Select Your Machine

Quickstart Guide

Five minutes from download to your first calculated cut. Here's how every piece fits together.

What This App Does

ToolPath Advisor is a single-file CNC reference tool for small-shop makers. It helps you choose the right bit, calculate feeds and speeds for your specific machine, look up G-codes, check material properties and dust hazards, and run a pre-flight checklist before every job. Everything runs in your browser — no install, no account, no internet needed after download.

Step 1: Set Up Your Profile

The first time you open the app, a setup wizard asks four questions:

Your profile saves to your browser automatically. Next time you open the app, you skip straight to work. Change your profile anytime using the button in the top-right corner.

Step 2: The Tab Bar

The app is organized into eight tabs across the top. Here's what each one does:

Step 3: Your First Calculated Cut

The fastest path to a real result:

1. Go to the Feeds & Speeds tab.

2. Select your material (e.g., "Hardwood — Soft" for walnut or cherry).

3. Select your operation (e.g., "Pocket").

4. Select your bit, or add a custom bit using the "My Bits" section.

5. Check the chip load gauge — the needle should land in the green "OK" zone.

6. Adjust with sliders if needed. Advisory notes appear when something needs attention.

7. Click "Copy for CAM" — formatted values go to your clipboard, ready for Fusion 360, VCarve, or whatever you're using.

8. The job auto-logs in the Log tab for future reference.

Getting the Most Out of the App

Check Materials before cutting an unfamiliar species. The dust hazard ratings and CNC tips can save you a respiratory problem and a ruined workpiece.

Run Pre-Flight on new jobs. The mistakes that break bits and ruin stock happen in the first five minutes. The checklist catches them.

Use the Job Log. It feels like overhead at first, but after a few months you'll have a library of proven settings for your machine. That's worth more than any calculator.

Read the Learn articles when you have time. Start with "Chip Load" — understanding that one concept changes how you think about everything else.

Data & Privacy

Everything stays in your browser. Profile, custom bits, and job log are stored in local storage. Nothing is sent anywhere — no server, no analytics, no tracking. Clear your browser data and you'll go through the wizard again. Export your job log to CSV anytime from the Log tab.

From Sawdust to G‑Code

50 years of making. Here's what changes when a computer runs the router — and what doesn't.

There's a moment every experienced woodworker hits with their first CNC machine. You've spent years developing feel — the sound of a sharp bit, the grain reading that happens before your eyes do. And then you're staring at a screen entering numbers.

That instinct doesn't go away. You just need a new language for it.

I started making things in the early 1970s. Cabinet making, furniture and millwork, custom guitars. Forty years running software companies alongside all of it — which is probably why I ended up building tools that translate craft knowledge into something a computer can act on.

Every number I enter at the CNC — RPM, feed rate, depth of cut — is a translation of something I already know from hand tools. How hard is this wood? How will this grain behave under a spinning cutter? What does tearout look like before it happens?

New CNC users get handed a machine and told to find feeds and speeds on a forum. They get numbers with no context — no explanation of why, no sense of what happens when the machine or material is different. They crash bits. They assume they're doing something wrong when often they're just missing the reasoning.

That's what ToolPath Advisor is for. Not just the numbers — the reasoning.

Start with chip load. Everything else follows from there.

Chip Load — The One Number That Rules Them All

Chip load is the thickness of material each flute removes per revolution. Get this right and everything else follows. Get it wrong and you're burning bits, ruining surfaces, or both.

Most CNC beginners focus on RPM. It's the most visible number — it's on the router dial, it's what people argue about on forums. But RPM alone tells you almost nothing about whether your cut is right.

Chip load is the number that actually matters.

Why Too-Light Chip Load Is Dangerous

When the chip is too thin, the bit isn't really cutting — it's rubbing. Friction builds. Heat builds. The bit dulls faster than it should, the wood burns, and the surface looks terrible. Beginners see this and slow down further, which makes everything worse.

A proper chip carries heat away from the cut. No chip, no heat removal.

Why Too-Heavy Chip Load Breaks Things

Too much chip load overloads the flutes. On a low-rigidity machine — an MPCNC or stock X-Carve — this causes deflection: the bit bends slightly away from the cut, leaving a surface that isn't square and dimensions that aren't accurate. Push it further and the bit snaps.

Material Changes Everything

Softwood wants a heavier chip load than hardwood. MDF wants more than solid wood. Aluminum wants far less than wood. The formula gives you the number — the material tells you whether that number is right.

