When inserts break ?

So, I'm kinda used to what to do on the CNC mill, but on a cnc lathe if you're part way through roughing or parting off and the insert/tools calls it quits and starts chewing things, is E-stop the only option or what do you do? This is probably what worries me the most about this turning thing, walking away for a few minutes and next thing I know big mess... I pretty much only do stainless of various flavors, a lot of it gets parted off, so not much give there, so just want to be sure of best way to recover from that?
Gonna change tips more often than I would on manual lathes just in case. Also maybe change the roughing procedure to only take a few cuts, M0, take a look, an continue on if its a part with many cuts to get down to dia?

Really wishing I could have gotten this CNC learning and screw ups out of the way on someone else's machines back when I had a day job, however short that might have been...

Can you monitor torque? Perhaps more difficult on a lathe than a mill, but if you can model the loads during normal cutting, then set an alarm when you go higher (as in holder trying to push it's way through stock), this might be an easy, if not optimal solution.

If you have the space, multiple roughing tools set to work for a "known good" number of cycles, then swap? Inspect used inserts, change as needed.

Do you have a good microscope? Might help with coming up with cut time and load parameters for inserts where you correlate edge wear and loss of coating to materials, cutting time, and conditions.

SND said:

So, I'm kinda used to what to do on the CNC mill, but on a cnc lathe if you're part way through roughing or parting off and the insert/tools calls it quits and starts chewing things, is E-stop the only option or what do you do?

Click to expand...

Feed hold. It's generally not a problem tho. Swap the edge before they get so dull that breakage is an issue.

I'm used to backing out with the differential resolver but you most likely don't have those

SND said:

So, I'm kinda used to what to do on the CNC mill, but on a cnc lathe if you're part way through roughing or parting off and the insert/tools calls it quits and starts chewing things, is E-stop the only option or what do you do? This is probably what worries me the most about this turning thing, walking away for a few minutes and next thing I know big mess... I pretty much only do stainless of various flavors, a lot of it gets parted off, so not much give there, so just want to be sure of best way to recover from that?
Gonna change tips more often than I would on manual lathes just in case. Also maybe change the roughing procedure to only take a few cuts, M0, take a look, an continue on if its a part with many cuts to get down to dia?

Really wishing I could have gotten this CNC learning and screw ups out of the way on someone else's machines back when I had a day job, however short that might have been...

Click to expand...

.
1) usually tool life is used to eliminate using dull tools. at the end of a certain time you replace tool or at least look at it and judge whether to add time
.
2) feeds and speeds and depth and width of cut are used that give reliable usage without sudden tool failures. taking too much first sign is getting a random 2% sudden tool failure rate
.
3) width and depth of cut. often the harder the material the less depth and width of cut is taken to stop loosing insert corners breaking off. parting on a lathe its common on high depths to go part way back up shift over .005 and cut to previous depth this opening the sides is used to relieve the side rubbing trying to part large diameters. if tool .125 than the part ends up .130 or .135 wide. its just one way to relieve pressure on cutting tool
.
4) some materials have hard spots or slag inclusion in metal usually got to stop feed within seconds and even when tool replaced you can easily dull a 2nd or 3rd tool til past the hard spot. depends very much on quality of metal. small hard spots you go right past and might not even notice them. obviously feed hold will stop the feed and can start again and feed hold again if noise just as bad. if too much material at that spot often have to slow rpm and feed cause its just too much for the cutter. extra cuts often called what if big cuts are used if part is bigger than expected. often cuts air on 1st pass rather than if piece big have a sudden tool failure overloading tool. obviously if harder metal a tool that can take .200 passes with soft alloy might be limited to .100 or less passes on a harder alloy
.
5) tool length or stick out of tool holder amount. when you double length of a tool sticking out 2x it is 1/2x1/2x1/2= 1/8 less rigid. often a sudden tool failure is caused by a tool setup sticking out too much

I know a decent bit about tool life... just not so much about how deal with the cnc when I screw something up or tool decides to quit prematurely, right buttons to push in what order type deal...
Nice thing about manual lathes is the clutch or feed lever usually kicks out eventually...

What do you do after Feed Hold to stop the spindle and safely get yourself back out of the cut?
These knobs/buttons aren't like what I got on the mill, I can feed hold that one and just turn knob to handle and spindle stops, no knob like that on here. Maybe feed hold, jog button, spindle stop button? than carefully move out of the cut?

So what's the actual machine you're running? Have the operation manual? Is there a program you can keep in MDI that would give you a safe retract?

