After a CNC Tool Break: Containment, Restarts, and Safe Program Edits

Sooner or later a tool breaks, a part comes out wrong, or the machine hits something. What you do in the next ten minutes decides how much it costs. Restart too fast and you crash a second tool, or send out parts with a missing feature. Handle it well and you lose one tool and a part or two. This is the mid-level skill: stop safely, find out why, work out which parts are in doubt, get the machine going again from a safe point, and change the program only through a controlled process.

What You Will Be Able to Do

• Stop the machine the right way and capture what happened before it is lost.
• Read a broken tool to find the likely cause.
• Work out which parts are suspect, including parts missing a feature.
• Check a machine after a crash and know what needs maintenance.
• Restart mid-program from a safe block.
• Make a program edit that is controlled, proven and recorded.

The First Minute

If something sounds wrong, or you see a tool break, press feed hold. Use the emergency stop if a person or the machine is in danger. Feed hold keeps the position and the program state, which helps you recover. An E-stop drops everything at once, so the tool can stay buried in the part with the spindle stopped.

Before you touch anything, write this down:

1. The program number, the block number, and the active tool.
2. The alarm text, word for word.
3. The part count.
4. The load meter reading, if you saw it.
5. What you heard or saw just before it happened.

Clearing the alarm or resetting the control can erase some of this. A photo of the screen with your phone, if your shop allows phones on the floor, takes five seconds.

Warning: A stopped axis is not a safe machine. Wait for the spindle to stop fully before you open the door. Reaching in to clear a broken tool or a jammed part may count as servicing, not normal operation. OSHA's lockout rule has a narrow exception for minor tool changes that are routine, repetitive and integral to production, and only with effective protection in place. A crash cleanup may not fit it. Follow your site's procedure, and if it calls for lockout, an authorized person locks the machine out first.

Reading the Broken Tool

Do not throw the broken tool away. It is evidence.

Look at the part as well. A smear of tool material in the cut, a hard spot, or chips jammed in a pocket all help explain the break.

One question matters most: was this normal tool life, or did something change? A tool that broke at its usual part count needs a tool-life change. A tool that broke at a third of its usual life points to a bad batch of stock, a wrong offset, a coolant line that stopped, or a chip problem.

Containment: The Part in the Machine

Treat the part that was in the cut as nonconforming until someone decides otherwise. Tag it. A tool that dragged across a surface, or a broken drill left in a hole, is not something you fix quietly. Removing a broken tap and carrying on is rework, and rework needs approval.

Containment: The Parts Before It

This is the step people skip. The tool did not always fail at the moment you noticed it.

Worked example. You run a batch of brackets. Inspection runs every 20 parts. Part 140 passed. At part 153 you hear a change in the sound and find a broken 1/4 drill. The drill runs before a tap in the same program.

1. Parts 141 to 152 were not checked. You do not know when the drill's cutting edges started to fail. That is 12 parts in doubt.
2. Part 153 is tagged, since it was in the cut when you stopped.
3. If the drill broke earlier than you noticed, the holes in some parts may be shallow or missing, and the tap that follows would have hit solid metal. So you check the tap as well.
4. Thirteen parts get checked for hole depth, hole size and thread. If 148 through 153 fail, you have found where it started.

Think about the features the broken tool cut, and then the tools that came after it. A missing drilled hole can break the next tap. A missing chamfer may pass every size check and still fail at assembly. Parts with a missing feature are the worst kind of escape, because a size check on the other features finds nothing.

If any suspect parts have left your station, tell your lead right away. They may be at the next operation, in a tote, or at shipping.

After a Crash

A crash is any time the tool, holder or spindle hits something it should not. Report every crash, even a small one. Hidden damage shows up later as bad parts, and your lead needs to know where to look.

Work from the part outward:

Do the checks your role allows. Spindle runout limits come from the machine builder. Geometry checks, a spindle rebuild and ball screw work belong to maintenance or the builder's service person. Reseating a holder is fine. Taking guards off to see what moved is not, unless that is your job and the machine is locked out.

A rule worth keeping: if you hit it hard enough to be scared, have it checked before you run production.

Restarting Mid-Program

Most machines let you start from a chosen block. That does not mean every block is a safe place to start. The control's state comes from the lines above, and many of those lines are modal, so they stay active until changed.

N300 T4 M06 (1/2 END MILL)
N310 G90 G54 G00 X1.5 Y-0.75 S4200 M03
N320 G43 H04 Z1.0 M08
N330 G01 Z-0.25 F12.0
N340 X4.0
N350 Y1.5

Say the tool broke at N340. If you start at N340 after loading a new tool, here is what the control does not know:

• The spindle is not on. N310 never ran.
• No G43 is active, so tool length is not applied. The tool can drive to a Z that is off by its full length.
• Coolant is not on.
• Work offset, absolute mode and feed may be left over from something else.