This is where hand-tool experience pays off directly. You already know that routing end grain in maple is not the same as routing long grain in pine. The chip load targets are different because the material behaves differently under a cutter.

Climb vs. Conventional Milling — Which Direction and Why

Cut direction is as consequential as speed or feed. Running the wrong direction for your machine won't just hurt surface finish — it can grab the bit, break it, or pull your workpiece off the table.

What's Actually Happening

The bit spins. That part doesn't change. What changes is the relationship between that spin and the direction the router is moving. Point a spinning endmill along the edge of your workpiece and feed it in one direction — the flutes either bite into fresh material on the way in (cutting) or scrape their way out (rubbing). Those two behaviors have completely different consequences for surface quality, heat, and machine stress.

In a top-down view, the endmill rotates clockwise (standard right-hand flutes). If you're moving the bit from right to left along the top edge of a workpiece, the left side of the bit is cutting into the wood. Whether that's climb or conventional depends entirely on which way you're feeding relative to that rotation.

Climb Milling (Down Milling)

In climb milling, the bit rotates in the same direction as the feed. The flute meets the workpiece at full chip thickness and exits thin. This is the cut starting fat and finishing lean.

Because the chip starts thick, the cutting edge is genuinely cutting from the first contact — no rubbing, no skating. The chip carries the heat out with it. The result is a cleaner surface, less heat in the workpiece, and less wear on the bit per pass.

The downside is mechanical: climb milling creates a force that pushes the bit in the direction of feed. On a machine with backlash — any slop in the drive system — that push can cause the bit to lunge forward, digging deeper than intended. On a solid ball-screw machine, this isn't an issue. On a flexible machine with a lead screw or worn drive nuts, it can be.

Conventional Milling (Up Milling)

In conventional milling, the bit rotates against the feed direction. The flute enters the material thin — nearly zero chip thickness — and exits thick. That thin entry means the cutting edge is initially rubbing, not cutting. Friction runs higher, more heat stays in the workpiece, and the surface is rougher than climb.

Why ever use it? Because the cutting forces push the bit away from the feed direction, not with it. On a machine with backlash, that outward push keeps everything loaded in one direction and prevents the lunge. It's also more forgiving on low-rigidity machines where the frame itself flexes under cutting forces.

Conventional also works better in two specific material situations: cutting through hardened or scaled surfaces (the thin entry chip doesn't hammer the edge against a hard skin) and cutting some plastics where climb milling creates burrs on the exit side.

For Your Machine

The right default depends entirely on your drive system, which is stored in your machine profile. If ToolPath Advisor shows ball screws, climb milling is the right default for finish passes. If it shows a lead screw — or if you're on an MPCNC, an older X-Carve, or anything with a Delrin anti-backlash nut — conventional is the safer default, or limit climb to a very shallow stepover.

Upcut, Downcut & Compression — Choosing the Right Spiral

The Tool Recommender suggests bit types, but understanding why matters when you override or when the material is unusual. Spiral direction isn't a minor preference — it changes the surface quality, chip evacuation, and workholding forces on every cut you make.

The Spiral Direction

All three types are spiral endmills — the same basic geometry as a drill bit or router bit. The difference is which direction the flutes are twisted, and therefore which direction the cutting action pushes chips: upward, downward, or both at once.

That chip direction matters more than most beginners expect. It controls surface quality on both faces of your workpiece, heat buildup in the slot, and whether the bit pulls the workpiece off the table or pushes it down onto it.

Upcut (Up Spiral)

The flutes spiral upward, so the cutting action throws chips up and out of the slot — exactly like a drill bit ejecting material from a hole. The bottom surface of the workpiece gets a clean, sharp edge because that's where the cutter is doing its best work. The top surface is the exit side, where fibers or veneers can lift and fray before the bit shears them cleanly.

Upcut is the most versatile bit for general CNC routing. It handles deep pockets well because chips evacuate naturally. Hard plastics and aluminum both benefit from the aggressive chip clearance — chip re-cutting is the enemy in those materials, and upcut minimizes it. The caution is workholding: the spiral geometry creates an upward force on the workpiece with every pass. Strong vacuum, clamps, or both.

Downcut (Down Spiral)

Flutes spiral downward, pushing chips back into the slot rather than ejecting them. The top surface is where the cutter enters, and the downward action compresses the fibers and veneer against the workpiece instead of lifting them. Result: a very clean top edge with no tearout. The bottom surface takes the exit side, which is rougher.

