LB-15 w/OSP 5000L-G

Hi All,

We have purchased a 1990 LB-15 with a OSP 5000L-G controller.

We are trying to write a small program by hand (not using IGF) We seem to no luck with this. Could anyone explain what screen we need to enter this program and could you supply us with a simple program that would open the chuck and close it, turn on spindle move x then move z, change turret.

I do have 5 original books that came with the machine buy we can't seem to locate a page that explains how to enter a program manually.

We do have extensive experience with programing our Fadal milling machines. Both manually writing as well as using Virtual Gibbs.

Any guidances would be very appreciated.

Thanks,
George

Press Edit/Aux mode key, a new set of softkeys come up on the screen. Press Edit softkey, enter new program name then press [Write]. If you try to edit a program that does not exist, it creates a new one.

Hi

after you have written the new File, u have to go in "Automatik" Mode
and with F1 "Programm select" activate your Programm.

Thanks for the quick response guys,

We are up and running for now.

I'm sure i will have more question in the future.

George

Hello Dennis from Ansun .We wrote a simple program and got this error message. 465-3 alarm b plus var.limit x-axis 2.
The program looked like this.
m84
m83
m20 m24
g40
g50 s1000
t0101
m41 s120 t0202
m03(program runs to here)
g01 f50. z1.(error)
g01 x1.
g04f3.
m05
m02
Also if some one could explain the user parameters I would be grateful.Ours are set to this
+ vari limit(prog) x9.43 z14.004
- vari limit(prog) x-3.01 z-1.4596
+ vari limit(mach) x346.6906 z329.6164
- vari limit(mach) x334.2505 z313.7564

Thank you for the help.

change the line to:

g01 g90 g94 f50. z1.

You are probably in incremental mode and the X is at the + limit for the turret index. If you're in incremental it's trying to move past the limit, giving you the alarm. G90 is absolute mode so it'll make your program move to z1.0 work coordinate then x1.0 work coordinate. The G94 makes the f50. mean 50 inches per minute. Most often you'll use G95 for your actual cuts (inches per rev) so for an actual roughing pass it'd be

G01G90G95F.010Z1.0 (.010" feed per revolution of the spindle)

Two more G codes to look into for good looking finishes when facing your part are G96/G97 constant surface speed. You'll want to rapid/feed in G97 (CSS off) to your clearance point right above the part, then turn G96 on (CSS on) for the facing maneuver. This speeds the spindle up as your tool moves closer to the centerline of your part maintaining a constant cut. The only thing to remember is do NOT leave G96 on when moving in rapid to the turret index position, this keeps your spindle synchronized with the X position rapid move and the spindle accels/decels very hard to maintain the synchronized value and wears out the drive/motor.

For the USER limits (don't change the system stroke limits page, you'll hard overtravel the machine if you move these around a lot):
+ vari limit(prog) x9.43 z14.004 - this is the + limit of the X and Z axes that can be programmed in the machine. You can edit these to allow for a closer turret index program by program. Just find the closest point all tools clear the part and calculate these values. They are here just for that, minimize the work envelope to decrease cycle time. Between setups you can add to these to open them up to match the size of the travel. These initial values are calculated from your machine (system) limits combined with your zero offsets.
- vari limit(prog) x-3.01 z-1.4596 - this is the -limit of the X and Z axes that can be programmed in the machine. I usually set these up to a little before your longest tool would contact the chuck/jaws and modify if necessary. This side of the limits is more safety related to help prevent crashes.

+ vari limit(mach) x346.6906 z329.6164 - do not change these, these are your system limits based on no zero offset being included. They do not relate to a value the every-day operator will need to use, and can confuse issues if you try to use these. The only way I've seen these used to help in setups is to write down the limits off the System Parameters page and set the Vari limit (mach) values to match the System Parameters page. This maximizes your work envelope and allows you to re-set your user limits as preferred for the next part.
- vari limit(mach) x334.2505 z313.7564 - same as + vari limit (mach)

Thanks Okumaguy.I tried the g90 & g94 first thing this morning.Unfortunately it did not work,it gave me the same error message.The machine will run this program,but only if the moves are rapid and it will do it with or without the g90.

I finally got it to work.After M03 I Put in:
G0 Z4.
G0 X6.
G94G01F5.X5.5
G94G01F5.Z3.5
G0 X6Z4.
I am still confused as to why it would not feed from the limits.

I'm not sure either that seems weird, I would try setting it against the limits in the header, My header is always the same and I never have problems, as follows

G90G0X50.Z40.T0000M3M8G97S500

Then G1, or G0, whatever, obviously my machine has a little more travel than yours. Nothing personal its just bigger:) Robert

Thanks for all the help.I have the machine running and even managed an "IF THEN" statement for a parts counter.I was wondering if anybody knew how to get the parts catcher working.When I type M76 or M77 in MDI mode I get an unusable code message.I have also tried M88,M89,M90,&M91 none of which worked but did not give me an error message.I am thinking I need to assign either a 1 or 0 to a parameter bit.Thanks

hi dennis

for the parts catcher try m101 M102 or so, this worked for me

Thanks phx.That worked.It was funny to watch it deploy and the part role right off the end and not into the door.I readjusted it after that & it works great.

Could some one please explain G96 constant cutting speed.We are cutting 6061 aluminum .75" diameter 6.5" long.The part sticks 7.5" out of the chuck when we part it,it leaves a small nub on the part that falls.The parting tool geometry points toward the part that falls,and we put an arm on the parts catcher that deploys before it starts parting to support the work.
My question is what should I use after G96? The current code is:
G50 S2000(I did not like the spindle noises at 3000rpm)
M42 M03 S2000
G0 X.1 Z0
G96S1000
G01 X-.99
G01 X.1
G97 S2000
Should I use G95 (feed per revolution)after G96?
As it is coded the x moves very fast.

I guess I don't understand why the tool is feeding almost an inch past X- zero but the spindle will run as fast as the G50 command when it gets to X- zero. G96 allows the spindle to turn as fast as it needs to at the specified diameter, allowing the appropriate surface footage to be attained. Robert

I don't see a feedrate at all. The G95 is probably already active, but you may be feeding too fast.

dcoupar is right. If you've not assigned a feed rate on that line it will use the last called feed rate in the program. Look in the block data screen and you'll see the actual feed in inches per rev.

Most of Okuma's toolholders allow you to adjust tool tip to centerline. You may need to do this. Try using a standard grooving insert and face the part. If you still get a nub you need to adjust the the cam to slide the tool tip back to centerline. You can also slow down the rpms at the end of the cut to keep the part from breaking off due to centrifical force as well. I did not see any issues with your program and you seem to be using the correct cutter.