How to Do Setups for CNC Machine Work
A setup decides whether the part comes off the machine on size or in the scrap bin. This guide walks through the sequence our machinists use on 3-axis, 4-axis and 5-axis work, from workholding choice to first-article sign-off. Written for engineers and shop leads who need a repeatable procedure, not a theory lesson.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
- 8
Key takeaways
Plan the Workholding Before the Program
Most bad setups are decided before the machine is even free. Start with the part geometry: where can a vise, chuck, or fixture plate grab it without blocking the surfaces that need cutting? If the answer is nowhere, the process needs two operations, and the setup sheet needs to say so.
Look at the stock allowance next. A block with 1 mm of material to remove behaves very differently from a casting with 6 mm of varying skin. Thin walls below 1.5 mm will deflect under clamping pressure, so plan support or use low-pressure fixturing rather than a standard vise jaw cranked tight.
For parts longer than about 400 mm, consider how the material will move after the first face is machined. Stress relief in the stock is real. A part that measures flat at setup may bow 0.05 mm after the second side is opened up. Our 4,000 mm maximum processing size machines still need the same discipline.
Write the setup sheet while you plan. It should name the fixture, the zero point, the tool list with holder numbers, and the inspection points. If a machinist cannot set the job from that sheet without calling you, the sheet is not finished.
- 1Rule of thumbIf clamping marks would land on a finished surface, redesign the fixture, not the finish callout.
- 2Watch forChips that cannot escape a deep pocket will recut and break small end mills.
Set the Zero Point and Document It
The zero point is where the machine believes the part lives. For prismatic parts we normally use a corner: X and Y on two machined datum edges, Z on the top face or on a gauge block of known height. For round parts going into a chuck or a Ø400 mm rotary table, center is more natural and easier to re-establish after a power loss.
Touch off with a 3D taster or an edge finder, then verify with an indicator on a known feature. A 0.02 mm error at the zero point becomes 0.02 mm on every dimension in that axis, so this step deserves more time than it usually gets.
On 4-axis and 5-axis work, the rotary centerline must be dialed in, not assumed. Sweep the chuck or fixture with a test indicator and record the runout. If the rotary axis is out by 0.03 mm, every indexed face inherits that error, and no amount of tool compensation will fix it.
Record the zero point in the setup sheet with the exact method used. "Corner, left rear, top face" is not enough. Write the datum feature, the gauge height, and the probe routine if one was used.
Tool Length and Diameter Offsets Done Right
Tool length offset errors are the single most common cause of crashes we see. Each tool, holder, and pull stud combination has its own length, and it changes slightly with spindle temperature. Touch off all tools at the start of the shift, not at the start of the week.
Use a tool presetter if you have one, but confirm the first tool in the spindle against the machine. Presetter and machine zero can differ by 0.01 to 0.03 mm depending on how the taper seats. That is enough to matter on a ±0.005 mm callout.
Diameter offset is where the machinist controls size. Start conservative: leave 0.1 mm on finishing passes, measure, then adjust the offset toward the nominal. Chasing size by editing the program instead of the offset makes the next run unpredictable.
Keep a tool list on the machine with holder numbers, offsets, and remaining life. When a tool is replaced mid-run, the new tool goes into the same offset number and the first part off is inspected before the run continues.
Dry Run, Clearance Check, and First Cut
Before the spindle turns, run the program with the Z offset raised by 50 mm and the rapid feed at 25 percent. Watch the distance-to-go display, not the moving axes. The display tells you what the control is about to do, which is what matters.
Check clearances at the extremes: the highest Z, the lowest Z, the longest tool, the shortest tool. A long drill in a deep pocket is where holders hit vises. If the setup uses a tailstock or a rotary unit, rotate the axis through its full range while watching the gap.
The first cut should be a conservative one. Reduce feed and speed by 30 to 40 percent on the first part, then step up once the tool is in a stable cut. This is not about being slow. It is about hearing and feeling the cut before the machine is running at full parameters.
Measure the first feature before the second is cut. If X is out by 0.15 mm, stop and fix the offset. Cutting the whole part and then measuring wastes the part and the setup.
Common Setup Mistakes and How They Show Up
The most expensive mistakes are quiet ones. A part that is 0.08 mm out of position on the second operation still looks correct until assembly, when the bolt holes will not line up. This is almost always a zero point that was re-established from a different feature than the first operation used.
Clamping distortion is the second. A vise tightened to 40 N·m on a thin section can close a slot by 0.1 mm. Release the part and it springs back. If measurements only make sense while the part is clamped, the setup is the problem.
