How to Stop Tearout on a CNC Router: Climb Cuts, Downcut Bits, and Spoilboard Support
How to Stop Tearout on a CNC Router: Climb Cuts, Downcut Bits, and Spoilboard Support
Tearout on a CNC router is one of those problems that can ruin an otherwise good part in a fraction of a second. You are watching a profile cut come together, the piece looks clean, and then the bit blows out a chunk of veneer on the last pass. If you are cutting plywood, figured wood, or anything with a face veneer you care about, you have almost certainly been there.
The good news is that knowing how to stop tearout on your CNC router is mostly a matter of understanding three things: which direction the cutter is fighting the wood, what geometry your bit uses to shear fibers, and whether your material is properly supported. Get all three right and tearout becomes rare. Get one wrong and it will dog you every session.
This article covers each factor in plain language, with the trade-offs spelled out.
Why Does Tearout Happen in the First Place?
Wood is a bundle of fibers. When a spinning bit hits those fibers, it either shears them cleanly or levers them up and snaps them. Which one happens depends on the direction of cut, the sharpness of the tool, and whether the fiber has anything supporting it from the other side.
Wood is anisotropic — its properties change with grain direction — and it is sensitive to heat, burning instead of just discoloring. That anisotropy is the root cause of most tearout. A cut running with the grain behaves very differently from one running across it, and even the same direction can produce different results depending on whether you are on the uphill or downhill side of the grain angle.
Three levers control whether fibers tear or shear:
- Cut direction — climb vs. conventional milling
- Bit geometry — upcut, downcut, or compression spiral
- Support — what is holding the fiber in place at the moment the bit contacts it
Work through them in that order.
Climb Milling vs. Conventional Milling: Which One Reduces Tearout?
This is the question that fills forum threads, and the honest answer is: it depends on where the tearout is occurring and what you are cutting.
What the Terms Actually Mean
There are two distinct ways to cut materials when CNC milling: conventional milling (up) and climb milling (down). The difference is the relationship of the rotation of the cutter to the direction of feed. In conventional milling, the cutter rotates against the direction of the feed. During climb milling, the cutter rotates with the feed.
A practical way to keep them straight: think of the spindle as a pinch roller that can either help move the workpiece in the direction it was already going (climb milling), or that might fight that movement (conventional milling).
How Each Affects the Wood Fiber
Climb cutting accomplishes several things that reduce tearout. One, it reduces cutting forces, so there is less force trying to tear out the wood. Two, chips are cut as little C-shaped pieces — thin at one end and thick at the other. With climb cutting, they start to get thicker as the cut progresses; the cutter eases in. With conventional cutting, they are fat and get thinner. The cutter basically slams in at full force, which can make tearout more likely.
So for edge quality on solid wood or hardwood plywood, climb cutting is generally the better starting point on a CNC router — unlike a handheld router, where the machine controls the forces for you.
If you have used a handheld router, you know that climb cutting is very uncomfortable — the router wants to take off on its own. But one of the beauties of CNC is it controls those forces so you can make climb cuts whenever you want.
When Conventional Cutting Is the Right Call
Climb cutting is not always the answer. Conventional milling offers more control and less vibration than its climb milling counterpart. For materials that traditionally chatter or tear, conventional milling can be the proper strategy.
Specifically: for CNC routers, climb milling is generally preferred because modern ball screws handle the forces. Switch to conventional only for flexible materials — thin plywood, sheet plastic — that deflect under climb cutting forces.
There is also a grain-direction wrinkle. Generally, conventional cutting will almost always give a better quality cut than climb cutting, but there are exceptions. The most important factor when cutting wood is preventing tearout. To avoid tearout with conventional cutting, you need to make sure there is always some wood on both sides of the bit. When the bit is breaking out through an open edge using conventional direction, the tool is pulling the wood toward the edge, which will result in splintering — so for rebates and edge cuts, climb cutting is often the right move.
The practical takeaway: Use climb for profiling solid wood and hardwood-faced plywood. Use conventional when material is thin or flexible enough to deflect, or when you are doing a finishing pass in a pocket where the walls provide support on both sides.
Does Bit Geometry Matter More Than Cut Direction?
Often, yes. Cut direction affects chip formation; bit geometry determines whether the fiber is being pushed into the surface or pulled away from it on the face you care about.
Upcut Spiral
An upcut spiral is the workhorse. It evacuates chips efficiently and is good at plunge cuts. The downside: upcut spirals offer great chip removal but can tear out the top of thin veneer such as finish-grade plywood. The helix lifts chips — and face fibers — upward. If the show face is on top, that is the face getting torn.
