Holding Size on a CNC Run: Tool Wear, Drift, and Offset Decisions

Making one good part is a setup skill. Making 800 good parts in a row is a different skill. Tools wear, machines warm up, and each measurement carries a little noise. A mid-level operator knows which of those is moving the size, how much correction it needs, and when to leave the machine alone. Bad decisions here go both ways: the person who never adjusts runs out of tolerance, and the person who adjusts after every part makes the process worse.

What You Will Be Able to Do

• Plan where to start a dimension so tool wear carries it through the tolerance.
• Set an action limit and work out how many parts you can run between corrections.
• Tell real drift from measurement noise before you touch an offset.
• Allow for machine warm-up and handle an insert change without losing size.
• Spot size problems that no offset can fix.

How Size Moves During a Run

Tool wear is usually slow and steady in the middle of a tool's life. A worn turning tool has lost a little of its edge, so it cuts less deep. That means:

If you plot size against part count, you get a sawtooth. The size climbs slowly, you correct it back down, and it climbs again. Starting at the middle every time wastes half of your room. Starting low on an outside diameter gives the wear the whole band to travel through.

New edges often wear a bit faster for the first few parts, and a tool near the end of its life wears fast again. The steady middle is where your math works. Near the end of life, stop trusting the old rate.

Planning Corrections With Real Numbers

Worked example. You turn an outside diameter of 1.2500 +/- 0.0010 on a long run. Your log from the last run shows the diameter growing about 0.00015 inch for every 25 parts. Your micrometer and method can repeat to about 0.0002 inch.

1. The tolerance runs from 1.2490 to 1.2510.
2. Stay 0.0002 away from each limit, to allow for measurement error. Your working band is 1.2492 to 1.2508, which is 0.0016 wide.
3. The size grows 0.00015 every 25 parts. To cross the band takes 0.0016 / 0.00015 = about 10.7 steps of 25 parts, or roughly 265 parts.
4. Set your action limit at 1.2508. When a reading reaches it, you correct.
5. Correct back toward the low end. From 1.2508 to 1.2494 is 0.0014 on the diameter.

On a control in diameter mode, you enter -0.0014 in X wear. On a control in radius mode, you enter -0.0007. Either way, the tool moves 0.0007 inch toward center.

The action limit is not the tolerance limit. Reaching the action limit means a normal correction. Reaching the tolerance limit means something got past you, and you may have parts to contain.

Do Not Chase Noise

Every measurement has some scatter. If you correct for that scatter, you add the error of the gauge to the size of the next part.

Picture a stable process. Its size varies at random around a good center. If you shift the offset by the full error after every part, you make the spread about 40 percent wider than if you had left it alone. The math comes out to the spread growing by a factor of the square root of 2. Quality people call this tampering. It looks like hard work and it scraps parts.

Use these habits before you change an offset:

1. Measure more than one part. Take the average of the last three parts or so. One odd reading is not a trend.
2. Compare with your repeat. If your gauge repeats to 0.0002 and the size moved 0.0001, you have seen nothing yet.
3. Check the measurement. Clean the part and the gauge. Let the part cool. Check the gauge against a master if the reading surprises you.
4. Ask what changed. If nothing changed and the reading is inside the action limit, leave it alone.

Worked example. Your action limit is 1.2508. The last three checks read 1.2505, 1.2509, 1.2504. One reading is over the limit, but the average is 1.2506. Measure that part again and check the next one. Do not correct yet. If the next three read 1.2507, 1.2508, 1.2509, the average is 1.2508 and the trend is real. Now you correct.

Reading the Pattern in Your Log

Write down each check in order, and look at the shape as well as the latest number.

A step change is a warning. Tools do not lose 0.003 inch in one part from normal wear. Something broke or moved. Stop, look at the insert and the part, and do not correct until you know why. Part of the run may already be bad.

Heat and Warm-Up

A machine is made of metal, and metal grows when it warms. Spindle bearings and ball screws heat up as they run, so the tool's real position moves during the first part of a shift.

Steel grows about 0.0000065 inch per inch for each degree F. A 20-inch length of ball screw that warms 5°F grows 20 x 5 x 0.0000065 = 0.00065 inch. On a job with a 0.001 tolerance, that matters. Many modern machines reduce this with cooled screws and software, but do not assume yours does.

Practical rules:

• Run the machine's warm-up routine before tight work. A common approach is to run the spindle and axes for 15 to 30 minutes, or for whatever time your shop has shown works.
• Measure the first parts after a cold start more often.
• After a lunch break or a long stop, check the first part before you run again. The machine has cooled and the size can move back.
• Keep the cycle steady. A machine that runs all the time holds size better than one that stops and starts.
• Check the coolant. A tank that heats up during the day warms the part as well.

If the size moves in the first hour and then settles, that is warm-up. If you correct for it, you may have to correct back after a long stop. Note the pattern in your log so the next shift expects it.