Tool offset drift is the third. A holder that is not fully seated in the taper adds 0.02 to 0.05 mm to the tool length. The cut looks fine until a depth callout is checked with a micrometer.
Finally, undocumented changes. If the night shift adjusts an offset and does not write it down, the morning shift repeats the same mistake. A setup log on the machine is cheap insurance.
Step by Step: Setups for CNC Machine Work
- 1Clean the machine and the fixtureWipe the table, vise, and chuck faces. A chip under a vise jaw tilts the part. Check the taper for fretting or dents before loading a holder.
- 2Mount and indicate the workholdingClamp the vise or fixture and sweep it with a test indicator. Parallelism to the X axis should be within 0.01 mm over 100 mm. Re-check after tightening.
- 3Load the stock and set the zero pointSeat the part against the stops, then touch off X, Y, and Z. Use a gauge block for Z if the top face is rough. Record the method in the setup sheet.
- 4Load tools and touch off lengthsLoad in program order. Touch off each tool on the same reference surface. If a presetter is used, confirm tool 1 in the spindle.
- 5Verify the program and offsetsCheck the active work offset number and the tool offset numbers against the sheet. A wrong offset number is worse than a wrong value.
- 6Dry run at raised ZRaise Z by 50 mm, run at 25 percent rapid. Watch distance-to-go. Fix any clearance issue before the first cut.
- 7Cut the first article conservativelyReduce feed and speed by 30 to 40 percent. Measure the tightest tolerance on the drawing before continuing.
- 8Log the result and release the runRecord the measured values, the offsets used, and any adjustment made. The next setup on this part starts from that record.
Which Setup Approach Fits the Job
Match the fixture and zero point to the part, not to habit.
| Part situation | Setup approach | What to watch |
|---|---|---|
| Block, 3 faces open | Vise, corner zero | Parallelism after clamping |
| Thin wall under 1.5 mm | Soft jaws or vacuum plate | Clamp pressure and wall spring |
| Round part, turned features | 3-jaw chuck, center zero | Chuck runout and jaw marks |
| Features on 4 sides | 4-axis with rotary table | Rotary centerline dialed in |
| Complex contoured surfaces | 5-axis, single setup | Collision check across full travel |
| Long shaft over 400 mm | Steady rest or tailstock | Deflection and thermal growth |
| High mix, low volume | Modular fixture plate | Repeatability of pin locations |
A setup is done when it is documented
If the zero point, offsets, and first-article measurements are not written down, the next run starts from zero. Build the log into the process and the setup time drops every time the part comes back.
Setup questions we get asked
How long should a setup take?
It depends on the number of operations and how much of the part is open. A simple 3-axis vise job with four tools can be set in under an hour. A 5-axis job with a custom fixture, multiple zero points, and a dozen tools often takes half a shift.
The time worth protecting is the verification, not the clamping. Dry run and first-article checks are what keep a two-hour setup from turning into a scrapped batch.
Should I use a corner zero or a center zero?
Use a corner zero for prismatic parts that sit against hard stops. Use a center zero for round parts in a chuck or on a rotary table, because the center is easier to re-establish after an interruption.
Whichever you choose, use the same one across all operations on that part. Mixing methods between operations is a common source of position error.
Do I need to touch off every tool every time?
Yes, at least once per shift and after any holder change. Tool length is affected by how the taper seats, by pull stud torque, and by spindle thermal growth.
If you use a presetter, treat its numbers as a starting point and confirm the first tool in the spindle. A 0.02 mm difference is normal and matters on tight tolerances.
What tolerance can a good setup hold?
On our machines, setups are built to hold ±0.005 mm on critical features, with surface finish from Ra 0.2–0.8 μm where the process supports it.
That number depends on the part as much as the machine. A long, thin part will not hold ±0.005 mm no matter how good the setup is, because deflection and thermal movement dominate.
How do I stop chips from ruining a setup?
Plan chip evacuation at the fixture design stage. Air blast, through-tool coolant, and a fixture that does not trap chips in pockets all help.
Before loading a part, blow off the fixture and the locating faces. A single chip under a stop is enough to shift the part by 0.05 mm.
When should I move a job to 5-axis?
When the part has features on multiple faces and the tolerance stack from moving it between fixtures is larger than the tolerance itself. One setup removes the re-datum error entirely.
It is not always faster. On simple parts, a 3-axis vise job with two operations can still be the cheaper route.
Send us the drawing and we will flag the setup risks
Upload a STEP file and we return quotation and DFM feedback within 12 hours, including notes on workholding, datum strategy, and any feature that will be hard to hold.
12-hour quoteFree DFM analysisNDA on request
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
