Okuma Lathe Post M15/M16?

[BenK]

I'm trying to get a post setup to run for an Okuma lathe with live tooling. I am trying to do some C axis milling but can't get the M15/M16 codes to output correctly. Has anyone run into this in the past? Or can one of the post gurus help point me in the right direction?

I was hoping to be cutting chips tomorrow so I can't really just wait for the post builder to get back to me. 

 

LSPN
G50 S6000
G00 X22. Z22.
DEF WORK
PS RC,[01,0],[0,0]
END
CLEAR
DRAW
M01
N1
M01
T0404
(FINISH LOCATING FACE)
M110
G94 SB=2000
M13
G18
M146
G00 C3.586 M15
Z1.
X5.995
M08
Z.1
G94 G01 Z-.3 F30.
X5.8079 C3.702 F12.1
G41 D4 X5.6208 C3.825
X5.5719 C3.826 F.61
X5.5232 C3.76 M16 F15.58
X5.4759 C3.627
X5.4306 C3.428
X5.3883 C3.165
X5.3498 C2.841
X5.3158 C2.461
X5.287 C2.032
X5.2639 C1.562
X5.2471 C1.06
X5.2368 C.536
X5.2333 C0.
X5.2334 C180. M15  <--- should not be output
C0. M16  <--- should not be output
X5.2368 C359.464 M15  <--- should not be output
X5.2471 C358.94 M16  <--- should not be output
X5.2639 C358.438
X5.287 C357.968
X5.3158 C357.539
X5.3498 C357.159
X5.3883 C356.835
X5.4306 C356.572
X5.4759 C356.373
X5.5232 C356.24
X5.5719 C356.174
X5.6208 C356.175 M15 F.37
X5.8079 C356.298 F12.63
G40 X5.995 C356.414
Z.1 F100.
G00 Z1.
M09
M12
G00 X22. Z22. T0400
M146
M109
M102
M02

 

[Greg Williams]

What control do you have?

M960 will give you shortest path on the later P200L and P300L

The control will not like the D value on the G41 line you will need to use the tool offset T040404

[gcode]

depending upon whether or not you post respects machine and control definition settings,

you might get the results you want by changing these settings

They can be found on the Propertied page on the C axis in the Control Definition

 

see attached file

 

C axis rotary settings.pdf

[BenK]

Control is a OSP-P 300L.

I will have to look into the M960.

Yes the post does respect the control definition. I tried signed continuous but that output C axis values above 360° that the machine didn't like. I might have to try shortest direction and see what happens.

Keep the suggestions coming, I would rather have several things to try before I make the drive. 

[gcode]

9 hours ago, BenK said:

X5.2333 C0.
X5.2334 C180. M15  <--- should not be output
C0. M16  <--- should not be output

if you delete the M15 and M16 from these lines does the machine execute the code properly

If you set M960 (shortest distance) the machine has 2 solutions moving from C0 to C180 and does not know which is the desired motion.

see attachement

M15-M16.pdf

[BenK]

Yes, all It takes is removing those codes. I would do that in a heartbeat to get this project rolling if the code was this simple but this is just a sample code I put together for testing. 

 

You are correct about the M960 it doesn't know what direction too go.. I have tried breaking the moves but I can't get it to. That is what I have been working on this morning.

[gcode]

does your post have this variable

fullrev        : 0      #Machine capable of rotating 360 or more in a single line [0=No,1=Yes]

[BenK]

I'm not finding anything.

[BenK]

Huge shout out to Gcode for helping me with this. I'm now using the Okuma face interpolation function and it's working perfectly. Before today I didn't even know this function existed. Thank you. 

[Mick]

Face interpolation? You mean coordinate conversion function? (G101/102/103)?

Where have you been?

[BenK]

14 minutes ago, Mick said:

Face interpolation? You mean coordinate conversion function? (G101/102/103)?

Where have you been?

Yes, that's what I mean. 

I have been in the land a Fanuc and Siemens for too long I guess. This has been a learning experience to say the least. 

[gcode]

Face interpolation is not unique to Okuma

Fanuc mill/turns can do this as well, and most Mastercam lathe posts can output the code

[Greg Williams]

Happy to help you out Ben. You will get a smoother result if you use G137 Y to C conversion

NAT6
G50 S4000
M110
G0 X888. Z555. T060606
SB=2546 M13
M9
G17
Z30.
C0.
G137 C0
G0 G94 X-100. Y-10.
G17
Z10.
G101 Z-10. F3.6
X-90. F381.9
G103 X-80. Y0. L10.
G102 X0. Y80. L80.
X80. Y0. L80.
X0. Y-80. L80.
X-80. Y0. L80.
G103 X-90. Y10. L10.
G101 X-100.
G0 Z30.
G136
M12
M109
G0 X888. Z555. M9
T0600
M02

[BenK]

The way it looks G137 is the only way I will get any results. I made it my default when posting so this doesn't come up again.

 

12 hours ago, gcode said:

Face interpolation is not unique to Okuma

Fanuc mill/turns can do this as well, and most Mastercam lathe posts can output the code

Maybe I should have said I have been in the land of 5-Axis milling instead. I haven't spent much time on a Lathe but that looks like its changing. Most all controls have comparable features now. It's amazing what you can do.

[Zoffen]

I used to use the G12.1 Polar interpolation on the live tool mazaks alot. That feature is great. Just watch out for a rapid move going through  centerline in this mode as alot of the accell/decell stuff is not taken into account. It will rapid to center and back and servo overload on this move as the c spins 180 and the x axis reverses real fast and the machine does not like this especially on a larger lathe with a larger turret with all that mass. I had this on a few programs and all i did was manualy change this move to a fed move. Hope this makes sense and helps someone in the future.

[Brad Lisle]

if you enable shortest direction and force to output every quadrant that solves the 0-180 direction issue. It would go 0-90-180 or 0-270-180.