CNC Cycle Time Reduction Without Losing Capability

A shop makes money on the minutes a part takes. But a faster cycle that scraps parts, or needs an offset every ten pieces, costs more than it saves. The senior skill is knowing where the time really goes, taking out the waste first, and only then pushing the cut, with data showing that the process still holds. This also covers holding size on hard jobs, because a fast process you cannot trust is no use to anyone. Reminder: any change to feeds, speeds or toolpaths goes through your program control process, and it may need a new first article.

What You Will Be Able to Do

• Time a cycle by element and find the biggest target.
• Remove air cutting, tool changes and rapid time before you touch the cut.
• Compare a slotting path with a high-efficiency path using real numbers.
• Weigh speed against tool life with a simple calculation.
• Use Cpk to check that the change did not damage the process.

Measure Before You Change

People guess wrong about where the time goes. Run the job and break the cycle into elements. Use the block times from the control, a stopwatch, or video.

Worked example. A bracket has a cycle of 7 minutes 20 seconds, or 440 seconds.

Only 54 percent of the time is removing metal. The other 46 percent, about 204 seconds, does not cut anything. Most of that can be reduced without risking tool life or finish. So you start there.

Also ask if the machine is the constraint. If the next operation can only take 7 parts an hour, saving a minute on this machine adds a pile of parts and no extra output. Check the whole line before you spend your time.

Order of Attack

Work in this order, from lowest risk to highest.

1. Remove air cutting and wasted moves.
2. Cut tool changes.
3. Cut load and unload time.
4. Improve roughing.
5. Touch finish passes last, if at all.

Finish passes set size and surface. Roughing only has to remove material. A change to roughing rarely hurts capability. A change to finishing often does.

Air Cutting

Air cutting means feeding at cutting speed where there is no material. CAM defaults often cause it, with big safety clearances and long lead-ins.

• Bring the tool to a short approach height at rapid, and start feeding close to the stock. Allow for the real variation in the stock. A casting needs more room than a machined blank.
• Trim lead-ins and lead-outs to what the tool needs.
• Use the real stock model, so that CAM does not cut where the material is already gone.

Retract Heights

Each hole in a canned cycle has a retract. Where there are no clamps in the way, use G99 and a low R plane.

Worked example. A plate has 120 holes. Going from a 1.0-inch retract to 0.1 inch saves 0.9 inch up and 0.9 inch down at each hole. At 1,000 IPM rapid, 1.8 inches takes 0.108 second, so 120 holes saves about 13 seconds. The real saving is often a bit more, because shorter moves spend less time speeding up and slowing down. Check the fixture first. A low retract across a clamp is a crash.

Tool Changes

Each tool change costs time, plus the moves to and from the tool change position.

• Combine tools. A spot drill that also chamfers removes one tool. A form tool can replace two.
• Order operations to reduce changes, and on multi-part setups, run each tool across all the parts before you change it.
• Move to the tool change position with only the axes you need.

Load and Unload

These seconds are easy to overlook.

• Use a pallet changer or a second fixture, so that loading happens while the machine cuts.
• Use fixtures that load fast and cannot be loaded wrong.
• Stage parts, gauges and deburring within reach.

When an operator can do the next part's deburring while the machine runs, that work leaves the cycle. If all of that work is hidden inside the cut time, your real cycle is only the machine's time.

Adding It Up

Suppose you get 40 seconds from air cutting, 13 from retracts, 12 from two fewer tool changes and 5 from waits. That is 70 seconds, with no change to any cut.

• Before: 440 seconds, or 3,600 / 440 = 8.2 parts an hour.
• After: 370 seconds, or 9.7 parts an hour, a gain of 19 percent.
• On a 5,000-part order, that saves 70 x 5,000 / 3,600 = about 97 machine hours.

Better Roughing

Slotting Versus High-Efficiency Milling

A full slot engages the tool's whole width. Heat stays in the tool and only a small part of its length does the cutting. High-efficiency milling (HEM), also called trochoidal or dynamic milling, takes a narrow width at a large depth. It uses more of the flute, spreads the wear, and gives heat time to leave.

A narrow cut also makes a thinner chip than the feed per tooth suggests. To keep the same real chip, you raise the feed.

Adjusted feed per tooth = target chip x D / (2 x square root of (D x WOC - WOC squared))

Here D is the tool diameter and WOC is the width of cut.

Worked example. A 1/2-inch, 4-flute end mill in mild steel.

For the HEM column, the thinning factor is 0.5 / (2 x square root of (0.05 - 0.01)) = 0.5 / 0.4 = 1.25, so a 0.003 target becomes 0.00375. Material removal is width x depth x feed, so 0.100 x 1.000 x 68.8 = 6.9.

That is 33 percent more metal an hour, with wear spread along four times as much flute. The HEM path needs a rigid setup, a holder that grips well, a tool made for the job, a machine that can hold the feed, and a CAM system that keeps engagement steady. Feeds from thinning formulas can get very high at small widths, so raise them in steps and watch the load meter.

