Problem- Crashed 4th axis on a 5025 VMC

[Cncjunkie]

I have a 5025 Daewoo with a SMW 4th axis. The problem is, it has been crashed and destroyed the 4th axis. I am getting ready to replace the 4th axis. But I fear that it is going to happen again. I know that if a height offset is set incorrectly a crash will happen and if the program is started in an incorrect place a crash can happen. I was going to restrict the machine travel but we are doing work thru the fixture plate. I also thought about setting a default height for the tool at the beginning of the program and having it check the default against the offset that was entered into the machine.
Any ideas on how to keep a crash from happening?

[WOLOG]

Does this happen often? Does anyone believe in running the first part in 5% rapid? Please explain a little more on your setup.

[PBMW]

I don't get it either....
I been running nad programming 4 and 5 ax machines since 1982. I've crashed machines. Everybody has. But i've never crashed a 4x. If you have your work offsets correct, there ain't no way.
I set tools from the table. I know people that program from C of Rot. I don't like it cause I can't adjust it. But to each their own. I set up Work offsets for each face. Never had a problem

[Cncjunkie]

Well that is also the problem, this is the second time. The first time the operator was changing something in the program and didn’t pick up the tool height offset. (Which needed to be changed in the tool geometry and not the program but..) This last time I don’t know what happen. The machine had an error, incomplete home return. Before the crash happen, and it crashed into the table in z. The programs have been proven and setups are simple. Its a plate that is ball locked down to the main 4th axis fixture and the 4th axis, tail stock and main 4th axis fixture between the 2 are never removed . a few tools have to be switched out of the machine and tool height offset entered and some geometries. All geometries are on a sheet that is posted by the machine and are updated from the last run. We use a presetter for the tool height offsets. Also we use dedicated tooling 99.9% of the parts run on the machine. Short of holding the operators hand I’m at a lost on how too keep another fatal crash from happening. If it was u guys what would you be looking at?

[lshingleton]

The first crash was by someone touching a program -Turn on 3202 and set Ne9 to one in the parameters------Change your program to (O9100--etc)this limts access to you -and if some unlocks this dicipline them
The second one is write a macro progam that checks the tool height and limits the amount of offsett devatation that can be done
The other more serious crash caused by incomplete ref-thats a hard one---make sure at least somewhere at the start of the program the machine is referenced in the control-
G00G91G28Z0
G00G91G28X0.Y0.A0.C0
G90
()

[Cncjunkie]

Thanks, On the incomplete ref. I have it ref via the control after every tool. Its hard so say what really happened. I was gone for a week and returned to this mess.
On the macro, I thought about setting 30 variables in the program (1 for each tool) at the beginning when I set the workoffsets. and then having it check that hard number against the number entered into the tool height offset via the macro. Is this the way u would do the macro ?
Also 3202, Will u need to shut the control down for it to take effect?

[Cncjunkie]

The operator that crashed the machine with the incomplete ref. to home, He said it was running and etc.... Do you know of this ever happening? I tried to reproduce the error. Any ways that you know that I could? So I might see a better way to prevent it?

[lshingleton]

Yes i have saw that before on older machines-because they relied on the switches to register home--acually if your having that problem ref the machine in manual only and change your program to g30 instead-then it goes to a set position every time and doesnt keep reseting from the switches-cuts down the risk-----to one time you power the machine on compared to everytime you go home-and the first part after startup run slowly---------the 3202 parameter just need to go to mdi and turn on pwe and this will let you change it
()
tool life -check the fanuc manual for you machine address but this is hoem the tool length check is done

O6666(setup a sub proram at the start of the main tool geo check)

IF #2001[Le 100]goto n9999-----------
IF #2001[Ge 102]goto n9999--------

N9999#3001[tool length incorrect]


the macro number 2001 is an example which can be found in the fanuc book for the address related to the h1 value for your tool-you are just putting a value in like i have used of 100 which is you tool length limit----
if i find a machine example i will post for you

[Cncjunkie]

ok cool, thank you very much for your help man.

[Cncjunkie]

On the incomplete ref. Is there a parameter setting that will not let the machine run if that error has happen?

[lshingleton]

Is the 4th axis an add on for this machine --like a fanuc or hass table?
Daewoo's are set up to not preform any action until ref completed and also the ref speed in rapid can be slowed in the keep relays

[HuFlungDung]

One precaution a person might take, is to program an XY positioning movement to a safe spot, like to the X0Y0 of the current work offset, but with Z still fully up. The reason I suggest this, is that sometimes, I have noted that a crash could occur on some of my programs if I start from the machine home position, such as would be the case every morning.

It is easy to overlook this when one is busy setting up a new program after the machine has already been running that day, and the table may be conveniently parked at the work unload position.

However, after a cold startup, a long tool may actually be found moving to the first programmed XYZ position from behind the indexer. If the XY move is longer than the Z, and all 3 axis move on rapid, then the Z may reach its lower endpoint before X and Y are completed. This puts it in the danger zone and could crash into the indexer.

I also have a habit from the old days, wherein I take care to set my tool length offsets always to some height above the rapid clearance plane of the part. This ensures that my length offsets are always negative, and if I accidentally edit the length offset to a positive value, then the tool moves safely up, rather than down.