- Check three things first, every time: bit sharpness, feeds/speeds, and workholding — they cause the vast majority of cut quality problems
- Burning means your bit is dwelling too long — increase your feed rate before you lower your RPM
- Fuzzy or torn edges usually mean wrong bit type — upcut bits tear the top surface, downcut bits tear the bottom
- Chatter marks are a rigidity problem — reduce depth of cut and shorten your tool stickout before changing anything else
- If your cut doesn't go all the way through, it's almost always a Z-zero or wasteboard flatness issue — not your feeds and speeds
- When in doubt, try a fresh bit — you'd be surprised how often that's the entire fix
Before You Diagnose Anything: The 3-Thing Checklist
Before you read any further or change any settings, check these three things. They solve most problems. We mean most.
1. Is your bit sharp? Run your fingernail across the cutting edge. If it doesn’t bite in and catch, it’s dull. Carbide bits last longer than HSS, but they still wear out. If you’ve been cutting MDF or plywood, your bit dulled faster than you think.
2. Are your feeds and speeds reasonable? You need enough chip load. Each flute should be taking a real bite, not rubbing. If you’re making fine dust instead of small chips, your feed rate is too low for your RPM. Check our feeds and speeds guide or plug your setup into our free calculator for starting points.
3. Is the material actually locked down? Push on your workpiece. Does it move at all? Even a tiny shift mid-cut ruins everything. Clamps, tape, or vacuum. Pick one and make sure it’s solid.
Now let’s figure out what’s wrong with your specific cut.
Burned Edges
What it looks like
Dark brown or black scorch marks along the cut edges, especially on hardwoods like maple, cherry, and oak. The burn may be on the sides of a profile cut, inside slots, or along pocket walls.
Most likely cause
Your feed rate is too slow for your RPM. The bit rubs instead of cutting, friction builds, wood burns.
Fix it (in this order)
- Increase feed rate. This is the #1 fix. On trim routers that bottom out around 10,000–12,000 RPM, moving faster is your main lever.
- Lower RPM if you can. Dial 1–2 on a Makita or DeWalt is often enough for wood.
- Check your bit. A dull bit generates more friction no matter what. Swap in a fresh one.
- Improve chip evacuation. Recut chips = more heat. Use a dust boot or air blast, and consider fewer flutes for better clearance.
The hobby CNC community is nearly unanimous: burning is a feed rate problem, not an RPM problem. The instinct is to slow everything down when cuts look bad, but for burning, you actually need to speed up.
Cherry and maple burn if you even look at them funny. Those species are just heat-sensitive. Be extra aggressive with feed rates on those woods.
Fuzzy or Torn Edges
What it looks like
Ragged, hairy, splintery edges, especially on the top surface of plywood or along the grain in softwoods like pine and poplar. The cut might be smooth on one side and fuzzy on the other, or fuzzy on top but clean on the bottom.
Most likely cause
You’re using the wrong bit geometry for where you need the clean edge. Upcut spiral bits pull chips (and wood fibers) upward, which tears the top surface. Downcut bits push everything down, giving a clean top but potentially rough bottom.
Fix it (in this order)
Switch your bit type based on which surface matters. We explain upcut vs downcut vs compression bits in detail:
- Need a clean top surface? Use a downcut bit.
- Need clean top AND bottom (cutting through plywood)? Use a compression bit, but your first pass depth must be deeper than the upcut portion of the bit (typically 5-7mm minimum).
- Pocketing where only the top matters? Downcut works great, but watch chip evacuation.
If switching bits isn’t an option, try reducing your feed rate slightly. Excess feed makes tearout worse, especially when cutting across the grain.
A dull bit tears more than a sharp one. This is the sneaky cause. The bit still “feels” sharp but the micro-edge is gone. If you’ve been cutting plywood or MDF (both are extremely abrasive), swap in a fresh bit.
For really stubborn fuzz on softwoods, try this trick from the Tormach community: spray a coat of lacquer or shellac on the wood surface before cutting. It stiffens the fibers enough to get a cleaner shear.
Chatter Marks
What it looks like
Evenly spaced ridges or waves on the cut surface, like tiny washboard ripples. You can feel them with your fingernail. They follow a regular pattern, which distinguishes chatter from random roughness.
Most likely cause
Something in your system is vibrating. On hobby CNC machines, this is usually a rigidity problem. The machine, bit, or workpiece is flexing during the cut.
Fix it (in this order)
Reduce your depth of cut. This is the fastest fix. Take shallower passes. Half the depth of cut means dramatically less cutting force and less deflection.
Shorten your tool stickout. Only extend the bit as far as you actually need. A bit hanging 2 inches out of the collet vibrates way more than one hanging 1 inch out. This matters more than most people realize.