I occasionally run a Haas TL-1, and I get a machinery version of "uncanny valley" with the panel, as it's almost what I'm used to, but not quite...

The RESET button is your friend. It stops all machine movement, including the spindle.

Remember on a Fanuc, when you reset in the middle of the program, the program pointer will still be at the line where the machine was at when reset.

You have to go into Edit mode, then the Program page, to set your program pointer to where you want it.

Milland said:

So what's the actual machine you're running? Have the operation manual? Is there a program you can keep in MDI that would give you a safe retract?

I occasionally run a Haas TL-1, and I get a machinery version of "uncanny valley" with the panel, as it's almost what I'm used to, but not quite...

Click to expand...

It all depends on the machine as said above. On my Takisawa TC-1 I have 3 options, MDI, the jog buttons, or the hand wheel. As for when to change inserts I use my ears and the tachometer that shows RPMs. All the lathes I ran have showed actual RPMs, not all have had load meters. It is best to change inserts right before failure especially with parting tools. On most jobs the inserts fail at the same rate every time. I have a note pad handy and keep track of when I last changed an insert.

SND said:

So, I'm kinda used to what to do on the CNC mill, but on a cnc lathe if you're part way through roughing or parting off and the insert/tools calls it quits and starts chewing things, is E-stop the only option or what do you do?

Click to expand...

You do the same thing you do on the mill. Feed hold, reset, dial the tool away and roll the insert.

Make sure there is no carbide buried in the part, then re-run the tool. Use the feedrate override to ease past the chewed up spot, then go back to what you were doing...

Turning inserts are/should be pretty tough, if you are using little thin crappy inserts, you are going to need to stand by the Machine and attend it. OTOH if you are using a CNMG 432 you are going to lose corners as a wear item, not a breakage item. So it isn't total Tool failure, it's wear, and wear isn't a catastrophe, that's why people use Roughing and Finishing Tools. There are Operations that I attend.<that is a Period. Indexable Drills, Bottom of a tight bore, Cross Drilling, Deep hole.---Part off.

It's really just like any other Machine operations, you will learn to listen to the Machine, you will hear when the Spindle starts to whine a little-because you need to, simple as that. You'll learn to listen to Tool changes, and approaches. You'll wait to hear the Tool start the cut, and finish a pass. Wind up and down with CSS, your ears will get keen. I use a Microscope regularly to inspect Inserts and the wear patterns, get comfortable with what is happening and why. It takes time and there isn't really a magic answer.

As far as E-stop goes, I only use it when it might actually be an Emergency. Reset is the same thing.

Indexable Drilling, and Part off are the most catastrophic failure items. So be there, M0 if you need to. Part off is the bane of my existence, I don't do it as much as others. BUT if I need to, I DO NOT use crappy part off blades, the ones Sandvick gives you when you buy 10 Inserts. (complete marketing BS) I use Deep Groove, Grooving tools. Positive locking Tools with a clamp screw, not a wedge thingy with a stupid ass wedge thingy Tool. I really hate them.

And Indexable Drilling (my favorite thing BTW). Problem is, you have nanoseconds to get that one shut down before your part and Tool are dead-dead. So I attend that one, and some may say "but you are wasting time needing to go over there and watch it". Maybe, or maybe not, I can conservatively Drill a 1" hole in 304, 3" deep in 1 minute--So STFU!!! Drill bodies are too expensive to not watch them run. Plus that's 304, watching a 2" Drill go 6" deep in 2 minutes with Cold roll is just fun.

R

If I see or hear something going awry, say, while turning and OD I will feed hold, then jog the tool out of the way with the spindle still turning just in case it needs to cut a smidge of mtl off while clearing, then reset button to stop the spindle...on my Fanuc-controlled lathes you have to HOLD the reset button for a few seconds before it will stop the spindle.

Some controls have load monitoring and I like it to at least protect against catastrophic failures. Keeping track of tool life on repeat jobs is a good way to set ballpark tool life, too, if your machine has a tool life counter or you can write a macro to keep count. Good luck!

Nerdlinger said:

Keeping track of tool life on repeat jobs is a good way to set ballpark tool life, too, if your machine has a tool life counter or you can write a macro to keep count. Good luck!

Click to expand...

I have found inconsistencies with materials has defeated that for me many times. I need to start asking for certs at all times. Sometimes tools that kicked butt on a job last time (I will write down the exact insert number) don't work worth a damn.