[cbrannam]

Hi,

I just landed a new job as shop manager at a machine shop here in the town I live. We have a couple of Okuma cnc lathes. One is a LB15 and the other is a caption (2010 year).
On the LB15 how to I check x axis position of the tools. The program says it is at X but the tool is off about .300” from the center. I have touched off each tool and changed it in the Parameter page but when we do a dry run on the program the #4 center drill is off.
My owner(does not know anything about the machines or how to run them) told me I wants me to indicate in the location of where the center drill is at.
How do I do that?
Would I chuck up a co-axis indicator and find the center of the tool holder?
I think all I have to do is change the position of X but how do I know that im in the right stop?
The part that is being turned down is 1 1/8” diameter and about 1 7/8” long.
Tools that I’m using is a
#4 center drill
Spade drill
Threader
Face off bit

Thanks
Chris

[txcncman]

Wow! Shop manager you say? Tough position. I am guessing none of the machinists working there know anything. Right? Have you set up a manual lathe before? Indicating is the best way to align the center of the spindle with the center of the tool. Do you know which offset to change? Do you know how to change it? Do you have all the manuals there? Have you read through them? Are all of the turret locations off zero position?

Normally on a lathe when using a center cutting tool (i.e. drill) the X offset for that tool should read 0.0000. Does yours read 0.0000. If not, what happens to the tool position when you set it to 0.0000?

[broby]

Sounds like you need someone with at least basic knowledge of setting CNC machines to come in and give you guys a training session.
See if there is an Okuma rep in your area that could come in and help.
This will save you bucket loads of time/grief/crashes and loads upon loads of frustration as you come to grips with this machine.
Once you have the basics, then it is a matter of time to learn the small details.
In order to try and teach you everything via this forum would be damn tough (from both sides of the screen!).
Good luck.

[littlerob]

I agree with Broby, but just for kicks and giggles, go to MDI, enter T**** G0 G90 X0 -press cycle start, now jog that tool to the face of the part, go to tool data page make sure the X offset is 0 for that tool, you should be able to see if it on center without an indicator, but use it if needed (the way you described co-ax). If it is not on center then the machine is mechanically at fault, and you are back to calling Okuma to come in.

EDIT; I meant along the Y axis only for calling in a tech, you can realign the turret yourself IF it's out, but that woudl be a different thread.

[cbrannam]

yes all of the guys that knew what to do walked out. now im stuck with a new group of people that dont know much about anything but they are cheap labor.

and i will get the offset today while at work and reply with that info.

[mfgbydesign]

To put the drill on spindle centerline you will need only an indicator on a magnetic base.
Mount the indicator on the chuck.
Jog the tool close to center and close to the face of the chuck.
Place the stylus of the indicator on the shank of the drill along the X axis.
Rotate the chuck 1/2 a turn by hand (you might need to MDI M5 on an Okuma to take off the brake). This is "tram."
Observe the Total Indicator Reading (TIR). Move the X hafl the distance and tram again until you get the same reading on both sides.
Tram perpendicular to X to verify the drill is on center in all directions.
When it's on center look at the absolute position in X and place that number in the Geometry offset for that tool.

[underthetire]

To put the drill on spindle centerline you will need only an indicator on a magnetic base.
Mount the indicator on the chuck.
Jog the tool close to center and close to the face of the chuck.
Place the stylus of the indicator on the shank of the drill along the X axis.
Rotate the chuck 1/2 a turn by hand (you might need to MDI M5 on an Okuma to take off the brake). This is "tram."
Observe the Total Indicator Reading (TIR). Move the X hafl the distance and tram again until you get the same reading on both sides.
Tram perpendicular to X to verify the drill is on center in all directions.
When it's on center look at the absolute position in X and place that number in the Geometry offset for that tool.

Mostly correct. LB15 has no brake, so no issue there. Second, after you sweep in a boring bar holder, you use the zero set function on an Okuma and calculate X zero. Now all BB holders will be at 0 on the position page at center line. Then you offset the tools, and generally, all turning tools will have a + offset, all boring bars will have a - offset, and all drilling tools will have a 0 offset in X.

[txcncman]

To put the drill on spindle centerline you will need only an indicator on a magnetic base.
Mount the indicator on the chuck.
Jog the tool close to center and close to the face of the chuck.
Place the stylus of the indicator on the shank of the drill along the X axis.
Rotate the chuck 1/2 a turn by hand (you might need to MDI M5 on an Okuma to take off the brake). This is "tram."
Observe the Total Indicator Reading (TIR). Move the X hafl the distance and tram again until you get the same reading on both sides.
Tram perpendicular to X to verify the drill is on center in all directions.
When it's on center look at the absolute position in X and place that number in the Geometry offset for that tool.

What do you do if the Y axis is out of alignment?