The problem is chip evacuation — or rather the lack of it. Every chip you make stays in the slot, getting recut on subsequent passes. Heat builds fast. In hardwood or deep cuts this accelerates dulling significantly. The rule of thumb is to keep depth of cut around ¼ of the bit diameter per pass, and use air blast if you have it. Not the right bit for deep pockets or hard plastics.

Downcut shines for: plywood and veneer faces where top tearout ruins the part, thin materials that would lift under upcut force, engraving passes, and any operation where the top surface is the finished face.

Compression

A compression bit combines both spirals in one tool: the bottom portion of the flute is upcut, the top portion is downcut. Done right, this gives you clean edges on both faces simultaneously — the upcut section cleans the bottom, the downcut section cleans the top.

The catch is geometry. The upcut section at the tip is typically ½ to ⅔ of the bit diameter in length. For the compression effect to work, your first pass must go deep enough that the upcut section is actually cutting — if you only engage the downcut portion, you get a downcut bit. This means compression bits are essentially a through-cut tool. They're not useful for pocketing, because you can't run them at their required depth in the middle of a pocket without cutting through.

Best applications: through-cuts in plywood, melamine, and laminate where both faces need to be clean. Exactly the kind of cuts that come up constantly in cabinet and furniture work.

Depth of Cut vs. Stepover — Balancing the Engagement Equation

The F&S Calculator gives you depth of cut and stepover, but most users don't understand the tradeoff. These two numbers together define how much material each pass removes — and getting the balance wrong wastes time or breaks bits.

What They Control

Depth of cut (axial) is how deep each layer goes — how far the bit plunges into the material per pass. Stepover (radial) is how wide each pass is — how much of the bit's diameter is engaged with fresh material. Together they form an "engagement rectangle": the cross-section of material being removed per pass. That rectangle is the foundation of everything else in your cut settings.

The Tradeoff

For a given bit and machine, there's a total engagement limit. You can go deeper and narrower, or shallower and wider — the volume removed per unit time can be the same either way. But the forces are different.

Deeper and narrower engages more of the flute length simultaneously. That spreads heat across more cutting edge — better for tool life — but it also increases axial side load on the bit. Shallower and wider reduces axial load but increases radial force and introduces chip thinning once you drop below 50% of bit diameter.

Chip Thinning — The Hidden Trap

When stepover drops below 50% of bit diameter, the actual chip removed is thinner than the programmed chip load. The geometry of the arc of engagement compresses the chip. At 25% stepover, the actual chip can be 30–40% thinner than the number your calculator shows. That means the bit is rubbing more than cutting — heat builds, the edge dulls prematurely, and surface quality drops.

The F&S Calculator in this app accounts for chip thinning automatically based on your stepover setting. If you're manually adjusting stepover downward, you need to increase feed rate to compensate — effective chip load decreases as stepover decreases, and you must push feed rate up to restore it.

Rules of Thumb for Hobby Machines

MPCNC and low-rigidity machines: prefer wider stepover (40–50% of bit diameter) with shallow DOC (25–50% of diameter). The frame flex and spindle runout on these machines punish deep cuts harder than they punish wide ones.

Ball-screw machines (Onefinity, Carvera): can handle deeper DOC (75–100% of diameter) with narrower stepover (25–35%). The increased rigidity lets you use more flute length without losing dimensional accuracy.

For roughing: maximize MRR — use the widest stepover and deepest DOC your machine can hold without deflection. For finishing: use 10–15% stepover for a smooth surface. The tiny engagement leaves very little scallop height.

Rigidity & Tool Deflection — Why Your Machine Is the Limit

The Bit Override Score factors in machine rigidity, but most users don't understand what deflection actually does to their parts. Every CNC machine flexes under load. The question is how much — and whether that flex ruins your cut.

What Deflection Does

Under cutting forces, the bit acts like a cantilever beam — it bends away from the cut. Even 0.001″ of deflection at the tip means your dimensions are wrong, your walls aren't square, and tool life drops dramatically. Harvey Performance data puts that number in stark terms: 0.001″ of deflection equals a 40% reduction in tool life. On hobby machines, deflection can be 5–10× worse than on industrial machines. The cut that looked fine in simulation is failing in physics.

Where Flex Comes From

It's not just the bit. Flex can originate from anywhere in the mechanical chain: (1) the bit itself — longer stickout means exponentially more flex; (2) the collet and spindle mount; (3) the Z-axis assembly; (4) the gantry; (5) the table and spoilboard. On an MPCNC with conduit rails, the gantry is typically the weakest link. On a Shapeoko, it's often the Z-plate. Every joint in the chain is a potential source of compliance, and they all add up.

