CNC operation guide

How Can Work CNC Machine: 6 Proven Steps From CAD to Part

A step-by-step walkthrough of what happens between your CAD file and a finished metal part. Written for design engineers and buyers who need to judge a process, not just watch it run.

Get Instant Quote Talk to an Engineer

±0.005 mm tolerance127 CNC machinesNo MOQ12-hour quote

How can work CNC machine: cutting tool path on a 5-axis machining center

On this page

Key takeaways

It runs a file, not a drawingThe controller reads G-code, moves servo axes, and never measures the part unless a probe is programmed.

Setup decides accuracy firstWorkholding and tool offsets cause more scrap than spindle speed ever does.

Roughing and finishing are separate passesOne pass cannot hold both a 6 mm chip load and Ra 0.8–1.6 μm.

Material sets the parametersAluminum 6061 and Ti-6Al-4V use completely different surface speeds and feed rates.

Inspection closes the loopWithout an in-process check, a worn tool drifts until the last part fails.

Section 1

What Happens Inside When You Ask How Can Work CNC Machine

A CNC machine works by executing a program, not by following a picture. CAM software turns your CAD model into G-code: a list of coordinates, feed rates, spindle speeds and tool changes. The controller reads that list line by line and sends position commands to servo motors on each axis.

The servo loop is the key detail. Each axis has an encoder that reports actual position back to the drive dozens of times per second. If the tool meets harder material than expected, the drive adds torque to hold position. That correction is why a machine can hold ±0.005 mm on a good day, and why it loses that accuracy when the setup is weak.

The cutting action itself is simple. A rotating tool with defined edges shears material away in chips. Heat leaves with the chips, so chip evacuation matters more than coolant brand. If chips recut, surface finish drops and tool life falls fast.

Three systems must agree before a cut is correct: the program, the tool offsets, and the work coordinate system. Get the first right and the other two wrong, and every part is scrapped at the same offset.

1
ControllerReads G-code, runs the motion and logic loops.
2
Drives and motorsConvert position commands into axis motion with encoder feedback.
3
Tool and spindleRemove material at a defined surface speed and feed per tooth.
4
WorkholdingHolds the part rigid enough that vibration stays out of the cut.

Section 2

Read the Drawing Before You Touch the Machine

Most operating errors are drawing errors in disguise. Before loading a program, confirm the datum. A part dimensioned from a centerline behaves differently from one dimensioned from a corner, and the work coordinate system must match the drawing exactly.

Then check tolerances against the process. A ±0.005 mm bore and a ±0.1 mm clearance hole should not share a tool or a pass. Tight features need a finishing allowance, a sharp tool, and often a temperature-stable room.

Look at the material callout too. Aluminum 6061-T6 machines cleanly at high surface speed. Ti-6Al-4V does not. Titanium conducts heat poorly, so the edge stays hot and the tool wears quickly. Lower the surface speed, keep the feed per tooth up, and never let the tool rub.

Finally, find the features that cannot be reached in one orientation. Undercuts, cross-holes and deep pockets usually force a second setup or a 5-axis move. Plan that before the first cut, because a re-fixtured part rarely repeats as well as one cut in a single setup.

1
DatumMatch the work coordinate system to the drawing datum.
2
Tolerance splitSeparate tight features from cosmetic ones.
3
MaterialAdjust surface speed and feed per tooth by alloy.
4
AccessIdentify features needing a second setup or 5-axis motion.

Section 3

Cutting Parameters That Actually Hold Tolerance

Parameters come in pairs: surface speed and feed per tooth. Surface speed sets tool life, feed per tooth sets chip thickness. A chip that is too thin rubs and work-hardens stainless. A chip that is too thick overloads the edge.

For aluminum 6061 with carbide tooling, a surface speed around 300–500 m/min and a feed per tooth of 0.05–0.15 mm is a normal starting range. For 304 stainless, drop surface speed to roughly 80–150 m/min. Titanium Ti-6Al-4V sits lower still, near 40–70 m/min, with generous coolant.

Roughing removes bulk with a large axial depth and moderate radial engagement. Finishing uses a small radial stepover, a sharp tool and a lighter feed to reach Ra 0.8–1.6 μm. Trying to finish in the roughing pass is a common cause of chatter marks.

Watch spindle load and sound during the first part. A load that climbs steadily across a pocket usually means chips are packing. Reduce radial engagement or improve evacuation before the tool breaks.

