessary for non-laminated materials

Critical setup note: The compression geometry only works correctly when the cutting depth is sufficient to engage both the upcut tip section and the downcut body section simultaneously. For most compression bits, this means the cutting depth must be at least equal to the length of the upcut tip section — typically 3–8mm depending on the bit. Always check the manufacturer's specification for minimum cutting depth.

For cabinet shops using our 1325 wood CNC router for melamine panel production, the compression bit is the single most important tooling investment for improving daily output quality.

Recommended starting parameters for 18mm melamine particleboard:

• Spindle speed: 18,000–22,000 RPM

• Feed rate: 5,000–10,000 mm/min

• Depth of cut: Full thickness in one or two passes depending on bit diameter

2.3. V-Bit (V-Groove Bit)

The V-bit cuts a V-shaped groove into the material surface. It is one of the most widely used bits in sign making, decorative woodworking, and engraving applications. The angle of the V determines the character of the carved line.

Common V-bit angles:

• 30° — Very fine, deep V-groove for detailed engraving and fine lettering

• 60° — The most commonly used angle for V-carving and sign lettering

• 90° — Broader, shallower V-groove for larger lettering and decorative line work

• 120° — Very wide, shallow cut used for chamfering edges and broad decorative work

Best materials:

• MDF

• Solid wood

• HDU foam

• Plywood

• PVC foam board

• Aluminum composite panel (for surface engraving)

Typical applications:

• V-carving lettering and logos on wood and MDF signs

• Decorative line engraving on furniture panels

• Chamfering edges on cabinet doors and panels

• Creating V-groove fold lines in aluminum composite panel for box and fascia fabrication

• Engraving surface detail on display panels

Advantages:

• Produces sharp, clean engraved lettering and decorative lines

• The varying depth of cut automatically adjusts to letter width, producing naturally tapered lines that look hand-carved

• Versatile across many materials

• Available in a wide range of angles and tip styles

Limitations:

• Not suitable for through-cutting or pocketing operations

• The quality of V-carving depends heavily on the accuracy of the machine's Z-axis — any surface variation in the material will affect carving depth consistency

For sign shops using our 6090 CNC router or 1325 CNC router for wood sign production, the 60° V-bit is typically the most frequently used engraving tool. CAM software such as Vectric VCarve Pro is specifically designed to generate V-carving toolpaths that take full advantage of this bit geometry.

Recommended starting parameters for MDF:

• Spindle speed: 18,000–24,000 RPM

• Feed rate: 3,000–6,000 mm/min

• Depth of cut: Controlled by toolpath software based on letter geometry

2.4. Ball-Nose Bit

The ball-nose bit has a hemispherical cutting tip that produces smooth, curved surface cuts. It is the standard tool for 3D surface machining, relief carving, and any operation that requires a smooth curved surface finish.

Best materials:

• MDF

• Solid wood

• HDU foam

• Plywood

• Soft metals (with appropriate grades)

Typical applications:

• 3D relief carving for decorative panels and signs

• Dimensional lettering and carved artwork

• Surface finishing passes after roughing with a straight bit

• Organic shape machining for furniture components and architectural elements

• Carving decorative cabinet door panels

Advantages:

• Produces smooth, curved surface finishes

• Essential for 3D relief work and organic shapes

• Available in a wide range of diameters for different levels of surface detail

• Smaller diameter ball-nose bits produce finer surface detail; larger diameters cover area faster

Limitations:

• Slower material removal rate than straight bits — typically used for finishing passes rather than roughing

• Requires 3D CAM software (such as Vectric Aspire or Type3) to generate proper 3D toolpaths

• Fine detail work with small diameter bits requires slow feed rates and multiple passes

Choosing ball-nose bit diameter:

• 0.5mm–2mm — Very fine surface detail, slow feed rates, used for intricate relief work

• 3mm–6mm — Standard range for detailed 3D carving and dimensional sign work

• 8mm–12mm — Faster area coverage for larger relief panels and architectural carving

For businesses using our wood CNC routers for decorative carving and 3D relief work, a set of ball-nose bits in 3mm, 6mm, and 12mm diameters covers most applications from fine detail to large-area finishing.