The whole chain matters. A great collet mounted to a flexy gantry still deflects. This is why machine class matters as much as bit selection.

Practical Rules

Minimize stickout. Only extend the bit as far as the cut requires, plus ~3mm clearance. Every millimeter beyond that is deflection you're paying for in accuracy.

Use the largest diameter your operation allows. Diameter fights deflection with a fourth-power advantage. Going from 1/8″ to 1/4″ gives you 16× more stiffness, not 2×.

Reduce cutting forces on long-reach operations. Lighter depth of cut and slower feed are not conservatism — they're compensation for physics you can't engineer away.

Step down in small increments for deep operations. Guitar neck pockets, deep mortises, tall profiles — these require patience. Full-depth passes on a hobby machine will deflect and chatter. Small steps stay in control.

How the App Helps

The machine profile wizard captures your machine's rigidity class — industrial, semi-pro, or hobby. The Bit Override Score uses that class to penalize long stickout and small diameter combinations. A low override score almost always traces back to a deflection problem.

The fix is almost always one of three things: shorter stickout, fatter bit, or lighter engagement. The app will tell you which lever matters most for your specific combination of machine, bit, and material.

The Pre-Flight Checklist — Before You Hit Start

Most broken bits and crashed jobs trace back to skipped steps before the cut even started. This checklist isn't bureaucracy — it's the fastest way to stop wasting material and bits.

In CAM (Before You Post)

Start before you ever touch the machine. Open the simulation and work through these four things in order.

First: verify your zero point matches your physical setup. If you zeroed in CAM to the corner of the stock, your machine zero has to be the same corner — not the center of the bed, not a reference pin. A mismatch here cuts air on one side and air on the other, until it doesn't.

Second: confirm you've selected the correct post-processor for your controller. GRBL, Mach3, LinuxCNC, and UCCNC all speak slightly different dialects. Posting for the wrong controller is one of the more baffling failures you'll encounter because the machine moves — it's just doing the wrong thing.

Third: run the toolpath simulation and watch for plunge moves that don't match your step-down, and for rapids that pass through the material. CAM software will let you program that. The simulation catches it before the machine does.

Fourth: check that your depth of cut per pass doesn't exceed what your bit can handle. The ToolPath Advisor's Feeds & Speeds calculator shows recommended DOC for your bit diameter and material — use it as a ceiling, not a target.

At the Machine

Clean the collet before every tool change. A brass brush or a short burst of compressed air removes chips and debris that cause runout. Runout means the bit wobbles as it spins — even 0.05mm of runout multiplies into surface quality problems and accelerated wear.

Seat the bit properly. Never bottom out the shank in the collet — leave a 2–3mm gap at the bottom. The collet grips the shank along its length; contact at the bottom can push the bit out under cutting load. Then set the collet nut firmly by hand before using the wrench. Snug, not gorilla-tight.

Verify stickout matches what you set in CAM. If your CAM model assumed 25mm of stickout and you've got 40mm hanging below the collet, you have a deflection problem waiting to happen. Shorter is stiffer. Only extend what you need to reach the cut depth.

Secure the workpiece, then do the push test. Push the material by hand — firm lateral pressure in multiple directions. If it moves even slightly, it will move under cutting force, and cutting force is orders of magnitude higher than your hand. Fix it now.

Set Z-zero with your touch plate or the paper method, then repeat it once. Two consistent readings mean you've got it. A discrepancy means something shifted between attempts — find it before you run.

First Run Protocol

For any new job or any material you haven't run in this setup before: raise Z 10mm above the stock surface and run the program as an air cut. Watch the machine move through the full toolpath. Ugly surprises happen during air cuts where they're free.

When you're ready to cut for real, start with the feedrate override at 50%. Listen and watch the first few seconds — the sound of the first engagement tells you a lot. If it sounds clean and the chips look right, bring the override to 80%. Let the first toolpath complete at 80%. Only push to 100% after you've seen the full cut behave.

This isn't timidity — it's information gathering. A new piece of stock in a species you've run before can still have a knot or a density change that rewards caution on the first pass.

Reading the Cut — What Chips, Sound & Surface Tell You

The chip load article explains the theory. This article teaches you to diagnose problems in real time — while the machine is still running and you can do something about it.

Read the Chips

Good chips are small consistent curls or comma-shapes — warm to the touch but not hot. When you pick one up between your fingers and it feels like room-temperature wood shaving, the cut is working.

