How to Run a CNC Machine
This guide covers the setup sequence we use on the floor: workholding, tool offsets, dry run, first cut, and first-article inspection. It is written for machinists and engineers who need to know which checks actually prevent scrap, and which ones only look safe.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
What you need in place before you run a CNC machine
Running a CNC machine is not a single action. It is a chain of small confirmations, and the part fails at whichever link you skipped. On a 3-axis vertical mill, the chain starts with a clean table and a vise that is indicated square to the X axis within 0.02 mm. On a lathe, it starts with a chuck that grips the bar stock over enough length to resist the cut.
You need four things ready before the first rapid move: a posted program you have read, a workholding setup that will not move, tool data for every tool in the carousel, and a stock allowance that leaves material for a finishing pass. If any of those is vague, stop and fix it. A program that is 90 percent correct scraps parts just as fast as one that is wrong everywhere.
Match the machine to the part. A 500 × 500 × 450 mm envelope handles most plates and housings. Deep pockets with undercuts need a 5-axis center, and turning with cross-drilling needs a mill-turn. Running a simple part on a large machine wastes setup time; running a complex part on a 3-axis machine means extra fixtures and extra chances for error.
- 1Drawing and revisionConfirm you are holding the current revision, not a superseded PDF.
- 2Stock checkMeasure the blank. Programmed stock that is 0.5 mm thin will cut air on the finish pass.
- 3Tool listEvery tool in the program must exist in the carousel with a measured length.
- 4Coolant and airCheck level and nozzle direction before the first tool enters the cut.
Vise, fixture, and zero position
Clamp the part so the cutting force pushes it into the jaws, not out of them. On a vise, that means the fixed jaw takes the load and the movable jaw only holds. For a 50 mm face mill at 2 mm depth of cut in 6061, the side force is significant; a part held only by friction will creep and the finished thickness will drift.
Set the work zero from a feature the drawing controls, not from whatever edge is convenient. If the drawing dimensions from the center bore, zero on the center bore. If it dimensions from a corner, indicate that corner. Every downstream measurement inherits this choice.
Thin plates need support under the cut. A 6 mm aluminum plate spanning an open vise will ring and chatter at 3,000 rpm. Support it with parallels or a sacrificial plate, and keep the overhang short. For parts with a finished face that must not be marked, use soft jaws machined to the part profile.
- 1Indicate the viseSweep the fixed jaw. Correct anything over 0.02 mm over 200 mm.
- 2Seat the partTap it down onto parallels and check with a feeler gauge that it is not rocking.
- 3Stop against a hard stopFor repeat batches, a stop pin gives you the same X zero on every part.
Tool offsets, feeds, and spindle speed
Touch off every tool and enter the length offset before you press cycle start. A missing offset on tool 4 is the most common crash we see. Use a tool presetter if the machine has one; if not, touch off on a known surface and record the value. Diameter offsets matter for cutter comp, so measure a new end mill rather than trusting the nominal size.
Set feeds and speeds from the material and the tool, not from habit. In 6061 aluminum with a 10 mm carbide end mill, 0.05–0.1 mm per tooth at 3,000–4,000 rpm is a reasonable starting window for roughing. In 304 stainless, drop to 0.03–0.05 mm per tooth and 800–1,200 rpm, and expect to take lighter radial cuts. Titanium Ti-6Al-4V runs slower again; heat goes into the tool, so coolant flow matters more than speed.
For finishing, the stepover decides the surface finish more than the feed rate does. A 0.2 mm stepover with a 10 mm tool at Ra 0.8–1.6 μm is typical for a semi-finish pass. If the drawing calls for Ra 0.2–0.8 μm, plan a separate finishing tool with a small corner radius and keep the stepover under 5 percent of the cutter diameter.
- 1RoughingDeep radial cuts, moderate feed. Leave 0.3–0.5 mm for finishing.
- 2FinishingSmall stepover, higher speed, light depth. Control the finish here.
- 3Deep pocketsUse a smaller tool with a shorter flute length to reduce deflection.
- 4CoolantFlood for steel and titanium. Air blast for aluminum and plastics.
Dry run, single block, and distance-to-go
Before the first real cut, raise the tool 50 mm above the part and run the whole program with rapid override reduced. Watch the distance-to-go screen on every approach. If a rapid move heads toward the vise rather than the stock, you catch it with the feed hold button, not with the e-stop after the crash.
Then run the first part in single block for the first few tools. Check that the tool actually enters the material where you expect, and that the sound is steady. Chatter, a high-pitched squeal, or a load meter climbing past 70 percent all mean stop and adjust.
Keep a setup sheet with the program number, offsets, tool list, and any notes from the run. The next time the part comes back, that sheet saves an hour. It also tells the next operator which tools were changed and why.