Recommended starting parameters for MDF (6mm ball-nose finishing pass):

• Spindle speed: 18,000–22,000 RPM

• Feed rate: 2,000–4,000 mm/min

• Stepover: 10–20% of bit diameter for smooth surface finish

2.5. Single-Flute O-Flute Bit (for Acrylic and Plastics)

The single-flute O-flute bit is specifically designed for cutting acrylic (PMMA), PVC, polycarbonate, and other thermoplastic materials. The O-flute geometry — a single large, rounded flute channel — provides maximum chip clearance and prevents the heat buildup that causes plastics to melt and re-weld behind the cutter.

Best materials:

• Acrylic (PMMA)

• PVC foam board

• Polycarbonate

• PETG and other thermoplastics

• Soft aluminum (with appropriate grades)

Typical applications:

• Acrylic letter cutting for channel letters and backlit signs

• PVC foam board profiling for display signs

• Cutting acrylic sheet for display cases and retail fixtures

• Profiling polycarbonate panels

Advantages:

• Prevents melting and re-welding in thermoplastic materials

• Produces clean, polished cut edges in acrylic

• Single-flute design maximizes chip clearance at high spindle speeds

• Significantly longer tool life in plastics compared to standard woodworking bits

Limitations:

• Not designed for wood or MDF — the geometry is optimized for plastics

• Requires high spindle speed and appropriate feed rate to work correctly

• More expensive than standard woodworking bits

Why standard woodworking bits fail in acrylic:

Standard two-flute upcut bits do not clear chips fast enough in acrylic. The chips re-melt and weld back to the cut edge, producing a rough, frosted appearance instead of a clean, polished edge. The O-flute geometry solves this by providing a much larger chip channel that evacuates material before it can re-melt.

For sign shops cutting acrylic on our 6090 CNC router or 1325 CNC router, the single-flute O-flute bit is non-negotiable for professional-quality acrylic edges.

Recommended starting parameters for 10mm acrylic:

• Spindle speed: 18,000–24,000 RPM

• Feed rate: 2,000–4,000 mm/min

• Depth of cut per pass: 2–4mm

• Coolant: Air blast recommended to assist chip evacuation

2.6. Straight Downcut Spiral Bit

The straight downcut spiral bit pushes chips downward into the cut rather than pulling them upward. This produces a clean, chip-free edge on the top surface of the material, making it useful for operations where the top face finish quality is the priority.

Best materials:

• Veneered plywood

• Solid wood panels

• Softwood where top-face tearout is a concern

• Thin sheet materials

Typical applications:

• Shallow surface routing where top-face finish is critical

• Routing veneered panels where the veneer surface must remain chip-free

• Decorative surface work on solid wood furniture components

Advantages:

• Clean, chip-free top surface finish

• Useful for veneered materials where the top face is the show face

Limitations:

• Poor chip evacuation — chips are pushed into the cut, generating heat

• Not suitable for deep through-cutting or pocketing operations

• Can cause tearout on the bottom face of the material

In practice, the downcut bit is used less frequently than upcut or compression bits in production woodworking. For most applications involving laminated panels, the compression bit is a better solution because it produces clean edges on both faces simultaneously.

2.7. Surfacing Bit (Spoilboard Cutter)

The surfacing bit — also called a spoilboard cutter or fly cutter — is a large-diameter bit used to skim the surface of the machine's spoilboard flat and level. It is not used for workpiece cutting but is an essential maintenance tool for any CNC router.

Typical applications:

• Resurfacing the MDF spoilboard after it has been cut into during production

• Flattening a warped or uneven spoilboard

• Preparing a fresh spoilboard surface for vacuum table use

Why spoilboard maintenance matters:

The spoilboard is the sacrificial MDF sheet that sits on top of the machine table and protects the table surface during through-cutting operations. Over time, the spoilboard accumulates cut lines and becomes uneven. An uneven spoilboard causes inconsistent cutting depth across the sheet, which affects edge quality and dimensional accuracy.

Regular resurfacing with a spoilboard cutter keeps the working surface flat and ensures consistent cutting depth across the full working area of the machine.

For machines used in high-volume cabinet and panel production — such as our 1325 wood CNC router — spoilboard resurfacing should be performed regularly as part of the machine maintenance schedule. For more detail on machine maintenance best practices, see our guide on CNC router maintenance tips.

