Troubleshooting · Dimensionsbeginner~4 min read

CNC part cut the wrong size: diagnose it by the error

Short answer

Measure the error. If it is exactly one bit diameter, you cut on the line instead of outside it. If it is two full diameters, the offset went to the wrong side. If it is a few thousandths, it is the real bit diameter, deflection or runout. If it is a percentage, it is calibration.

Symptom

A finished part that does not match the drawn dimension. May be consistently undersize, consistently oversize, or wrong in one axis only.

Check
first

Measure the error and compare it to your bit diameter. The amount tells you the cause faster than anything else. One diameter, two diameters and a few thousandths are three completely different problems.

Most likely causes

Profile cut on the line instead of outside or inside itMost common
The part comes out exactly one bit diameter small, or the hole one diameter big. See profile toolpaths.
Bit diameter in CAM does not match the bit in the colletCommon
A nominal 1/4 inch bit is often a few thousandths under, and a 6 mm bit entered as 1/4 inch is 0.35 mm out. The error is half the difference on each side.
Tool deflectionCommon
The tip bends away from the material and leaves the part oversize, more so at depth. A finishing pass removes it. See rigidity.
Offset applied to the wrong sideOccasional
Inside instead of outside. The part comes out two full bit diameters small, which is dramatic enough to be obvious.
Steps per unit wrong for one axisOccasional
A percentage error that scales with the part, in one direction only.
RunoutOccasional
The bit sweeps a circle wider than its diameter, so it cuts more and leaves the part undersize. Clean the collet before blaming the spindle.
Units mismatchOccasional
A factor of 25.4 is not subtle. Check the design, the CAM and the G20 or G21 line in the file.
Machine not squareLess common
Rectangles come out as parallelograms. See squaring.

Diagnostic steps

Measure the error with calipers, then find it in this table. The amount identifies the cause.

Error	Cause	Fix
Exactly one bit diameter undersize	Cut on the line instead of outside it	Set the profile offset to outside. See profile toolpaths.
Exactly two bit diameters undersize	Offset applied to the wrong side	Check which side the toolpath puts the tool on
About half a diameter, or some other odd amount, consistent everywhere	Bit diameter in CAM does not match the real bit	Measure the bit with calipers and enter the real number
A few thousandths oversize on an outside cut	Real bit diameter smaller than the value in CAM, or deflection	Measure the bit and enter the real number, then add a finishing pass
A few thousandths undersize on an outside cut	Runout, so the bit cuts wider than its diameter	See runout. Clean the collet first.
Error in one axis only	Steps per unit calibration wrong for that axis	Calibrate. Cut a long test cut, measure, and correct the setting.
Error scales with size	Steps per unit, or units mismatch	Check both, including whether the design imported at the right scale
Error by a factor of 25.4	Inches and millimetres mixed up	Check the design units, the CAM units, and the G20 or G21 in the file
Rectangle is a parallelogram	Machine not square	See squaring.
Walls tapered, so size depends on where you measure	Tool deflection	Add a finishing pass and reduce stickout

Calibrating steps per unit

If one axis is consistently off by a percentage, the machine's steps per millimetre or per inch setting is wrong for that axis.

Jog the axis a large known distance, as long as your machine allows. Longer is better because it makes the error measurable.
Measure the actual movement accurately with a good rule or calipers.
New value = old value multiplied by (commanded distance divided by actual distance).
Enter it, and repeat the test to confirm.

Test in air, not in a cut

Calibrating with a cut test mixes the steps-per-unit error together with deflection, runout and bit diameter error. Measure the axis movement itself with an indicator or a rule, and you isolate the one thing you are trying to fix.

Fixes, for parts that must fit

Set the offset side deliberately for every profile: outside for parts, inside for holes.
Measure the actual bit with calipers and enter that number in CAM.
Cut a test in scrap and measure before committing to the real material.
Leave an allowance and take a finishing pass, which removes deflection error.
Calibrate steps per unit if the error is a percentage, using the air test above.
Remember inside corners are round. A square peg will not enter a CNC-cut square hole without a dogbone relief.
Account for the material. Wood moves with humidity, and a joint cut to a perfect fit in a damp shop can bind in a dry one.

Why it happens

CAM never cuts your drawing. It cuts a path for the centre of a tool it believes is a certain size, offset from your drawing by the tool's radius. Every dimensional error is a disagreement between that belief and reality: the wrong radius, the wrong side, a tool that bent away from where its centre was, a spindle sweeping a bigger circle than the tool, or an axis that moved a different distance than it was told. Measuring the error tells you which belief was wrong.

Prevention

Keep a note of the measured diameter of every bit you own, and use those numbers in the tool library rather than the nominal size.
Preview the toolpath in CAM and look at which side of the line it sits before you post.
Calibrate each axis once, in air, and write the values down.
Make the finishing pass a habit on any part that has to fit something.