Dust instead of chips means the feed is too slow or the bit is dull. You're rubbing, not cutting. This is the most common mistake among new CNC operators: they see the machine moving and assume it's cutting. Rubbing generates heat without removing material efficiently, and that heat goes somewhere — into the bit, into the wood, into your surface finish.

Large irregular chunks mean the feed is too fast or the depth of cut is too aggressive. The flutes are overloading before they can clear. Reduce feed or DOC and the chip size normalizes.

Stringy or melted chips in plastics mean the heat isn't evacuating — feed faster, increase chip clearance, or switch to a single-flute bit designed for plastics.

Color tells you about heat. Wood chips that are noticeably darker than the raw material are showing you that heat built up in the cut. The wood scorched before the chip could carry the heat away. Increase feed rate, check bit sharpness, or reduce RPM.

Listen to the Cut

A healthy cut has a consistent, low-frequency hum. It sounds like work being done. Learn that sound on a job you know is dialed in, and it becomes a reference point for everything else.

A high-pitched whine or squeal is chatter — the bit is deflecting and vibrating harmonically. The fix is usually to change RPM by 10–15% in either direction (you're trying to move off the resonant frequency) or reduce depth of cut. If neither helps, look at stickout — a bit extended too far is the most common cause of persistent chatter on hobby machines.

Grinding or growling means something is fundamentally wrong: the bit is dull, you've hit a fastener in the stock, or you're asking the cut to do something it can't. Stop the cut. Don't push through a grinding cut hoping it resolves.

Intermittent knocking — a rhythmic or irregular thump — usually means the workpiece has shifted or there's backlash in a drive axis. Workpiece movement during a cut is an immediate stop condition. A fastener left in the stock sounds similar and is equally urgent.

Sound changes when the bit enters a knot or cross-grain. That's normal and usually brief. But if an unusual sound persists beyond the anomaly, it warrants investigation — slow the feedrate override and assess.

Read the Surface

Burn marks are the most readable diagnostic in wood. They mean the bit was in contact with the surface long enough to scorch it — feed too slow, bit too dull, or RPM too high for the feed rate. Increase feed, check sharpness, or slow RPM proportionally.

Fuzzy or hairy edges on plywood typically mean you're using an upcut bit where a downcut is needed. The upcut geometry pulls fibers up through the top surface. Switch to a downcut spiral for plywood and laminated sheets where top surface quality matters. A dull bit on any material produces similar fuzz.

Washboard ripples across the surface — a regular pattern of undulation — are chatter. The bit is vibrating in a consistent pattern as it moves. Reduce depth of cut, shorten stickout, or change RPM until the ripples disappear.

Dimensional inaccuracy — a slot that's 0.3mm too wide, a pocket that's 0.2mm too deep — usually means deflection or a calibration issue. Deflection pushes the bit away from the cut during side walls, then it springs back. Run a finishing pass at full depth with a light stepover and the dimension corrects itself.

A rough pocket bottom, especially with downcut bits in deep pockets, means you're re-cutting chips that have nowhere to go. Increase chip clearance passes or switch to an upcut bit for roughing inside pockets.

The Feedrate Override Save

The feedrate override dial on your controller is a diagnostic instrument, not just a convenience. When something looks or sounds wrong mid-cut, drop it to 50% and watch what happens.

If the problem gets worse when you slow down — more burning, higher-pitched sound, more dust — the feed was already too slow. The override just confirmed it. Bring it back up past the original setting.

If the problem improves, you were running too aggressively for the conditions. Stay at the lower rate, finish the cut, and recalculate before the next job.

This takes the guesswork out of in-cut adjustments. You're running a controlled test with a machine that's still in the material — use it.

Workholding for Small-Shop CNC — Clamps, Tape, Tabs & Vacuum

The best feeds and speeds in the world mean nothing if the workpiece moves. Workholding is the foundation everything else sits on — and in a small shop, you rarely have the luxury of custom fixtures for every job.

Screw-Down

The simplest method and the most reliable for anything with some bulk to it. Drill sacrificial through-holes in the material at corners or along the perimeter, drive screws down into the spoilboard, and the workpiece isn't going anywhere.

Use flat-head screws and countersink the holes so the head sits flush or below the surface. The bit doesn't know there's a screw there — it will find it if it's proud. Map every screw location in CAM before you post and verify no toolpath passes within 5mm of a fastener.

Best for roughing, prototyping, and any job where the screw holes will be machined away or end up in a hidden face. It's ugly, it works, and it's essentially foolproof under heavy cutting loads.

