What's new
What's new

Okuma LB12 OSP500L-G Toolchange and X+ limit error

slodat

Aluminum
Joined
Jun 8, 2010
Location
Vancouver, WA
I can't get a tool change to work. I keyed in a program that was posted out from Fusion 360. It works great on T010101. Now I am trying to use another tool. T010101 is the finishing tool, T020202 the roughing. I keep getting an X+ limit over travel error after the tool change. The soft limit for X+ is set as high as I can make it. I'm new to lathe programming, obviously. I think what I need is to tell the control to ignore the soft limit, or take it out of play, when changing tools.

My origin in my chuck. Only using two tools - T010101 and T020202. X and Z offsets are set and correct. I know it's something about the way I'm doing it.

I'm new to the Okuma, and I know it's simple. Can someone show an example of how to program T010101, so some turning, then move the turret to the X+ limit, change to T020202, do some stuff, and back to T010101? Or show me what I'm doing wrong? I would really appreciate it.

This is my program. Keep in mind I do know I need to clean things up, there are most definitely easier ways to do this (I just don't know them yet), and I've mostly focused my experimenting around the first call to T010101:

Code:
$T3.MIN%
(3 INCH STAB)
G50S2000
G0X12
G0Z12
T020202
G90 G95
G97 S454 M3
G0 X5.525 Z4.75
G50 S2000
G96 S656 M3
G0 Z4.3016
X3.525
G1 X3.2381 F0.012
X3.125 Z4.245
X-.0312
X.0819 Z4.3016
G0 X3.525

G94 G40
G50 S2000
N80 G0 X12 Z12
M1
T010101
G90 G95
G97 S454 M3

G1 Z3.9316
G1 X3.2381 F.005
X3.125 Z3.875
X-.0312
X.0819 Z3.9316
G0 X5.525
Z4.75
G97 S454 M3
(ROUGHING)
G0 X12
G0 Z12
M1
T020202
G90 G95
G97 S656 M3
G0 X3.925 Z4.75
G50 S2000
G96 S656 M3
G0 Z3.8947
X3.0463
G1 Z1.0594 F.012
X4.125
X3.205 Z1.0994
G0 Z3.8947
X2.9675
G1 Z3.5937 F.012
X3.02 Z3.5675
Z1.0594
X4.0463
X3.1263 Z1.0994
G0 Z3.8947
X2.8888
G1 Z3.6331 F.012
X2.9675 Z3.5937
X3.0475 Z3.6337
G0 Z3.8947
X2.81
G1 Z3.6725 F.012
X2.8888 Z3.6331
X2.9688 Z3.6731
G0 Z3.8947
X2.7313
G1 Z3.7119 F.012
N118 X2.81 Z3.6726
X2.89 Z3.7125
G0 Z3.8947
X2.6525
G1 Z3.7512 F.012
X2.7313 Z3.7119
X2.8113 Z3.7519
G0 Z3.8947
X2.5738
G1 Z3.7906 F.012
X2.6526 Z3.7512
X2.7326 Z3.7912
G0 Z3.8947
X2.4951
G1 Z3.83 F.012
X2.5738 Z3.7906
X2.6538 Z3.8306
G0 Z3.8947
X2.4546
G1 Z3.8502 F.012
X2.4951 Z3.83
X2.5751 Z3.87
G0 Z3.8947
X2.4142
G1 Z3.8704 F.012
X2.4546 Z3.8502
X2.5346 Z3.8902
G0 X3.925
Z4.75
G97 S639 M3
G0 X12
G0 Z12
M1
(FINISHING)
T010101
G90 G95
G97 S656 M3
G0 X3.925 Z4.75
G50 S2000
G96 S656 M3
G0 Z3.9504
X2.4272
G1 X2.3908 F.012
Z3.8704
X3.005 Z3.5658
Z1.0594
X3.16
(FINISH 2)
G0 X3.925 Z4.75
G0 Z3.9504
X2.4272
G1 X2.3908 F.005
Z3.8704
X3. Z3.5658
Z1.1094
X3.16
G0X3.925
Z4.75
G97 S639 M3
G0 X12
G0 Z12
M2
%
 
Make sure you have decimals and your soft limits are set correctly.
Also, check the control's indicator lights. If you see the yellow light with the arrows illuminated then the machine is at its correct position. If that light is not illuminated, then the machine is not meeting a soft limit tool change requirement.
 
