CNC Relief Carving Settings: Feeds, Speeds, Stepover and Depth per Pass

There is no single set of “perfect” feeds and speeds for every CNC relief carving. A setting that works beautifully with a 1/4-inch cutter in walnut can be completely wrong for a 1/16-inch finishing bit in maple on a lighter machine.

That does not mean you have to guess. CNC settings become much easier when you understand what each one controls and change one variable at a time. The goal is to give the cutter a steady, reasonable workload while producing the surface quality the project actually needs.

This guide explains feed rate, spindle speed, plunge rate, depth per pass, stepover and finishing allowance in plain language. It also gives you a repeatable way to find usable settings without treating a random number from the internet as a guarantee.

The Six Settings That Control Most Relief Carvings

Feed Rate

Feed rate is how quickly the cutter moves through the material during a cutting move. Depending on your software and location, it may be shown in inches per minute or millimeters per minute.

If the feed rate is too slow for the spindle speed, the bit can rub instead of cutting clean chips. That creates heat, dulls the cutter and may burn the wood. If the feed rate is too fast for the cutter, material and machine, the bit can chatter, deflect, break or force the CNC to lose position.

Spindle Speed

Spindle speed is how quickly the cutter rotates, measured in revolutions per minute. More RPM does not automatically make a cleaner cut. RPM and feed rate work together to determine how much material each cutting edge removes.

Small routers often run at high minimum speeds. If the router cannot slow down far enough for a recommended combination, you may need to adjust the feed within safe limits or choose a more suitable cutter. Never exceed the bit, collet, spindle or machine manufacturer's rated speed.

Plunge Rate

Plunge rate controls how quickly the cutter moves downward into the material. Most router bits do not clear chips as effectively during a straight plunge as they do while moving sideways, so plunge rate is normally lower than feed rate.

Ramps or helical entries are often gentler than driving the cutter straight down. If your CAM software offers a ramp option and the toolpath has room, it can reduce the sudden load on the bit and machine.

Depth per Pass

Depth per pass, sometimes called stepdown, is the vertical amount removed in each roughing layer. A deeper pass removes material faster but places more load on the bit, spindle and machine.

Safe depth depends on tool diameter, cutting length, flute geometry, material, machine rigidity, spindle power, workholding and feed rate. A number that is conservative for a heavy machine may be too aggressive for a lightweight desktop CNC—or unnecessarily slow for a stronger machine.

Stepover

Stepover is the sideways distance between adjacent toolpath passes. It is usually entered as a distance or a percentage of tool diameter.

During roughing, a larger stepover removes material more quickly but increases tool engagement. During ball-nose finishing, stepover controls the size of the tiny scallops left between passes. Smaller stepover usually creates a smoother surface, but it also creates more passes and a longer run time.

Finishing Allowance

Finishing allowance is the thin layer intentionally left on the model after roughing. The finishing bit removes it to create the final surface.

Too little allowance can let roughing marks or deflection reach the finished model. Too much forces the small finishing cutter to remove more material than necessary. The goal is a light, consistent skin—not a second roughing operation.

How Feed Rate and RPM Work Together

The useful concept connecting feed rate, spindle speed and flute count is chip load: the approximate thickness of the chip removed by each cutting edge.

Chip load = feed rate ÷ (RPM × number of flutes)

You do not need to become a machining engineer to use this idea. It simply explains why changing one number affects the others:

• Increasing feed while keeping RPM the same increases chip load.
• Increasing RPM while keeping feed the same decreases chip load.
• Adding more flutes at the same feed and RPM decreases the chip removed by each flute.

When chip load becomes too small, the cutter can create powder and heat instead of healthy chips. When it becomes too large for the setup, cutting forces rise and the machine may chatter or stall. Use the bit maker's chart as the starting point because the manufacturer knows the tool's material, geometry and intended use.

Roughing Settings vs. Finishing Settings

Roughing and finishing have different jobs, so they should not use the same strategy.

A Practical Starting Range for Stepover

Unlike feed rate, stepover is often discussed as a percentage because that makes it easier to compare different cutter diameters. These are useful testing ranges, not universal prescriptions:

• Roughing: roughly 35–50% of tool diameter is a common place to begin evaluating an ordinary pocket-style strategy.
• General ball-nose finishing: roughly 8–12% of tool diameter can provide a reasonable balance of surface quality and time.
• Fine-detail finishing: roughly 5–8% may reduce visible scallops when the project justifies the longer run time.

Those ranges still have to fit the bit manufacturer's guidance, material and toolpath. A steep wall, hard wood or tiny cutter can behave differently from a broad, shallow relief.

The image or simulation should make the tradeoff clear: large stepover leaves wider ridges, while small stepover places the passes closer together. At some point, reducing stepover further adds hours but produces little improvement after normal cleanup and finishing.

How to Choose Depth per Pass

There is no safe shortcut such as “always cut one tool diameter deep.” Bit geometry, material and machine rigidity vary too much for that to be reliable.

Use this order instead:

1. Find the tool manufacturer's recommended range for the exact bit and material class.
2. Check your CNC and spindle limits.
3. Use a more conservative depth if the cutter has long stickout, the machine is light or the stock is difficult to hold.
4. Make a short test cut and inspect the chips, sound, edge quality and tool temperature.
5. Increase efficiency gradually only when the cut is stable.

A shallower pass is not automatically safer if it is combined with rubbing, excessive RPM or poor chip evacuation. Judge the whole cutting system.