Blue Tape and CA Glue

This is the small-shop workhorse for finish parts. Apply blue painter's tape to the spoilboard surface, apply blue tape to the bottom face of the workpiece, then put CA glue (cyanoacrylate — standard superglue) between the two tape layers and press the workpiece down for 30–60 seconds. The tape-to-tape bond is strong enough to resist most lateral cutting forces and releases cleanly when you're done — peel up, no residue, no hole.

Best for thin materials, parts where screw holes would compromise the workpiece, engraving, two-sided machining where you need to flip without leaving marks, and anything that needs to look good all the way around.

Limitations: the tape-and-CA bond has a finite shear strength. Aggressive profile cuts with high lateral force — especially with large-diameter bits at full DOC — can shear the tape. If you're not sure, do the push test after bonding before you run. And don't use it on rough or dusty surfaces; the tape won't bond to a surface it can't contact fully.

Holding Tabs

Tabs are bridges of uncut material that your CAM software leaves in place during profile cuts to keep the part tethered to the surrounding stock. They're not a substitute for workholding — they work alongside your primary hold — but they're essential for any through-cut where the finished part would otherwise be free to move before the toolpath ends.

Tab width should be 2–3× the bit diameter. A 6mm bit warrants 12–18mm tabs. Tab height of 1–2mm is enough — you want them to hold, not to be a cleanup project. Too tall and you're sanding or filing for ten minutes per part.

After cutting, snap or saw the tabs free and sand the break points flush. On tight-grained hardwood they snap cleanly. On plywood they sometimes want a saw cut to avoid tearout — read the material before you force it.

Critical point: upcut bits generate upward axial force on the workpiece throughout the cut. When the profile is 95% complete and only the tabs are holding, that upward pull becomes the dominant force. On a lightweight part with an upcut bit, even well-bonded tape can lose the battle. Use tabs any time you're profiling through with an upcut spiral.

DIY Vacuum

A simple vacuum fixture — a manifold routed into a sacrificial spoilboard connected to a shop vac — can provide excellent hold for flat sheet goods. Large, flat workpieces that seal well against the spoilboard (MDF is ideal, smooth plywood works) get held uniformly across the entire surface, which eliminates the bow and buckle you sometimes get with perimeter clamping only.

For light cuts in sheet goods — 2D profiles, pockets, engraving — a shop vac pulling through a simple grid of channels delivers enough force. It's not practical for 3D carving where the workpiece area changes as material is removed, for small parts that don't cover enough of the manifold to seal, or for aggressive cuts with high lateral force.

The investment is modest: a few hours to route the spoilboard channels and a fitting to connect your shop vac. The payoff is fast, clamp-free setups on sheet goods you run repeatedly.

G-Code Demystified — The 10 Commands You'll Actually Use

You don't need to write G-code from scratch — your CAM software does that. But understanding what the machine is reading turns mysterious crashes into diagnosable problems, and lets you make small edits without re-posting.

The Basics

G-code is a plain text file. Each line is one instruction. The machine reads them top to bottom, executes each one, moves to the next. That's it. No loops, no branching — just a list of commands in order.

The letters tell you what kind of instruction it is: G for geometry and motion, M for machine functions (spindle, coolant, program control), F for feed rate, S for spindle speed, and X/Y/Z for coordinates. A number always follows each letter. G1 X6 F72 means: linear cut move, go to X=6, at 72 inches per minute.

The 10 Commands That Matter

Out of the hundreds of G and M codes that exist, these are the ones you'll see in nearly every program your CAM software posts:

G0 — Rapid move. The machine travels to the given coordinates as fast as it can. This is repositioning — not cutting. No material should be in the way during a G0 move.

G1 — Linear feed move. A straight-line cut at the commanded feed rate (F). This is the workhorse — most of your actual cutting happens on G1 lines.

G2 / G3 — Circular arc, clockwise and counterclockwise. Used for curves and circles. The I and J values define the arc center relative to the start point. Your CAM handles these automatically for any curved toolpath.

G17 / G18 / G19 — Plane selection: XY, XZ, or YZ. G17 (XY plane) is the default for routers. You'll rarely change this.

G20 / G21 — Unit selection. G20 = inches. G21 = millimeters. One wrong unit code means every coordinate in the program is interpreted in the wrong unit. A move meant to travel 1 inch suddenly travels 1 millimeter, or 25.4 millimeters instead of 1. Verify this at the top of every program.

G28 — Return to machine home. Often used at the start or end of a program to get the machine into a known safe position.