[underthetire]

Call in a service guy. The machines been crashed and needs a turret alignment. You can offset the BB holders on Y by a few thousanths if need be. The LB15 has an eccentric pin that locates the blocks on the turret. Loosen the bolt and rotate till you get one holder in. Then with a mag base and indicator, move the turret back, index and come back to the indicator. Loosen the next one and turn it till it matches the one you set up and continue to the next one etc..
Done 100 alignments on those things back in the day....

[txcncman]

Good answer!

[cbrannam]

ok i have indicated in the #5 center drill. it is out .006.

now what do i need to do?

also the program is calling for a spade bit insert to drill a hole that is 21/32 dia. do i need to check to see if that is indicating the same?

[underthetire]

.006 in what direction, x or y (height).

[txcncman]

0.006 TIR? that is only 0.003 off center. Not really too bad. Within 0.001 would be better. If it were my machine, I would run it like that and see the results. If the results were acceptable, I would not make further adjustment.

[littlerob]

I agree, but if you're planning on running smaller parts, might as well deal with it now. Anything under .25 is going to piss you off. Might as well get it dialed in, later you can say to yourself "I know it's not that".

Search this sub-forum for "turret alignment", it's all there.

[cbrannam]

ok problem fixed. new bit and problem went away.

now is there anyone that can write me a program to do a warm up cycle?

[txcncman]

Not me. But i can try to tell you how. Part of the learning process. The safest is to actually have a program that reads some of the system variables. But I do not think you are ready for that yet.

So, you will need G-code that will turn the spindle on. Index the turret. And move the axis around a little for a period of time.

Okumas are pretty good about power up in a safe mode. Any G8X codes should be canceled. But to make sure, put a G80 in. G90 is for absolute positioning, which should be the default start up. But again, to be sure, put in G90 so you will know. G20 for inch input. G40 cancels cutter compensation. G97 put the spindle in constant RPM mode. The chuck will have to be in its operating position, either opened or closed. Then you will need to send the turret to a safe position. Nice thing about Okumas is you can toss some wild numbers in here since they basically won't over travel. So a G0 for rapid. X30. Z30. should be enough to get you to a safe point. M3 will turn the spindle on clockwise. Start with a low RPM, say S200. Then do a tool change to some tool you want, like T0200. Put a dwell in, say G4 X10. Then switch to incremental mode with G91. Then switch to feed rate with G1. Then tell the Z axis to move some distance that will still be a safe distance away from the spindle. Maybe Z-10. Put in a feed rate of say F0.1. Then do the same for the X axis with X-10. Then maybe put in another dwell with G4 X5. Then move the turret back to where you started with X10. on one line and Z10. on the next. Then you can stop the spindle with M5. Then restart it in the opposite direction with M4 and maybe a faster RPM like S400. Then index the turret to another tool, like T0400. Then repeat your X and Z moves with maybe a slower feed rate since you spindle will be going faster with F0.04. Keep repeating this until you get tired of writing G-code or until you feel you have run the machine long enough to be warmed up. At the end, be sure to send the turret back to a safe position and end with an M30, which resets the program and machine ready to run again.

[fordav11]

I never do a warm up. real men just put the next piece of material in the chuck and press start
if it can't handle that we'll burn it and buy something that can

Getting back to the original post(s), you really should hire someone that knows his sh*t.
If you crash the machine it'll cost you a WHOLE LOT more than his wages to repair it.
Just like you wouldn't attempt to repair the electronics in the back of the machine, leave the technical stuff to those that are qualified. You'll have peace of mind knowing the job is being done right and you'll have production & profit which I'm guessing is the main reason you were employed......

I don't know the exact spec and the full stroke limits on your machine but you can make it do anything as a warm-up and almost everyone will have a different idea about how it is done and what you should do. if it has OSP5000/7000 (according to google) then you could do something simple to just move the turret around while the spindle is turning at various RPMs and throw in a few tool changes. depending on the machine spec you can exercise other axis as well. Remember to clamp the chuck or it won't spin. Or you can add a chuck clamp M-code or the M-code to cancel chuck open interlocks. It's easier to just put a ring in the chuck and clamp it or follow my first suggestion if you're a real man

$WARM-UP.MIN%
(WARM-UP LB15 MACHINE)
( )
G0 X30 Z30
G0 T0101
G97 S200 M3
G01 X6 Z6 F0.5
S400
X30 Z30
T0100
G0 T0505
G01 X6 Z6 F0.5
X30 Z30
G96 S300
G01 X6 Z6
X30 Z30
T0500 M5
M1
( )
M02

[Algirdas]

sometimes machine doesn't needs a warm up

[fordav11]

Unless I need a precision hole I never bother jerking around clocking center of turret and chuck when setting drills. especially on my machine because it's seen better days due to being butchered by previous owners. depending on the condition of the machine the turret will likely not be dead on center anyway so the drill be will off center (high or low), especially if the machine is old.

turn the material and measure it. lets say it's 2.0"
bring the side of the drill to touch the diameter of the material.
lets say the drill is 0.5" diameter. go to tool offset page, cursor to the tool you want to set in 'X' and press CAL then type 2.5 and press WRITE
for X setting of drills that is all that's required.