Recommended parameters for spoilboard surfacing:

• Spindle speed: 12,000–18,000 RPM

• Feed rate: 4,000–8,000 mm/min

• Depth of cut: 0.3–1.0mm per pass

2.8. Drill Bits for CNC Routers

CNC router drill bits are used for drilling dowel holes, shelf pin holes, hinge cup holes, and cam lock fitting holes in cabinet panels. Unlike conventional drill bits, CNC router drill bits are designed to run at the high spindle speeds of a CNC router spindle.

Typical applications:

• Dowel hole drilling for cabinet assembly

• Shelf pin hole rows in cabinet side panels

• Hinge cup drilling for concealed hinges

• Cam lock and confirmat fitting holes

• Through-holes for cable management and hardware

Types of CNC drill bits:

• Brad point drill bits — Produce clean entry holes with minimal tearout, preferred for visible faces

• Twist drill bits — General-purpose drilling, widely available in standard diameters

• Forstner-style bits — Used for flat-bottomed holes such as hinge cup recesses

Important note on drilling with a CNC router:

Standard CNC router spindles are designed for high-speed rotary cutting, not the slower speeds typically used for drilling. When drilling with a CNC router, use bits specifically rated for high-speed operation and confirm that the spindle speed and feed rate are appropriate for the bit diameter and material.

For cabinet factories running dedicated drilling operations, a multi-spindle drilling head or a dedicated line boring machine may be more efficient than using the main CNC router spindle for all drilling work.

2.9. Diamond Drag Engraving Bit

The diamond drag engraving bit does not cut — it scratches. A spring-loaded diamond tip drags across the material surface under controlled pressure, scratching through surface coatings to reveal the substrate beneath.

Best materials:

• Aluminum composite panel (ACP/Dibond)

• Anodized aluminum

• Coated metals

• Acrylic with surface coating

• Brass and stainless steel (with appropriate tip)

Typical applications:

• Engraving text and logos on ACP sign panels

• Producing fine-line engraving on metal plaques and nameplates

• Scratching through anodized aluminum coatings for decorative effect

Advantages:

• No spindle speed required — the diamond tip drags at any speed

• Produces very fine, consistent line quality

• No chip generation or dust

• Long service life if the tip is not damaged

Limitations:

• Only works on materials with a distinct surface coating or color contrast

• Cannot produce variable-depth engraving

• Not suitable for cutting or profiling operations

Bit Selection by Material: Quick Reference

This section provides a quick reference for selecting the right bit type for the most common CNC router materials in woodworking and sign making.

3.1. MDF (Plain and Moisture-Resistant)

MDF is highly abrasive due to its resin content. Carbide bits are essential. Expect shorter tool life in MDF than in solid wood. Dust extraction is critical when cutting MDF — the fine dust is a significant health hazard.

3.2. Melamine-Faced Particleboard and MDF

The compression bit is the essential tool for melamine panel cutting. Using an upcut bit will chip the melamine surface and produce panels that require additional finishing or must be rejected.

3.3. Plywood (Hardwood and Softwood)

Plywood cuts well with standard upcut spiral bits. For veneered plywood where both faces must be clean, use a compression bit.

3.4. Solid Wood (Hardwood and Softwood)

Solid wood is generally less abrasive than MDF and produces better tool life. Grain direction affects cut quality — cutting against the grain can cause tearout in some species. Test feed rate and direction on scrap material before running production.

3.5. Acrylic (PMMA)

Never use standard woodworking bits for acrylic cutting in production. The O-flute single-flute bit is the correct tool. Spindle speed should be high (18,000–24,000 RPM) and feed rate should be moderate to fast to prevent heat buildup.

3.6. PVC Foam Board (Sintra/Forex)

PVC foam board cuts best at high speed and fast feed rate. Slow feed rates cause melting at the cut edge. Use a sharp bit and replace when the edge quality begins to deteriorate.

3.7. Aluminum Composite Panel (ACP/Dibond)

ACP consists of two thin aluminum skins bonded to a polyethylene core. Use bits designed for composite materials. Sharp tooling is essential — dull bits generate excessive heat in the aluminum skins.

3.8. HDU Foam (High-Density Urethane)

HDU foam carves beautifully and produces very fine surface detail. High spindle speed with light passes gives the cleanest results. Multiple finishing passes with a small ball-nose bit produce a smooth surface that requires minimal hand finishing.