G90 / G91 — Absolute vs. incremental positioning. G90 (absolute) means coordinates are measured from the work zero — X10 Y5 always means the same position regardless of where the machine is now. G91 (incremental) means coordinates are relative to the current position — X10 Y5 means "move 10 units right and 5 units forward from here." Most CAM output uses G90. If you see G91 unexpectedly, pay attention.

M3 / M5 — Spindle on (clockwise) and spindle off. Every program should have M3 before the first cutting move and M5 before the end. If you edit a program and accidentally delete M5, your spindle will keep running after the job finishes.

M30 — End of program, rewind. The machine stops, the program pointer resets to the beginning. This should be the last line of every file.

F — Feed rate. F72 sets the feed rate to 72 inches per minute (or mm/min if G21 is active). Feed rate is modal — once set, it stays active until you change it. If you want a different rate for a plunge vs. a horizontal cut, you need separate F values on those lines.

Reading a Real Program

Here's a minimal five-line program with every line explained:

Notice the plunge rate (F30) is separate from the horizontal cut rate (F72). Plunging into material puts more load on the bit tip than a lateral cut — a lower feed rate here is intentional, not tentative.

Wood Grain Direction & CNC — What Changes Under a Spinning Bit

If you've spent any time with hand tools, you already know that wood isn't the same in every direction. That knowledge transfers directly to CNC — but the feedback is different. A hand plane tells you instantly when you're going against the grain. A CNC router tells you after the cut is done, when the tearout is already there.

Three Directions, Three Behaviors

Every board has three grain orientations relative to any given cut — and the same bit behaves differently in each one.

Long grain (cutting parallel to the fibers): the cleanest cuts, lowest resistance, most forgiving of variations in feed rate and chip load. This is where your machine will feel at its best.

Cross grain (cutting perpendicular to the fibers): higher resistance, greater tearout risk — especially at exit edges where fibers are pushed outward rather than sheared cleanly. Requires sharper bits and more careful feed rate selection.

End grain (cutting into the end of the board): hardest on the bit, worst surface finish, highest heat generation. The fibers compress rather than shear, and the cut demands more from both the edge geometry and the cutting parameters.

The critical point: the same board presents all three orientations depending on which direction the toolpath runs. A pocket cut in the center of a panel will encounter long grain on two sides and cross grain on the other two. Your CAM doesn't know which is which — you do.

Grain and Feed Direction

In CNC, the toolpath direction relative to grain determines your surface quality as much as any feed-and-speed setting. Cutting along the grain — toolpath parallel to the fibers — is smooth, low-resistance, and forgiving. Cutting across the grain demands lower feed rates and sharper bits to avoid tearing the surface.

The exit side of a cross-grain cut is where tearout concentrates. As the bit exits the material at the far edge of a pass, the fibers ahead of the cutting edge have nothing supporting them — they push outward and split rather than shear cleanly. This is the same phenomenon you manage with a hand plane by planing toward a supported edge.

Climb milling across grain tends to produce less tearout than conventional milling. In climb milling, the bit pushes fibers into the material rather than pulling them out toward the exit edge. The tradeoff is that climb cuts generate more lateral force and require a rigid machine. On an MPCNC or similar lighter build, use conventional milling but drop your feed rate 10-15% for cross-grain passes.

Figured and Difficult Woods

Curly maple, bird's eye, quilted maple, and similar figured woods present a problem that doesn't exist in straight-grained stock: the grain direction changes constantly across the face of the board. There is no single "good" toolpath direction. What cuts cleanly in one area will tear in another four inches away.

For figured woods, use a sharp compression bit, reduce feed rate 15-20% from your straight-grained equivalent, and use climb milling where machine rigidity allows. Accept that some hand finishing — card scraper, light sanding — will be needed on the final surface. This is not a CNC failure; it's the nature of figured wood. Hand planes have the same problem.

These woods are a primary reason downcut bits exist. The downward cutting force presses fibers flat against the material surface instead of pulling them away from it — the opposite of what an upcut bit does at the top face of the cut.

The End Grain Challenge

End grain is 2-3× harder on the bit than long grain. The fibers compress under the cutting edge rather than shearing away cleanly, which means more friction, more heat, and more wear on the bit edge geometry.

When cutting predominantly in end grain, reduce your chip load targets by 25-30%. RPM can stay the same; drop the feed rate to compensate. This is one place where the ToolPath Advisor's chip load gauge earns its keep — dial in a lower target for the end grain section rather than using the same number you'd run in long grain.