1
Aluminum 6061300–500 m/min, 0.05–0.15 mm per tooth.
2
Stainless 30480–150 m/min, keep the chip thick enough to cut.
3
Ti-6Al-4V40–70 m/min, flood coolant, no rubbing.

Procedure

Step by Step: How Can Work CNC Machine Run a New Part

Follow this order on the first article.

1
1. Confirm the CAM setup and stockCheck stock size against the model, plus 1–2 mm per side for facing. Verify the program datum matches the drawing datum. Wrong stock allowance is the most common first-run error.
2
2. Set the work coordinate systemTouch off X, Y and Z with an edge finder or probe. Record the values. On a probe-equipped machine, run the probe cycle and compare the result to the touch-off value; a mismatch above 0.02 mm means a dirty or loose datum surface.
3
3. Measure and load tool offsetsSet each tool length on the presetter or in the spindle. Enter the radius and length into the offset table. A single wrong length offset usually shows up as a crash on the first rapid move.
4
4. Prove the program in single blockRun with rapid override low and distance-to-go visible. Watch the first approach move. Keep a hand on feed hold until the first full cut is confirmed.
5
5. Cut the first article with coolant onStart at 70–80% of the calculated feed and speed, then increase. Listen for chatter and check chip shape. Thin, powdery chips on stainless mean the feed is too low.
6
6. Measure the first articleUse calipers for general sizes and a micrometer or bore gauge for tolerances under ±0.02 mm. Record actual values, not pass or fail. Trend matters more than a single reading.
7
7. Adjust offsets and run the batchApply the measured deviation as a wear offset, then run two more parts and re-measure. If the deviation repeats, the offset is right. If it drifts, the setup or the tool is moving.

Reference

Process Choice by Part Feature

Pick the machine configuration from the geometry, not the other way around.

Feature	Typical setup	Watch out for
Simple prismatic block	3-axis, one setup	Datum mismatch between ops
Deep pocket, tight corner	3-axis with small stepover	Tool deflection at long reach
Holes on four faces	4-axis with rotary table	Rotary backlash on indexing
Undercut or contoured surface	5-axis simultaneous	Post-processor and tool clearance
Shaft with milled flats	Mill-turn center	Part push-out during cutoff
Thin wall under 1 mm	5-axis, light radial pass	Vibration and spring-back
Large frame, 4,000 mm long	3-axis gantry-style travel	Thermal growth over long cuts

Send the drawing, get a manufacturability read

We review tolerances, datum strategy and setup count before quoting, so the price reflects a process that can repeat, not just one that can cut once.

Get Instant Quote Talk to an Engineer

FAQs

Common questions

Does a CNC machine measure the part while cutting?

Only if a probe cycle is programmed. Standard cutting relies on the servo loop holding commanded position, not on feedback about the part.

That is why in-process measurement and a final inspection step matter. Without them, a worn tool keeps cutting to the same coordinates while the part slowly grows or shrinks.

How do I choose a feed rate for a new material?

Start from surface speed and feed per tooth, then calculate spindle rpm and feed from the tool diameter and flute count.

Run the first part at reduced feed, check chip color and shape, then increase in steps. Record what worked so the next job does not repeat the experiment.

Why does the first part pass and the tenth part fail?

Tool wear moves the cutting edge, so the effective radius changes across the batch. Thermal growth in the spindle and the part adds to that drift.

Apply a wear offset after the first article, then re-measure every few parts. On long runs, schedule a mid-batch check rather than trusting the first result.

What causes chatter marks on a finished surface?

Usually a combination of long tool overhang, weak workholding and too high a radial engagement. The tool starts vibrating instead of shearing cleanly.

Shorten the overhang, add support under the part, reduce radial stepover, and keep the feed per tooth high enough to avoid rubbing.

Can thin or flexible parts be machined accurately?

Yes, but the strategy changes. Light radial passes, more axial depth, and support from soft jaws or a fixture that backs up the thin section.

Simultaneous 5-axis work helps because the tool stays normal to the surface and cutting force direction stays consistent.

What should I check before the batch run starts?

Confirm the offset trend across three parts, verify the tool has life left for the full batch, and make sure coolant flow reaches the cutting zone.

If any of the three is uncertain, stop and fix it. Scrapping a batch costs far more than one extra setup check.