Hi Slodat.

Do you have IGF on your okuma ? if you do, throw fusion out the window ;)
If you learn IGF, you can program annything on your lathe.

You probably don't have the right post processor for your LB, these older machine's are very picky about the code.

I think the M1 code before the toolchange is your problem.
If you give me your drawing, I wil make the program in IGF and give it to you, so you can see how okuma wants the program.

Made a print screen of a program, so you can see how a tool change code should look.

for the fusion code, I think this will work. but please single block and finger on the stop button ;)

$T3.MIN%
(3 INCH STAB)
G50S2000
G0X12
G0Z12
T020202
G90 G95
G97 S454 M3
G0 X5.525 Z4.75
G50 S2000
G96 S656 M3
G0 Z4.3016
X3.525
G1 X3.2381 F0.012
X3.125 Z4.245
X-.0312
X.0819 Z4.3016
G0 X3.525

G94 G40
G0 X12 Z12
T010101
G97 S454 M3

G1 Z3.9316
G1 X3.2381 F.005
X3.125 Z3.875
X-.0312
X.0819 Z3.9316
G0 X5.525
Z4.75
G97 S454 M3
(ROUGHING)
G0 X12
G0 Z12
T020202
G90 G95
G97 S656 M3
G0 X3.925 Z4.75
G50 S2000
G96 S656 M3
G0 Z3.8947
X3.0463
G1 Z1.0594 F.012
X4.125
X3.205 Z1.0994
G0 Z3.8947
X2.9675
G1 Z3.5937 F.012
X3.02 Z3.5675
Z1.0594
X4.0463
X3.1263 Z1.0994
G0 Z3.8947
X2.8888
G1 Z3.6331 F.012
X2.9675 Z3.5937
X3.0475 Z3.6337
G0 Z3.8947
X2.81
G1 Z3.6725 F.012
X2.8888 Z3.6331
X2.9688 Z3.6731
G0 Z3.8947
X2.7313
G1 Z3.7119 F.012
N118 X2.81 Z3.6726
X2.89 Z3.7125
G0 Z3.8947
X2.6525
G1 Z3.7512 F.012
X2.7313 Z3.7119
X2.8113 Z3.7519
G0 Z3.8947
X2.5738
G1 Z3.7906 F.012
X2.6526 Z3.7512
X2.7326 Z3.7912
G0 Z3.8947
X2.4951
G1 Z3.83 F.012
X2.5738 Z3.7906
X2.6538 Z3.8306
G0 Z3.8947
X2.4546
G1 Z3.8502 F.012
X2.4951 Z3.83
X2.5751 Z3.87
G0 Z3.8947
X2.4142
G1 Z3.8704 F.012
X2.4546 Z3.8502
X2.5346 Z3.8902
G0 X3.925
Z4.75
G97 S639 M3
G0 X12
G0 Z12
(FINISHING)
T010101
G97 S656 M3
G0 X3.925 Z4.75
G96 S656 M3
G0 Z3.9504
X2.4272
G1 X2.3908 F.012
Z3.8704
X3.005 Z3.5658
Z1.0594
X3.16
(FINISH 2)
G0 X3.925 Z4.75
G0 Z3.9504
X2.4272
G1 X2.3908 F.005
Z3.8704
X3. Z3.5658
Z1.1094
X3.16
G0X3.925
Z4.75
G97 S639 M3
G0 X12
G0 Z12
M09
M2
 

Attachments

  • IMG_20230419_101717526.jpg
    IMG_20230419_101717526.jpg
    280 KB · Views: 1
Can you change your tool manually using the turret index button if you just turn the machine on, put it in manual, and handwheel up to the X limit? Your post is alittle confusing, are you starting with tool 2 and running the program you posted?

If you are getting an X overtravel, it could be because you still have tool 2 active while you are trying to go to X12. If you have a tool offset active and the machine can't go to that value wit the tip of the tool it will often alarm out. If you cancel the offset you can tell it to go to X12, X120, X120000, it won't care, it will simply go to rest on the soft stop. Th M01 should have no bearing on any of that working or not.

In this section:
X.0819 Z4.3016
G0 X3.525

G94 G40
G50 S2000
N80 G0 X12 Z12 T0200 (cancel the tool 2 offsets)
M1
T010101
 








 
Back
Top