Understanding Bit Life and When to Replace

Even the best carbide router bits wear out over time. Running a worn bit affects cut quality, increases spindle load, and can damage workpieces. Knowing when to replace a bit is as important as knowing which bit to use.

4.1. Signs That a Bit Needs Replacing

• Rough or fuzzy cut edges — The cutting edge is no longer sharp enough to shear cleanly

• Burning or scorching on the cut surface — The bit is generating excessive heat due to dull edges

• Increased spindle noise or vibration — A worn bit creates uneven cutting forces that cause vibration

• Chipping on laminated surfaces — A compression bit that was previously cutting cleanly is beginning to chip the surface

• Reduced feed rate required to maintain quality — Having to slow down to get acceptable results is a sign of bit wear

4.2. Factors That Affect Bit Life

• Material abrasiveness — MDF and particleboard are highly abrasive due to resin content and wear bits faster than solid wood

• Cutting parameters — Running at incorrect spindle speed or feed rate accelerates wear

• Depth of cut — Taking excessively deep cuts per pass puts more stress on the cutting edge

• Chip evacuation — Poor chip clearance causes chips to re-cut, accelerating edge wear

• Collet condition — A worn or dirty collet that does not hold the bit concentrically causes vibration and premature wear

4.3. Bit Life Expectations by Material

These are approximate guidelines — actual bit life varies significantly based on cutting parameters, machine condition, and bit quality.

Common Bit Selection Mistakes and How to Avoid Them

Mistake 1: Using an Upcut Bit on Melamine-Faced Panels

Problem: The upcut geometry chips the melamine surface, producing panels that must be rejected or require additional finishing.

Solution: Use a compression spiral bit for all through-cutting operations on melamine-faced MDF and particleboard.

Mistake 2: Using a Standard Woodworking Bit for Acrylic

Problem: Standard two-flute bits do not clear chips fast enough in acrylic. Chips re-melt and weld back to the cut edge, producing rough, frosted edges.

Solution: Use a single-flute O-flute bit specifically designed for acrylic and plastics.

Mistake 3: Running Too Slow a Feed Rate

Problem: Many operators reduce feed rate thinking it will improve cut quality. In most cases, too slow a feed rate causes the bit to rub rather than cut, generating heat, accelerating wear, and producing a worse surface finish.

Solution: Run at the recommended feed rate for the material and bit combination. Each flute should be taking a proper chip — not rubbing.

Mistake 4: Using the Wrong Collet Size

Problem: Using an adapter to run a bit with a mismatched shank diameter reduces rigidity and causes vibration, which affects cut quality and accelerates bit wear.

Solution: Use bits with shank diameters that match the collet on your spindle. If you regularly use bits with different shank sizes, invest in the correct collet for each size.

Mistake 5: Not Replacing Worn Bits Soon Enough

Problem: Running a worn bit to save money on tooling costs actually increases production costs through poor cut quality, material waste, and increased spindle load.

Solution: Monitor cut quality regularly and replace bits before quality deteriorates to the point of producing rejects.

Mistake 6: Ignoring Chip Evacuation

Problem: Chips that are not cleared from the cut zone re-cut the material, generate heat, and accelerate bit wear. This is particularly common when cutting deep pockets without adequate dust extraction.

Solution: Ensure your dust extraction system is working effectively. For deep pocketing operations, consider using a ramp entry toolpath rather than plunging straight down, which improves chip evacuation.

Tooling Setup: Getting the Best Performance from Your Bits

6.1. Collet Maintenance

The collet is the component that holds the bit shank in the spindle. A worn, dirty, or damaged collet can cause the bit to run off-center, producing vibration, poor cut quality, and premature bit wear.

• Clean the collet and collet taper regularly with a lint-free cloth

• Inspect the collet for wear or damage and replace if necessary

• Never overtighten the collet nut — use the correct torque as specified by the spindle manufacturer

• Replace collets periodically even if they appear undamaged — collets wear gradually and lose their grip precision over time

6.2. Tool Length Setting

Accurate tool length setting ensures that the cutting depth is correct and that the machine's Z-axis reference is accurate. Most CNC routers use a tool length sensor or a manual touch-off procedure to set the tool length.