Start at N300 instead. That line and the two after it rebuild the full state for this tool. A well-written program has one of these safe blocks at every tool change, and they exist for this reason.

The restart procedure:

1. Fix the cause of the break first. Otherwise you will break the next one.
2. Load the new tool and set its length and diameter. A new tool is not the same length as the old one.
3. Clear the damaged part, or get approval to keep it.
4. Find the last tool-change block before the point of failure.
5. Read every line from there to the failure point, and look for modal codes that a jump will skip.
6. Use your shop's restart function, or move the cursor to that block.
7. Turn on single block, drop rapid override, and set feed override low.
8. Watch distance-to-go on each approach.
9. Expect the tool to cut air where the old one already cut. That costs a little time and is the safe way to do it.

Some controls have a program restart function that scans the code and rebuilds the state. It helps, but check the screen before you press cycle start. Some shops do not allow restart in the middle of a tool at all, and they rerun the whole tool or scrap the part. Follow your shop's rule.

Safe Program Edits

A program is a controlled document, the same as a print. A quiet change at the machine can lose a revision, break the next job or put parts out of agreement with the first article that approved them.

Sort every change into one of these, and follow your shop's rules on who can do what.

Override is not always the answer. If the job only runs well at 60 percent feed, tell the programmer, so the program can be fixed for everyone.

How to Make an Edit

1. Get permission first. Know who owns the program.
2. Work on a copy. Save the proven version, or confirm it is safe in the master file.
3. Change one thing. If you change three things and it breaks, you will not know which one did it.
4. Think about what is modal. A change on one line can affect every line after it.
5. Add a comment. Include the date and your initials, such as (2/14 JR R0.1 TO R0.2 CLAMP CLEARANCE).
6. Prove it. Run the changed section in single block at low feed.
7. Update the master. If the shop sends programs from a server, your edit lives only on the machine, and the next download wipes it out.
8. Tell people. Note it on the setup sheet, and ask quality if the change needs a new first article.

Worked example. Tool 3 peck drills over a clamp, and a chip is catching at N80. You want to change G99 to G98, so the drill returns to the start height between holes.

N70 G99 G83 Z-0.75 Q0.2 R0.1 F6.0
N80 X3.0

The change is one word, and it adds a little time to each hole. But check the rest of the cycle. G98 and G99 are modal, so every hole in this block now retracts higher. That is what you want. Confirm that the start height is above the clamp. Then run it in single block, add the comment, update the master and write down the reason.

Typing Mistakes the Control Will Accept

A control checks syntax. It does not check whether a number makes sense.

• Missing decimal point. On many Fanuc-style controls in inch mode, X5 means 0.0005 inch, not 5 inches. Z-1 means 0.0001 deep. The tool goes to the wrong place and the control does not alarm.
• Wrong sign. Z0.25 instead of Z-0.25 cuts air, which is the lucky direction. Reversed, it cuts deep.
• Letter O for zero. G0O can be read as a different word, or it can alarm.
• Editing the wrong block. Two lines that look alike can sit far apart in a long program. Search by the N number, then reread the line.

Common Mistakes

Check Your Understanding

1. A drill breaks on the first peck of a new job, in a program that ran fine last month. The tool was new. Where do you look first?

At something that changed in the setup: the tool length, the H number, the work offset or the material. A new tool on a proven program points away from tool wear.

2. You check every 30 parts. Part 90 passed. A tap breaks at part 112, and you find the drill before it has chipped corners. What is suspect?

Parts 91 through 112, so 22 parts, checked for hole size and thread, because the worn drill may have cut undersize holes before the tap broke. Part 112 is tagged.

3. Why is N340 a bad restart point in a program where the tool change is at N300?

The spindle start, the tool length compensation and the coolant all happen above it. Starting at N340 skips them, and the tool can move with no length applied. Restart at the tool-change block.

4. A small crash bends a holder. You replace it, and the tool runs fine. Does anything else need checking?

Yes. Recheck the workholding and work offset, because they may have shifted, and report the crash so spindle runout can be checked. A clean sound does not prove there was no damage.

5. You corrected a program at the control and the job runs better. On the next shift, the old problem comes back. What probably happened?

The program was downloaded again from the server, and that wiped out the edit. A change has to go into the master file, with a record of what changed.

Key Takeaways

• Stop with feed hold unless someone is in danger, and capture what happened before you reset.
• The broken tool is evidence. Find out why before you run again.
• Contain back to the last good check, and think about every tool that came after the failed one.
• Report every crash, and check from the part outward. Spindle and geometry work belongs to the right people.
• Restart from a tool-change block, with a re-measured tool, in single block.
• A program is a controlled document. Get approval, change one thing, prove it, and update the master.