Speed Versus Tool Life

Speed has a price. Taylor's tool life equation describes how tool life drops as surface speed rises:

New life = old life x (old speed / new speed) raised to the power of 1/n

Textbooks often give n as about 0.25 for carbide, though real values vary a lot with the tool and material. Your own tool-life records beat any book.

Worked example. A carbide tool runs at 400 SFM, spends 60 seconds in the cut per part, and lasts 200 parts. You want to try 480 SFM, a 20 percent increase.

1. With n = 0.25, life changes by (400 / 480) to the 4th power = 0.48.
2. Tool life in cut time was 200 minutes. It falls to about 96 minutes.
3. Cut time per part falls to 50 seconds, so the tool now lasts 96 x 60 / 50 = about 115 parts.
4. Per 1,000 parts: tool changes go from 5 to about 9. At 4 minutes for each, including a first-part check, that adds about 16 minutes.
5. Time saved: 10 seconds x 1,000 = 167 minutes.

Here it is worth it. You also use nearly twice as many tools, and each one drifts faster. So price the tools, and watch size, before you call it a win. A tool that wears twice as fast may also need more frequent corrections. On an unattended run, a shorter tool life can matter more than the seconds you saved.

Protecting Capability

Capability is how well a process fits inside the tolerance. Cpk compares the distance from the process average to the nearer limit with three standard deviations of spread. A higher number means more margin. Many plans ask for 1.33 or more on ongoing production, but use your customer's figure.

Run a short study before and after each significant change. Use the same gauge and the same method.

Worked example. A bore is 1.0000 +/- 0.0020. Thirty parts before the change average 1.0003, with a standard deviation of 0.0004.

• Upper side: (1.0020 - 1.0003) / (3 x 0.0004) = 1.42
• Lower side: (1.0003 - 0.9980) / (3 x 0.0004) = 1.92
• Cpk is the smaller, 1.42.

Someone raises the finish feed to save 9 seconds. Thirty new parts average 1.0004, with a standard deviation of 0.0005.

• Upper side: (1.0020 - 1.0004) / (3 x 0.0005) = 1.07

Cpk has dropped to 1.07, under a 1.33 target. The parts still pass inspection, so no one would notice from the reject count, but the margin has gone. Put the finish feed back, and keep your other savings.

Keep the sample honest. A study run with a fresh tool on a warm machine in one hour shows less spread than a full tool life on real shifts. Short studies are good for comparison. Long-term results need real production data.

Holding Tight Features on Hard Jobs

Some features sit at the edge of what the process can do. Speed is the wrong thing to chase on those. Build the process around them.

Spindle probing lets the machine measure a feature during the cycle and update a wear offset. It costs seconds, and it can pay for itself on a tight feature or an unattended run. It needs care:

• A probe is a measuring system, so check its repeat and accuracy against a known standard.
• Clean the feature before you probe it, with coolant or an air blast.
• Limit how much a macro may correct, and alarm on anything larger.
• Remember that a warm part measures large. If the part is hot, probing can correct to the wrong size.

Steady running helps too. A machine that keeps the same rhythm holds its temperature, so long stops can cost you more in drift than they save.

Getting the Change Approved

A faster process is a changed process. Depending on your customer, you may need a new first article, a new capability study, or the customer's approval. Aerospace and automotive customers often restrict changes after approval. Bring quality in before you change a released job.

Record what you changed, the before and after times, the capability result and the tool life. The next person will want to know what you tried, and why.

Common Mistakes

Check Your Understanding

1. A cycle shows 300 seconds, with 120 in air cutting, tool changes and rapids. Where do you start?

There. That 40 percent carries little risk to the part, so reduce it before you change any cut.

2. A programmer switches a slotting job to a narrow high-efficiency path but leaves the old feed in place. The tool rubs, and the chips look like dust. Why?

A narrow cut makes a thinner chip than the feed per tooth suggests, so the chip is now too thin to cut well. Raise the feed using the thinning factor, in steps, and watch the load meter.

3. Raising speed 10 percent takes a tool's life to about 68 percent with n = 0.25. Is that automatically bad?

No. Work it out in full. Compare the time saved with the added changes, tool cost and any size drift.

4. A process had a Cpk of 1.5, and after a change it has 1.1, with no rejects. Is that a problem?

Yes. The margin has shrunk, and rejects may come when the tool wears or conditions change. Compare it with your plan's target, and reverse the change if it falls short.

5. You could save a minute on a lathe that makes 9 parts an hour, but the grinder after it only takes 7. What does that minute gain you?

No extra output. The grinder is the limit, so faster turning only piles up parts in front of it. Put your effort into the grinder, or into a job where this lathe is the constraint.

Key Takeaways

• Time the cycle by element before you change anything.
• Take out air cutting, tool changes and waits first. They are low risk.
• Improve roughing before finishing. Finish passes hold your capability.
• Work out tool life and change time, not just seconds saved.
• Run a capability check before and after any significant change. Passing parts can hide a lost margin.
• A faster process is a changed process, so get it approved.