Downcut Spiral
Downcut spiral bits are designed to produce perfectly clean edges on the top face of the workpiece, but since the bit's geometry causes wood chips to travel in a downward direction, the toolpath can become obstructed. Translation: they are excellent for clean top surfaces, but they push chips into the cut rather than clearing them, which limits how deep you can go per pass and how fast you can move before things get ugly.
Downcut bits are the right choice for grooves in tearout-prone materials like highly figured wood, plywood, and other veneers, for a clean edge on the tool side of your stock, and for cutting small parts on the CNC.
These bits are especially useful when routing material such as melamine and plywood.
Because chip evacuation is poor, downcut bits typically require lighter passes — in practice, keep depth of cut at or below half the bit diameter as a starting point and listen for the cut loading up. On a 1/4" downcut bit in 3/4" Baltic birch, that means multiple passes, not one plunge.
Compression Bits
Compression bits combine up and down spiral geometry, making them a great all-around bit — especially for plywood or laminated sheet goods. The lower flutes cut upward (clearing chips); the upper flutes cut downward (pressing the top veneer). The result is a clean edge on both the top and bottom faces simultaneously — but only when you are cutting through the full thickness of the material. If you are doing a shallow pocket, the compression geometry does nothing useful because only the lower upcut portion of the flute is engaged.
Compression bits make the most sense for full-depth profile cuts through sheet goods where both faces matter — cabinet parts, sign blanks, nested furniture components.
Quick Reference
| Situation | Recommended Bit |
|---|---|
| Pocket or dado, show face up | Downcut spiral |
| Through cut, show face on both sides | Compression |
| Through cut, only bottom face matters | Upcut spiral |
| Inlay or fine detail in figured wood | Downcut spiral |
| Full-depth profile in plywood | Compression |
Chip Load: The Feed and Speed Factor Nobody Talks About Enough
Bit geometry and cut direction only work if the bit is actually cutting rather than rubbing. A dull bit or an incorrect chip load produces the same symptom as bad bit selection: torn, ragged edges.
Chip load is the single most important concept in CNC routing. Every feeds and speeds decision flows from it. A correct chip load means efficient cutting, cool temperatures, long bit life, and clean surface finish.
The formula: Feed Rate (IPM) = Chip Load × RPM × Number of Flutes
Chip load for wood depends on species hardness and tool diameter. For a 1/4" bit as a starting point: softwood (pine, cedar) 0.10–0.25 mm per tooth, hardwood (oak, maple) 0.08–0.20 mm per tooth, plywood 0.08–0.18 mm per tooth, MDF 0.10–0.25 mm per tooth. These are starting points — treat them as the beginning of a test cut, not gospel.
For a deeper dive into the math and material-specific guidance, see our guide to CNC router feeds and speeds for plywood and sheet goods. The same principles apply across species and materials — it all comes down to finding the chip load that makes your machine sing.
Too low a chip load causes burning — rubbing instead of cutting. Too high a chip load causes tearout and possible bit breakage.
The chips coming off the cut tell you whether you have it right. If your CNC router is producing fine powder instead of small chip flakes, your chip load is too low. Increase the feed rate until you see actual chips. Dust means rubbing, which means burning and premature tool wear. Conversely, large ragged chunks with torn grain mean you are taking too much per tooth — slow the feed or increase RPM.
Carbide router bits stay sharp for 500–2,000 linear feet of cutting in hardwood, depending on the material and bit quality. A bit that is past its service life will tear rather than shear no matter how good everything else is. When edges that used to come out clean start coming out ragged on the same settings, the bit is usually the first thing to check.
As a depth-of-cut starting point: take multiple lighter passes — typically half the bit diameter or less per pass — rather than cutting full depth. On a 1/4" bit, that means 1/8" DOC to start. Adjust from there based on what you hear and see.
How Does Spoilboard Support Prevent Tearout?
Even perfect bit geometry and cut direction fail when the workpiece is not properly supported. Fiber needs something to push against at the moment the bit contacts it, or it levers away and breaks.
The Spoilboard as a Backing Surface
A backing board can do wonders for reducing tearout because it supports the surface of the wood. Obviously the backer can't be in the way of the cut. It's mostly useful when clamped against the endgrain so you can cut parallel to the grain. But you can also view your spoilboard as a backing board for the bottom of the cut — and stack another board on top to protect the top face.
A backer board, sacrificial spoilboard, or zero-clearance support under the cut prevents fiber blowout on the bottom face. Strong vacuum hold-down or clamps keep the part stationary during the cut.
That last point is critical. If the sheet lifts, vibrates, or loses support near the toolpath, tearout becomes more likely. A flat spoilboard, strong vacuum hold-down, tabs, clamps, or other workholding methods can help keep the material stable throughout the cut.