How Wood Changes the Settings

Wood is not a uniform engineering material. Species, grain direction, moisture, knots and even different areas of the same board can change the cut.

• Dense hardwoods: may demand lower engagement and sharp cutters but can hold crisp detail.
• Soft or stringy woods: can fuzz even when the load feels easy.
• Resinous woods: can build heat and material on the cutter.
• MDF: is consistent but creates very fine dust and can wear tools.
• Plywood: changes grain direction at every layer and may contain voids or glue pockets.

If you change from poplar to hard maple, do not assume the old setup will behave exactly the same. Test before committing a valuable board.

How Bit Diameter Changes the Settings

A 1/4-inch roughing bit and a 1/16-inch finishing bit cannot be treated alike. The larger cutter is stronger and can normally carry a heavier load. The tiny cutter has less cross-section, is more affected by runout and requires a lighter, more consistent remaining allowance.

When changing to a smaller bit:

• Load the exact tool definition in CAM.
• Reduce stickout as much as practical.
• Confirm the roughing pass left a uniform allowance.
• Use the smaller cutter manufacturer's recommended feed, RPM and plunge.
• Check that the tool can physically reach the deepest surface.

A finishing bit should not suddenly encounter a thick ridge that the rougher could not reach. Rest machining or an intermediate-size tool can help on complex models, but it adds another toolpath and alignment step.

Raster Direction and Surface Quality

A raster finishing toolpath moves back and forth in parallel lines. The direction of those lines can affect both runtime and the way the wood fibers respond.

Running with the grain may reduce cross-grain fuzz in some woods, while cutting across the grain can reveal detail differently. Steep features may also finish better in one direction than another. Offset or contour-style finishing follows the shape rather than using straight parallel passes and may suit some models better.

There is no direction that wins on every design. Preview the path, compare estimated time and use a small test area when surface quality matters.

What the Cut Is Telling You

Fine Dust Instead of Chips

The cutter may be rubbing because chip load is too low, the bit may be dull or the material may naturally produce small particles. Check feed, RPM, flute count and tool condition rather than changing one number blindly.

Burning or a Hot Bit

Common causes include dull tooling, too much RPM for the feed, recutting trapped chips and pausing in one area. Stop and correct the cause. Burning is not a normal price of obtaining detail.

Chatter or Repeating Ripples

Look for loose workholding, excessive stickout, a worn collet, tool runout, an overly aggressive load or machine flex. Slowing the feed alone may not solve vibration and can create more rubbing.

Fuzzy Detail

The wood species, grain direction, dullness, finishing direction and stepover can all contribute. Try a sharp tool and a small test in another direction before reducing stepover to an extreme value.

Lost Steps or Shifted Geometry

Stop the job. The machine may have been overloaded, the stock may have moved or a collision may have occurred. Do not continue a finishing pass after position is lost and expect the model to realign itself.

A Repeatable Test-Carve Method

A test does not have to be a miniature version of the entire project. Crop or choose a small section containing a flat area, a slope, a deep recess and fine detail. Carve it in offcut material from the same board whenever possible.

1. Record the bit, material, feed, RPM, plunge, depth per pass, stepover and finishing allowance.
2. Run the roughing and finishing test.
3. Inspect the chips, sound, heat, fuzz, scallops and missing detail.
4. Change only one important variable.
5. Run the test again and label the sample.

After a few projects, those labeled tests become your own setting library. They are more useful than a generic chart because they reflect your machine, spindle, bits and material supply.

Settings Checklist Before a Long Relief Carve

• The tool definition matches the physical bit.
• The units are correct.
• The feed and RPM begin within the tool maker's range.
• The plunge is appropriate or the entry is ramped.
• The roughing depth per pass is proven on this setup.
• The roughing stepover will not overload the tool.
• The finishing stepover produces acceptable scallops and runtime.
• The roughing allowance is light and consistent.
• The cutter has enough flute length and reach.
• The toolpath preview shows no collisions or overcuts.
• The board is secure and the clearance height clears every clamp.

Frequently Asked Questions

What feed rate should I use for a CNC relief carving?

Use the starting range supplied by the manufacturer of your exact cutter, then account for your material, spindle, machine rigidity and tool stickout. There is no responsible universal feed rate for every bit and CNC.

What stepover gives the best 3D finish?

For general ball-nose finishing, roughly 8–12% of tool diameter is a useful testing range. Fine-detail work may benefit from roughly 5–8%. Smaller is smoother but slower, so compare the result and run time instead of automatically choosing the lowest number.

Should I change RPM or feed rate first?

Begin with a manufacturer-recommended combination rather than isolating either number. If adjustment is needed, make a small documented change while staying within the limits of the bit, spindle and CNC. Watch chip formation, heat, sound and cut quality.

Why is my relief carving fuzzy?

Fuzz can come from soft or stringy grain, a dull cutter, the finishing direction, low chip load or tool deflection. Test a sharp bit and another toolpath direction before assuming an extremely small stepover will solve it.

How much material should roughing leave for finishing?

Leave a thin, consistent allowance that protects the final surface without overloading the finishing tool. The appropriate amount depends on cutter size, material, machine rigidity and CAM strategy; use your software and bit manufacturer's guidance and validate it with a test.

Can I copy settings from another CNC owner?

You can use them as context only if the machine, spindle, bit, flute count, tool stickout, material and units are comparable. Treat borrowed settings as an unproven reference, not a safe promise.

Always follow the cutter and CNC manufacturers' limits. Secure the workpiece, use dust collection and appropriate personal protective equipment, and never leave a running CNC unattended.