• Set the tool length accurately before each job or after each tool change

• If using an ATC spindle, verify that the tool length sensor is calibrated correctly

• Inconsistent cutting depth across a panel is often caused by inaccurate tool length setting rather than a machine problem

6.3. Runout

Runout is the amount by which the bit tip deviates from true center as the spindle rotates. Even small amounts of runout — as little as 0.05mm — can significantly affect cut quality, surface finish, and bit life.

• Check spindle runout periodically using a dial indicator

• A worn or damaged spindle bearing is the most common cause of excessive runout

• A damaged or worn collet can also cause runout even if the spindle bearing is in good condition

For guidance on spindle maintenance and how to identify spindle problems early, see our article on CNC router maintenance tips.

Building a Practical Bit Kit for Your Application

Rather than buying bits individually as needed, building a practical bit kit for your specific application ensures you always have the right tool available without overstocking.

7.1. Starter Bit Kit for Cabinet Making

This kit covers the majority of cabinet panel cutting, hardware drilling, and edge detailing operations for a production cabinet shop using a 1325 wood CNC router.

7.2. Starter Bit Kit for Sign Making

This kit covers acrylic letter cutting, wood sign V-carving, 3D dimensional sign work, and ACP engraving for a sign shop using a 6090 CNC router or 1325 CNC router.

7.3. Starter Bit Kit for General Woodworking

This kit covers the majority of operations for a general woodworking shop producing a mix of furniture components, decorative panels, and custom pieces.

Conclusion

Choosing the right CNC router bit is not a minor detail — it is a fundamental part of getting consistent, professional-quality results from your machine. The right bit for the right material and operation produces cleaner cuts, longer tool life, less material waste, and lower production costs over time.

The key principles to remember are:

• Use compression bits for all through-cutting on melamine-faced and laminated panels

• Use O-flute single-flute bits for acrylic and thermoplastic cutting

• Use V-bits for engraved lettering, sign carving, and decorative line work

• Use ball-nose bits for 3D relief carving and smooth surface finishing passes

• Use upcut spiral bits as the general-purpose workhorse for MDF, plywood, and solid wood

• Always use solid carbide bits for production CNC work

• Replace bits before they are worn to the point of affecting output quality

If you are setting up a new wood CNC router for cabinet making, sign making, or general woodworking, investing in the right tooling from the start will make a significant difference to your daily production results.

For questions about machine configuration, spindle specifications, or compatible tooling for specific applications, browse our Wood CNC Router product category or contact us with details about your materials and production requirements. Our team can advise on both machine selection and the tooling setup that will work best for your application.

Frequently Asked Questions

What is the best CNC router bit for cutting MDF?

For plain MDF, a two-flute upcut spiral carbide bit is the standard choice for through-cutting and pocketing. For melamine-faced MDF, use a compression spiral bit to produce chip-free edges on both faces.

What router bit should I use for cutting acrylic?

Use a single-flute O-flute upcut bit specifically designed for acrylic and plastics. Standard woodworking bits do not clear chips fast enough in acrylic and cause the material to melt and re-weld at the cut edge.

What is a compression bit and when should I use it?

A compression bit combines an upcut section at the tip with a downcut section above it, cutting cleanly from both the top and bottom faces of the material simultaneously. It is the correct bit for cutting melamine-faced particleboard, melamine MDF, and laminated panels where both faces must be chip-free.

How long do CNC router bits last?

Tool life varies significantly depending on material, cutting parameters, and bit quality. In MDF, a quality carbide upcut bit typically lasts 15–30 hours of cutting time. In solid wood, life is longer — 50–100 hours. In acrylic with an O-flute bit, expect 30–60 hours. MDF and particleboard are the most abrasive materials and wear bits fastest.

What is the difference between upcut and downcut router bits?

An upcut bit pulls chips upward and out of the cut, producing clean bottom-face edges but potential tearout on the top face. A downcut bit pushes chips downward, producing a clean top-face edge but poor chip evacuation. For most woodworking production, upcut bits are preferred for their chip clearance. For laminated panels, compression bits are the better solution.

What shank size do I need for my CNC router?

The shank size must match the collet on your machine's spindle. Common sizes are 6mm, 8mm, and 12mm in metric markets, and 1/4 inch and 1/2 inch in North American markets. Check your spindle's collet specification before ordering bits.

Setting up a new CNC router and need tooling advice?

Contact our team with details about your materials and production requirements, and we will recommend the right machine configuration and tooling setup for your application. Contact us today.