Common situations where end grain dominates: the heel area of a guitar neck, end-grain sections of a cutting board, and any workpiece that was cut from the end of a turning blank. If your bit chatters in end grain when it ran quietly in the same stock's long grain, it isn't a speed problem — it's a rigidity and chip load problem. Slow the feed, not the RPM.

CNC for Luthiers — Guitar-Specific Workflows

ToolPath Advisor was born in a guitar shop. If you're using CNC for instrument building — bodies, necks, pickguards, inlays — here's what matters most, from someone who's been making guitars for over fifty years.

Body Carving — Two-Sided Fixturing

Most electric guitar bodies require machining on both faces: the front for body contours and pickup cavities, the back for the control cavity and sometimes a belly carve. The key to making this work repeatably is a reference fixture — a jig plate with dowel pins or threaded inserts that lets you flip the workpiece and maintain registration within 0.005" or better.

CNC the fixture first, from the same material you'll use as the spoilboard. Every body blank you run drops onto the same pins in the same orientation. Flip it, same pins, same zero. Alignment error on a properly made fixture is typically under 0.003" — invisible in a finished instrument.

Separate your toolpaths into two categories: structural features (neck pocket, pickup cavities, control cavity, strap pin holes) and artistic features (body contours, belly carve, forearm relief). Keep these as separate CAM operations. When you want to adjust the carve depth or change a contour profile, you regenerate only the artistic paths without touching the structural ones. This separation has saved me from rebuilding full setups more times than I can count.

Neck Pockets — Where Tolerance Matters

The neck pocket is the most structurally critical feature on an electric guitar. A sloppy pocket produces a loose neck joint, and a loose neck joint produces dead spots, poor sustain, and intonation problems that no amount of setup work will fully correct. Target 0.002" tolerance or tighter on both width and length.

Run the pocket in two passes: a roughing pass that leaves 0.010-0.015" of stock on the walls, then a finishing pass with a sharp downcut bit at 10-15% stepover. Measure the finished pocket with calipers before you ever put a neck near it. If the pocket is 0.004" undersize, adjust your CAM offset and re-run the finishing pass — don't force a neck into a tight pocket.

Pocket depth is as important as width. The bottom surface should be consistent within 0.005" across the entire floor — any dip or ridge and the neck won't seat flat. Run a facing pass on the pocket floor as the final operation. This is one place where a dull bit will telegraph directly into the instrument's performance.

Pickup Cavities and Control Routes

Pickup cavities and control routes are straightforward pockets, but depth matters in ways that aren't always obvious. Use upcut bits for chip evacuation — the chips have nowhere else to go in a deep pocket, and an upcut geometry keeps them moving out rather than packing in.

Cavity depth for pickups should be measured from the face of the guitar, not from the spoilboard. If your body has any thickness variation — and all real wood does — spoilboard-relative depth will produce cavities that aren't consistent across the body face. A cavity that's 0.020" too shallow means the pickup sits too high and the strings contact the pole pieces. Too deep and you lose sustain and make height adjustment difficult. Measure from the face; program from the face.

Inlay Work

CNC excels at inlay pockets — the precision and repeatability that's tedious by hand become straightforward operations. Use a V-bit for decorative inlays with pointed corners, or a small-diameter downcut end mill (1/16" or 1/32") for rectangular pockets with square corners.

Pocket depth must match inlay thickness exactly. Too shallow and the inlay sits proud of the surrounding surface — you can sand it flush but you risk sanding through the inlay. Too deep and the glue line shows as a visible gap around the perimeter. For shell or stone inlays, program the pocket 0.003-0.005" undersized and hand-fit with a fine file. The CNC gets you 95% of the way there; the last few thousandths of gap fit are hand work. A zero-gap inlay line is worth the extra ten minutes at the bench.

Fretboard Slots

Slotting fretboards on CNC is one of the most satisfying applications of the machine — the precision needed (slot position accuracy within 0.005", kerf width within 0.001") is exactly what CNC does well and what hand sawing requires enormous care to achieve consistently.

Use a 0.023" kerf slotting saw or a micro end mill matched to your fret wire tang width. Each slot needs to be exactly perpendicular to the board edge — any angular error compounds across 20+ frets into visible intonation problems. Depth is equally critical: typically 0.055-0.060" for most fret wire. A slot that's too shallow means the fret won't seat and crown fully; too deep and you've weakened the board at the slot location. Run each slot as a separate toolpath in your CAM so you can adjust individual slot depth if the board thickness varies — and it will vary, even with surfaced stock.