Keep Your Spoilboard Flat
A spoilboard is a disposable work surface mounted atop the router's permanent table. It is typically MDF and protects the router table from damage while providing an expendable surface that can participate in workholding. A warped or uneven spoilboard creates high spots where the workpiece rocks, and low spots where it has no support at all — both of which make tearout worse.
From time to time a spoilboard will need to be surfaced: a spoilboard cutter is used to clean up any gouges or cuts and make the board flat and parallel to X and Y axis travel. If you have not surfaced your spoilboard since you built the machine, that is likely contributing to your tearout — especially on thin material.
Each surfacing operation removes 0.010"–0.020" of material. Track your total spoilboard thickness and replace when you have removed more than 1/4" of the original thickness. Over-surfaced spoilboards lack the rigidity and screw-holding capacity needed for secure workholding.
Onion Skinning for the Final Pass
For critical parts, some CNC users leave a very thin layer of material at the bottom of the cut, then remove it with a final pass. This technique — often called onion skinning — can help reduce movement and support the bottom veneer until the final cleanup pass. It adds a step, but on expensive or irreplaceable stock it is worth it.
Tape and Scoring
For small or delicate parts where vacuum or clamps are awkward: painter's tape on the visible face is a cheap, surprisingly effective tearout prevention on small parts and delicate veneers.
Scoring the veneer before cutting can help prevent splintering, especially on delicate plywood, cross-grain cuts, or prefinished panels. A sharp utility knife scribed along the cut line severs the top fibers before the bit gets there, removing the tearout mechanism entirely on that face.
Putting It Together: A Decision Workflow
Here is how to think through a new job before you hit run:
- Identify which face is the show face. Downcut bits protect the top face. Upcut bits protect the bottom. Compression bits protect both — but only on through cuts.
- Check whether you are profiling or pocketing. Compression bits in shallow pockets are pointless. Downcut bits in deep through cuts will struggle with chip evacuation.
- Set your cut direction. Climb for hardwood profiles and veneer-faced plywood. Conventional for thin or flexible material that deflects under lateral cutting forces.
- Dial in chip load. Start conservative — around half the middle of your target range. Look at the chips. Adjust.
- Confirm your spoilboard is flat and your workholding is solid. No bit geometry or toolpath trick compensates for a workpiece that is flexing or lifting mid-cut.
- Run a test cut on scrap of the same species and thickness. A test cut on scrap of the same material catches problems before they affect real parts. Run the program on a small offcut, inspect the edges, adjust if needed, then commit to the production run.
If you are using EdgeWright for your toolpath generation, the climb/conventional setting is exposed directly in the profile operation dialog — worth checking that it matches your intended strategy before you post.
FAQ
Does a dull bit cause more tearout than a sharp one?
Yes, significantly. A dull bit requires more force to cut the same material, which means it is more likely to lever fibers rather than shear them cleanly. If the same bit produces inconsistent results in the same material across a single run, the problem is probably the bit (dull, damaged, or with runout) or the machine (worn collet, loose spindle, soft workholding). Check the bit first, then the collet, then the holding setup.
Should I use a downcut bit for all plywood work?
Not all of it. Downcut bits are the right choice when a clean top face is the priority — dadoes, pockets, inlays, and parts where only one face shows. Downcut spiral bits produce perfectly clean edges on the top face of the workpiece, but since the bit's geometry causes wood chips to travel in a downward direction, the toolpath can become obstructed. For full-depth profile cuts in plywood where both faces matter, a compression bit is usually a better choice.
Does depth of cut affect tearout?
Directly. Shallower cuts reduce tearout because the deeper the cut, the more of the cutter's helix is engaged. It is that helical shape that causes the upward pull that leads to tearout and splintering. Reducing depth of cut reduces the amount of helix that can apply upward forces. When tearout is stubborn, try taking lighter passes before swapping bits.
Is climb milling safe on a hobby machine like a Shapeoko or Onefinity?
Generally yes, with caveats. Climb cutting does require rigid workholding and a machine that can handle the cutting forces. On a lighter gantry machine, keep your depth of cut conservative when climb cutting on profile passes — especially on hardwood. If you notice the machine deflecting or hear the spindle loading, reduce DOC or switch to conventional.
What causes tearout on the bottom face of a plywood through cut?
The bottom veneer has nothing supporting it as the bit exits the material. An upcut spiral lifts chips — and fibers — upward, blowing out the bottom layer as it exits. Fixes: use a compression bit (which shears the bottom face downward), make sure your spoilboard is flat and the workpiece is fully supported, or use an onion skin approach where you leave a thin layer and complete the cut in a final light pass.