[shaju]

My bose bought a Doosa Lynx 220LM lathe. I had a crash on the machine last week. After boring I didnt programme to move the turret to a safe position and it did the tool change with out retracting. All tools in the turret were set by the Q-setter and my job zero was at the face of the stock. Can any one help me to fool proof such incidents in the future.

Shaju

[Metalcutter]

I really don't know what CAM software has to do with paying attention to what you are doing. But you could set up a macro that is called out by a single G code that would act like a safe tool change block by moving the tool out to the front of the part then up in X. But there will always be limitations. Wether you program at the machine or remotely via a CAM package there is no substitute for paying attention to what you are doing. Your safety depends on it! Complacency is the enemy in a machine shop.

[Paulo E.]

LOL no disrespect to mmmilligan but if tha's your sales pitch for a cam software... you just lost me as a customer. I've seen cheesy ways to sell a software but to just suggest a software with out any explanation and say here this will solve all your problems is an insult. As MetalCutter suggested you just have to pay attention. I would say the first step is to make sure your cam software is posting the right code, it would be nice to have a macro but somehow I doubt if he knows how to do one. As for the crash Shaju, I have good news and bad news. The odds of you crashing a machine is high if you work in a machine shop. it just happens to the best and to the worst of us. The only way that I know of never crashing a machine is not working in a machine shop.

Just keep your eyes open, the rapid 5% and your finger on the E-Stop.

[Jaguar]

Single block and Distance to go are your friend.

J

[g-codeguy]

Start and end your programs with Safe Index subprograms. I use the Hardinge ones on all our Fanuc controlled lathes including our Daewoo Lynx lathes. I can give you the subprograms if you'd like them.

EDIT: If you are using a software program to develop your code, you should be able to hard-code the software so that the subprograms will be called with every operation. I did in Mastercam. I usually have a boring program in each control. Naturally these subprograms are also imbeded in my boring programs. I have mine set up to be called by an M-code. M91 thru M94 to be exact. (M91/M92 front turret, M93/M94 rear turret).

[Metalcutter]

g-codeguy:
I'd like to see these. Our Toshiba TUE-20 uses a B0 which gets the ram to the tool change position. We use SmartCAM and our code generators do pretty good clearing the tools before indexing. Either way, you still need to get the tool out from inside the part. It's just a good habit to practice that, be it a lathe or a mill.

[stucaruk]

Look at it this way. Everybody makes mistakes.
Failure to program the tool to clear the bore and move to a safe distance BEFORE the tool change was the issue and the root cause.

The second was failure to single block through the program and not notice the impending tool change with the tool buried in the bore.

I'll bet you won't make that mistake again.

Even a CAM system won't save you, since it was a procedural mistake. The best Cam program should still have you single block through the program the first time or for the first part after a new setup. That's the safest bet.

[g-codeguy]

g-codeguy:
I'd like to see these. Our Toshiba TUE-20 uses a B0 which gets the ram to the tool change position. We use SmartCAM and our code generators do pretty good clearing the tools before indexing. Either way, you still need to get the tool out from inside the part. It's just a good habit to practice that, be it a lathe or a mill.

These are for lathes. The G28V0 makes sure the subspindle is home. Z4. in O999 sub is modified by set-up person to be at least an inch more than the longest tool. I could set it up as a variable, but by the time I learned anything about variables everyone was use to making the changes themselves. I put the subs in protected numbers called by an M-code. M91 calls P9001, M92 calls P9002.

All I need to do is make sure the tool is clear in X-axis and call up M92. First thing the tool does is rapid to .5 in front of the part before going to my index position. It scares some people when they don't see a clearance move in the program until they learn how it works. I have two others for subspindle work.

I don't see why they couldn't be modified for a mill.



:9001 (MAIN SAFE START)
G28V0
G0G40G97G99M42
M98P999
M99

:9002 (MAIN SAFE END)
G0G97Z.5
G40
M98P999
M99

:999 (MAIN SAFE INDEX)
T0
X4.Z4.
M99

EDIT: M42 is for exact stop (no corner rounding). Rest should be common to most any lathe.

[Daewoosan]

I like to use the second reference point for tool changes. You must set this up in system parameter 1241 before using. There may be currently zeros there, so please don't call the G30 U0.W0. until you place numbers in 1241, because if you don't, that will send the face of the turret straight through the chuck to the face of the spindle nose flange. Not good. With all of that said, I make the X axis the same as it is in parameter 1240. As far as the Z axis, pick a place you would like your turret index to take place, multiply the z axis machine number by 25400 (if you are running in inch) and place that number in the Z axis of system parameter 1241. You will then command G30 U0.W0. before every turret index, and wallah no crashes (at least not yet). The position light indicators will flash when you are at the second reference point, and are solid when you are at home (the G28 u0.w0. position).

[shaju]

One of my friend who use to work on mazak lathes told me that his machine realises thye length of the longest tool in the turret and retracts it from the work zero before tool change. he thinks that it is a parameter setting. Could any one come up with similar safety setting in Doosa lathes?

[g-codeguy]

One of my friend who use to work on mazak lathes told me that his machine realises thye length of the longest tool in the turret and retracts it from the work zero before tool change. he thinks that it is a parameter setting. Could any one come up with similar safety setting in Doosa lathes?

I could be off base as I have zero experience with Mazak lathes....but...

I doubt it "realizes" what the longest tool length is and then retracts accordingly to a safe index point. More likely it uses a macro program that reads the tool geometry for each station, compares them for the longest tool, and then adds a set amount to that as a safe index position.

I don't see why something similar couldn't be done with the Doosan as long as it has Macro B type capability.

You would still have to remember to call this program up at the end of an operation, tho.