Check every bolt on your machine. Seriously. Grab a wrench and go through them all. Loose V-wheels, gantry bolts, router mount screws, and eccentric nuts are common culprits. Belts should be firm (not guitar-string tight, but not floppy either).
The counterintuitive fix: try increasing your feed rate. When chip load is too thin, the bit rubs instead of cutting, which induces vibration. Bumping the feed rate up gives each flute a meatier bite and can actually smooth things out.
Raise your workpiece if your Z-axis is extended way down. The more your router hangs below the gantry, the more leverage vibration has. Put a supplemental wasteboard under your material to bring it up.
Rough Pocket Bottoms
What it looks like
The walls of your pocket might be fine, but the bottom looks like a plowed field: ridges, scallops, or an uneven texture across the floor.
Most likely cause
Your machine’s wasteboard isn’t flat, or your bit has runout. Pocket bottoms are uniquely sensitive to both because the bit is sweeping across a surface at a consistent Z height.
Fix it (in this order)
Surface your wasteboard. If you haven’t done this recently (or ever), this is likely your problem. A surfacing bit across the full spoilboard ensures your Z-zero reference plane is actually flat.
Check for bit runout. Spin the bit by hand and watch the tip. Does it wobble? Even 0.002” of runout creates visible ridges on pocket floors. This can be the collet, the bit, or (on cheaper routers) the spindle itself.
Add a finish pass. Program a light final pass (0.5mm or less) at the full pocket depth with a higher feed rate. This cleans up the floor without the heavy cutting forces.
Stepover also matters. A 50% stepover leaves visible scallops with round-nose bits. Drop to 10-15% stepover for the final pass if you want a smooth floor.
Not Cutting All the Way Through
What it looks like
Your profile cut is done, but the piece won’t pop out. There’s a thin skin of material left connecting it, or it only cut through in some spots but not others.
Most likely cause
Your Z-zero is slightly off, or your material isn’t uniform thickness. This has almost nothing to do with feeds and speeds.
Fix it (in this order)
Re-zero your Z more carefully. Use the paper method (lower the bit until a piece of paper just barely drags) or a touch plate. Make sure you’re zeroing on the actual material surface, not the wasteboard.
Measure your material thickness with calipers. That “3/4 inch” plywood? It’s probably 0.72” or 0.69”. Set your cut depth to the actual measured thickness plus 0.5-1mm into the wasteboard.
Surface your wasteboard. If the wasteboard isn’t flat, Z-zero is only accurate at the spot where you zeroed. The rest of the board could be higher or lower. This is the most common hidden cause.
If it’s cutting through in some spots but not others, that’s a dead giveaway that either your wasteboard is uneven or your material thickness varies across the sheet.
Dimensional Inaccuracy
What it looks like
Circles aren’t round. Squares aren’t square. Parts are slightly too big or too small. Joints don’t fit. Features that should line up don’t.
Most likely cause
Bit deflection or mechanical slop in your machine. On hobby CNCs, both are common.
Fix it (in this order)
Use a larger bit when possible. A 1/4” bit deflects far less than a 1/8” bit under the same load. If your design allows it, size up.
Take a finish pass. Rough out your shape leaving 0.5mm of material, then do a light final pass. The finish pass has almost no cutting force, so deflection is minimal and you get accurate dimensions.
Check your belts and anti-backlash nuts. Loose belts allow the gantry to lag behind where the controller thinks it is. Tighten them. If you have lead screws, check for backlash.
Calibrate your steps per millimeter. Cut a known dimension (like a 100mm square), measure it, and adjust your GRBL settings if needed. Most machines ship reasonably calibrated, but it’s worth checking.
When to Blame the Bit vs. the Settings vs. the Machine
This decision framework saves you hours of chasing the wrong fix:
Blame the bit if: The problem appeared gradually over multiple projects, or you just switched to a new material (especially MDF or plywood, which dull bits fast). Try a fresh bit. It’s the cheapest experiment. If you’re not sure which bits to keep on hand, our beginner bit guide covers the essentials.
Blame the settings if: The problem appeared immediately on a new project with new settings, or you’re getting burning (too slow) or chatter (wrong chip load). Adjust feeds and speeds.
Blame the machine if: The problem appears on one axis but not the other, parts are dimensionally wrong in a consistent direction, or you hear unusual sounds from the motion system. Check bolts, belts, and wheels. Machine rigidity varies a lot by model. Our Shapeoko vs OneFinity vs LongMill comparison covers what to expect from each.
Blame the workholding if: The problem appeared partway through the cut, the cut started fine then went wrong, or you can see the material shifted. Lock it down better.
We don't write in a vacuum. Here's what we studied, what we trust, and why.