Changing an Insert or Tool

An insert change is the biggest size event in a normal run, so treat it like a small setup.

1. Stop at a planned point. Follow your tool-life count or part count, not your gut.
2. Clean the pocket. A chip under an insert tilts it and can break it.
3. Tighten to the torque the insert maker lists. Over-tightening can crack the insert or strip the screw.
4. Reset the wear value as your shop directs. Many shops have a known starting value on the setup sheet.
5. Move the size a little in the safe direction for the first part, so it comes out with stock rather than undersize.
6. Measure the first part after the change. Correct, then log it.

Worked example. Your setup sheet says the insert baseline is X wear 0.0000. The worn insert had reached -0.0038 in diameter mode. A new edge cuts deeper than the old one did by about that amount, so you reset to 0.0000. To be safe, enter +0.0010 instead, cut one part, measure it, and bring it down to the target. Keeping the old -0.0038 would cut the first part about 0.0038 undersize on the diameter, which is scrap on this tolerance.

Sister tools, also called backup tools, can be switched in by the control when a tool-life count runs out. They need their own offsets and their own check. A sister tool that was set a month ago is a new tool as far as size is concerned.

When One Tool Cuts Several Features

A wear offset moves everything that tool cuts. If one finish tool cuts two diameters, and only one is drifting, an offset that fixes one breaks the other.

Good programs avoid this by giving the tool two offset numbers, one for each feature. On a lathe, T0303 might cut the first diameter and T0313 the second, using the same insert with its own wear value. On a mill, the program might call D21 for one bore and D22 for another. If your job needs this and the program does not have it, ask the programmer. Do not rewrite it yourself.

Roughing tools rarely need a wear correction, because the finish tool sets the size. Watch the roughing tool anyway. A worn rougher leaves more stock, the finish tool sees more force, it deflects more, and the size moves. If the finish size changes right after a rough insert change, this is why. The fix is to keep rough wear under control, not to keep adjusting the finish tool.

Problems an Offset Cannot Fix

An offset moves the whole cut. If the error changes along the feature, or from part to part, a different number will not cure it.

A spring pass is a second pass at the same setting with no change in offset. It removes what the tool left the first time because it bent. It adds time, so it is a choice for the setup person or programmer.

If an offset moves one end of the feature into tolerance and pushes the other end out, you have proved the problem is not the offset. Stop adjusting. Report what you measured at each end.

When a Check Fails

There is a big difference between a reading past your action limit and a reading past the tolerance limit.

1. Past the action limit: make a planned correction, measure the next part, log it.
2. Past the tolerance limit: stop the run. Tag the part. Go back to the last check that was good. Everything since then is suspect until it has been checked.

Worked example. You check every 25 parts. Part 200 read 1.2507. Part 225 reads 1.2512, over the 1.2510 limit. Parts 201 through 225 are suspect, so that is 25 parts to measure, and you sort them by the real number. Then ask why your check did not catch it. A jump of 0.0005 in 25 parts is three times your normal wear rate, so look at the tool before you restart.

Common Mistakes

Check Your Understanding

1. A bore has a tolerance of 0.7500 +0.0010 / -0.0000. Where should you start the run, and why?

Near the top of the tolerance, about 0.7508. A worn boring tool cuts a smaller bore, so the size moves down through the band.

2. Your action limit is 1.0006. Readings over the last three checks are 1.0003, 1.0007, 1.0002. Do you correct?

Not yet. The average is 1.0004, under the limit, and one high reading in the middle looks like noise. Remeasure that part and watch the next few.

3. Size has climbed 0.0001 every 30 parts all morning. Then one part reads 0.0025 larger than the one before. What do you do?

Stop. That is a step, not wear. Look at the insert for chipping and check the holder and the part seat. Do not correct the offset until you know the cause, and go back to the last good check.

4. A long shaft measures 0.9995 near the chuck and 1.0015 near the free end. A coworker says to take 0.001 off the diameter with X wear. What happens if you do?

The free end comes down to about 1.0005 and the chuck end drops to about 0.9985, so you have only moved the error. The taper comes from the part bending away from the tool. It needs more support or a lighter finish cut.

5. You have an 80-part check interval and a wear rate of 0.0002 per 20 parts. Your band is 0.0006 wide. Is the interval safe?

No. In 80 parts the size moves 0.0008, more than the whole band. Check more often, at least every 40 parts, so you see the trend well before it reaches the limit.

Key Takeaways

• Start a dimension at the end of the tolerance that wear moves away from, and correct at a planned action limit.
• Do not correct on one reading. Over-adjusting widens the spread of a stable process.
• Slow change is wear. A sudden step means something broke or moved, so stop and look.
• Machines grow as they warm, so check more often after a cold start or a long stop.
• Treat every insert change as a small setup, with a reset, stock on the first part and a measurement.
• An offset moves the whole cut. It cannot fix taper, deflection or a part that is not seating.