- 1Verify the program numberLoading the wrong program is a classic first-shift error.
- 2Check the plane and unitsG17/G18/G20/G21 before the first move.
- 3Confirm the work offsetG54 for the vise, G55 for the second op. Say it out loud.
Step by step: how to run a CNC machine
Follow this order on a vertical mill or a lathe.
- 1Clean and inspect the machineWipe the table and taper. Check way lube level and air pressure. Remove chips from the vise jaw faces; a chip under the part tilts it.
- 2Mount and indicate the workholdingSet the vise square to X within 0.02 mm over 200 mm. For a chuck, check runout at the gripping length.
- 3Load and seat the stockTap down onto parallels. Confirm the top of the stock sits 0.5–1.0 mm above the jaw for clearance.
- 4Set work zeroEdge-find or indicate the datum feature. Store it in the correct work offset. Verify by moving to the zero point and reading the position screen.
- 5Measure every toolTouch off length and diameter. Enter values in the offset table. Double-check the tool number against the program.
- 6Dry run above the partRaise Z by 50 mm. Run the full program with rapid override at 25 percent. Watch distance-to-go.
- 7Cut the first part at reduced feedStart at 50 percent feed override. Watch the load meter and listen. Increase only when the cut is stable.
- 8Inspect before releasing the batchMeasure the first part against the drawing. Check critical dimensions, then release the run.
Starting parameters and setup checks by machine type
Ranges are starting points. Adjust for tool geometry, rigidity, and coolant.
| Machine type | Typical use | Setup check | Starting window |
|---|---|---|---|
| 3-axis mill | Plates, housings, open pockets | Vise square to X within 0.02 mm | 0.05–0.1 mm/tooth in 6061 |
| 4-axis mill | Parts on multiple faces | Rotary centerline to spindle | Reduce feed 20% on the A axis |
| 5-axis mill | Complex contours, undercuts | Verify post and RTCP offsets | Light radial cuts, short tools |
| Mill-turn | Shafts with cross features | Chuck grip length and runout | Turning 0.15–0.3 mm/rev in steel |
| CNC lathe | Round parts, threads | Bar feed alignment and stop | 300–600 sfm in aluminum |
The check that saves the most parts
If you only do one thing before the spindle turns, run the whole program 50 mm above the stock and watch the distance-to-go readout. It catches missing offsets, wrong work coordinates, and clamp collisions in under a minute.
Common questions
What is the difference between 3-axis and 5-axis CNC machines?
A 3-axis machine moves the tool in X, Y, and Z. The part stays in one orientation, so any feature on a side face needs a second setup or a custom fixture.
A 5-axis machine adds two rotary axes, so the tool can reach undercuts and angled faces in one setup. That reduces fixture count and holds position between features better. It also costs more per hour, so use it where the geometry demands it.
How do I program a CNC machine?
Most shops program in CAM from a 3D model, post the toolpaths to G-code, then verify the code in a simulation before it reaches the machine.
Manual G-code still has a place for simple facing, drilling, and quick edits at the control. The risk is the same either way: an unverified program goes into the spindle. Simulate first.
What safety measures should I take when operating a CNC machine?
Close the door before cycle start. Keep hands out of the envelope while the spindle is armed. Know where the feed hold and e-stop are without looking.
Wear safety glasses when the door is open and chips are flying. Never reach into a running machine to clear a chip. Use a hook or stop the spindle.
How do I maintain a CNC machine?
Daily: check way lube, air pressure, and coolant level. Weekly: clean the chip conveyor and check the taper for damage. Monthly: inspect belts, filters, and level the machine if it has moved.
Keep a log. Bearing noise, rising spindle load, and drifting position all show up in the log before they become a breakdown.
What materials can be machined with a CNC machine?
Aluminum 6061, 7075, and 2024; stainless 303, 304, 316L, and 17-4PH; steels 1018, 1045, 4140, and 4340; copper and brass; titanium Ti-6Al-4V; Inconel; and plastics such as POM, PEEK, and PC.
The setup changes with the material. Titanium and Inconel need slower speeds, rigid tooling, and heavy coolant. Plastics need sharp tools and air blast instead of flood coolant.
How do I know the first part is good before running the batch?
Measure the critical dimensions on the first part against the drawing. Check the ones that stack up from your work zero, since those inherit any zero error.
If the first part is in tolerance and the cut was stable, release the run. If it is close but drifting, adjust the offset before the second part, not after the tenth.
Need a shop that already runs this process
Send your CAD files and get a quotation with free DFM analysis within 12 hours. We run 127 high-precision CNC machines across 3 plants, hold ±0.005 mm, and inspect 100 percent of parts before shipment.
12-hour quote100% inspectionNo minimum order quantity
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
