How to Cut Out a Circle With a CNC Machine

• 1
  Key takeaways
• 2
  Prepare the Machine and Workpiece for a Round Cut
• 3
  Program the Circle: Tool Path, Entry, and Compensation
• 4
  Set Feeds and Speeds for Circular Interpolation
• 5
  Finish, Measure, and Hold Roundness
• 6
  Common Problems When You Cut Out a Circle
• 7
  Step-by-Step Circle Cutting Sequence
• 8
  Which Circle-Cutting Method Fits Your Feature

Every circular cut starts with the setup, not the program. A circle is unforgiving: if the stock sits 0.1 mm off the vise jaw or the part lifts during the cut, the diameter will still measure close while roundness drifts out of tolerance. Check that the stock is flat, deburred, and seated on parallels before you close the vise.

Toolholding matters more than most people expect. Use the shortest gauge length you can get away with, especially for thin-walled circular parts where a long tool deflects and leaves a tapered wall. On a Ø20 mm end mill in aluminium, a 60 mm gauge length behaves very differently from a 100 mm one.

For holes deeper than about 3× the tool diameter, helical interpolation with a smaller cutter is usually safer than plunging a large tool. A Ø10 mm cutter helixing a Ø30 mm bore keeps radial engagement low and chip evacuation steady.

Confirm the coordinate system before the first cut. Touch off the work offset on a known face, then verify with a test move or an indicator sweep. A wrong offset shifts the circle center, and no amount of feed tuning will fix a part that is bored in the wrong place.

• 1
  Clean the vise jawsChips under the stock tilt the part and create an oval bore.
• 2
  Check tool runoutMore than 0.01 mm TIR shows up as a rough wall and poor size control.
• 3
  Rigid workholding firstThin rings flex; support them or cut them from solid if the design allows.

In CAM, a circle can be produced three ways: helical interpolation with an end mill, circular pocketing for larger diameters, or a boring cycle on a lathe. Helical interpolation is the workhorse for milled holes from roughly Ø6 mm to Ø80 mm. Circular pocketing suits bigger bores where a single helix would leave a large uncut core.

Use cutter compensation, not an oversized program radius. If the tool measures 9.96 mm instead of 10.00 mm, comp lets you dial that 0.04 mm back at the control. Programming the nominal radius and hoping the tool matches it is how circles come out undersized.

Set entry and exit with care. A ramp or helical entry is gentler than a vertical plunge, and a short overlap at the end of the loop avoids a witness mark where the tool re-enters. For a full circle, program 360° of travel plus a small overlap, then lead out on an arc.

Choose climb milling unless the material tells you otherwise. Climb milling starts the cut with maximum chip thickness, which keeps the tool from rubbing and reduces work hardening in stainless and titanium. Conventional milling is occasionally better on older machines with backlash, but on a modern CNC the default should be climb.

• 1
  Do not break the circleTwo half arcs joined at the quadrant leave a visible step.
• 2
  Lead in on an arcA radial lead-in avoids a dwell mark on the finished wall.
• 3
  Keep chip load constantVarying radial engagement changes the cutting force and the wall finish.

Interpolated circles run at a different effective feed than a straight cut. The tool center travels a smaller radius than the cutting edge, so the actual chip load at the outside of the tool is higher than the programmed feed suggests. On a Ø30 mm bore cut with a Ø10 mm tool, the center path is only Ø20 mm, and the edge speed is roughly 1.5× the center speed.

A practical rule: reduce the programmed feed by 20–30% for interpolation, or use a controller that compensates automatically. In 6061 aluminium with a 3-flute carbide end mill, cutting speeds around 300–500 m/min and a feed per tooth of 0.05–0.10 mm are a reasonable starting point. Stainless 304 runs much slower, often 60–120 m/min.

Watch the radial depth of cut. A finish pass at 0.2–0.4 mm radial engagement keeps deflection low. If you take a 3 mm finish cut with a long tool, the wall will spring back and the bore will measure small at the top and large at the bottom.

Coolant and chip evacuation decide whether the finish holds. Through-spindle coolant or a strong air blast clears chips from a deep bore. Recutting chips is one of the fastest ways to ruin a finished wall on aluminium and to work-harden stainless.

• 1
  Start conservativeTune feed up in 10% steps while watching the chip shape.
• 2
  Listen to the cutA squeal or a high-pitched ring means deflection or chatter.
• 3
  Check chipsThin, powdery chips mean rubbing; proper chips are short and curled.

After the roughing helix, leave the wall at nominal minus 0.2–0.4 mm and take one continuous finish pass. A single finishing revolution at full depth gives the best roundness because the tool stays engaged around the entire circumference. Stop-and-go passes create lobing that a two-point micrometer will not reveal.

Measure diameter first, then roundness. A bore gauge or an inside micrometer gives size, but only a roundness check, a three-point bore gauge, or a CMM sweep shows lobing. If the feature has a tight roundness callout, plan for a boring head or a reamer as the final operation rather than trusting interpolation alone.

Surface finish follows the same logic. A finish pass at Ra 0.8–1.6 μm is normal for a well-tuned interpolated bore in aluminium. Bores that need Ra 0.2–0.8 μm usually go to a reamer, a boring head with a sharp insert, or a secondary lapping step.

Record what worked. Tool number, comp value, feed, and measured result should go on the setup sheet. The next run of the same part should not repeat the same trial-and-error, and a stable process is what keeps round features repeatable across a production lot.

• 1
  One finishing revolutionKeep the tool engaged all the way around for best roundness.
• 2
  Check at three pointsMeasure near the top, middle, and bottom of the bore.
• 3
  Deburr before measuringA raised edge reads as an oversize bore on some gauges.

An oval bore usually points to workholding or tool deflection, not the program. If the stock is not seated flat, the part tilts and the circle becomes an ellipse. If the tool is too long for the depth, it pushes away from the wall on one side and the bore is out of round in a repeatable pattern.

A tapered bore means the tool is bending or the machine is not square. Check tool runout and gauge length first, then check the spindle. On deep bores, a tapered wall can also come from chip recutting, where chips pack on one side and push the tool off line.

A visible witness mark where the tool re-enters the cut comes from a poor lead-in or a broken circle. Program a smooth arc lead-in and a small overlap. If the mark is already cut, there is no fix except a finishing pass with a different entry point or a boring operation.

Size that drifts across a batch is usually thermal or tool wear. Aluminium grows as it warms, so a bore measured hot can be undersize when it cools. Let parts settle to room temperature before final inspection, and track tool wear so the comp value is updated before the bore goes out of tolerance.

• 1
  Oval boreCheck workholding, then tool length and runout.
• 2
  Tapered wallShorten the tool or reduce the finishing depth of cut.
• 3
  Witness markFix the lead-in arc and the loop overlap.
• 4
  Size driftLet parts cool and update cutter comp for wear.