[jessebpm]

To start off the shop i work at has just purchased a okuma howa with a fanuc 18-t control. noone here has programmed this machine before. i am having trouble with the machine going past home when i give it a X+ Z+ for a tool change. what are we doing wrong. all the other okumas we have are not like this. thanks

jesse

[Algirdas]

i am having trouble with the machine going past home when i give it a X+ Z+ for a tool change
is it lathe?
is the trouble a sound, smoke/ smell or maybe some error message there?

[CNCZILLA]

Like Algirdas said, we need more info on the problem. I have some manuals and procedures for this control. Let me know an e-mail and after the holiday weekend i will see about sending them to you. They are in Adobe pdf.

[Oti]

with a fanuc 18-t control

Since it is a Fanuc control, i would think your home line should look like this:

Nxxxx G28 U0.0 Z0.0

Fanuc and OSP are a bit different.

[Chris D]

Since it is a Fanuc control, i would think your home line should look like this:

Nxxxx G28 U0.0 Z0.0

Fanuc and OSP are a bit different.

I think you meant G28 U0 W0

Chris

[jessebpm]

ok sorry guys yes it is act 15 lathe. no problem with the machine. just a programming problem. i think chris is on the right path. i did try this and when i give it the G28 line it nolonger give the overtravel alarm. but it does not go to the correct position to where my tools are touched off to X0. Z0. i wants to go past them. Is there anything special i have to do when touching off my tools. as in a work coord. or anything that would be diff from our other okuma lathes.

jesse

[Chris D]

Your geometry and or wear offsets are probably still active. You may need to cancel them with the addition of T0

G28 U0 W0 T0

Chris

[jessebpm]

ok tried the G28 U0 W0 T0. the machine will atleast move toward the turret now. however now it goes way past where i have the tool zeroed at. if someone had a simple sample program i could look at it might help me understand what i am doing wrong.

thanks

[Chris D]

ok tried the G28 U0 W0 T0. the machine will atleast move toward the turret now. however now it goes way past where i have the tool zeroed at. if someone had a simple sample program i could look at it might help me understand what i am doing wrong.

thanks

Unfortunately your explanations are part of the problem. How can the machine move towards the turret? I tried to reason that out as the axis moved towards the turret but that didn't make sense either. Let's try this...

G28 U0 W0 T0
This command will send the axis to home position and cancel any active tool offsets.

G28 X0 Z0 T0
This command will send the axis to home position and cancel any active tool offsets, however, it will first move to absolute zero which can result in a crash.

G00 X0 Z0
This command will move the axes to absolute X0 Z0. Now, if you don't have any offset active, that means the tool lengths will not be taken into account and the turret may try to get to the part (destroying the tool on it's way).

T0101
This will call up tool one (T01), the second 01 activates the offsets stored in register 01. There can be wear offsets (on the wear page) and Geometry offsets (on the Geometry page).

T0
Cancels all active tool offsets (wear and geometry).

Chris

[jessebpm]

sorry i know i am not the best at explaining what i mean. here is what i think i am saying. If i command G0 X0 Z0 the turrett in my machine goes as far away from the chuck as it can. almost like absolute zero has been changed to machine home position. let me know if this helps

[Thawk53]

%
Jesse,
Are you sure this machine has geometry offsets. We used to have a twin spindle Okuma-Howa (late 1980's model) that required the use of the G50 coordinate system. I don't recall what control was on this machine. I have included a program from this machine for your reference.

Rick

N10G0G28U0W0
N20M11
N30M1

N40G0G28U0W0
N50G50X20.014Z19.115S400
N60T0500M74
N70G97S50M3
N80X14.85Z0.13T0505M8
N90X13.85
N100G96S126
N110G99G1X10.3F0.011
N120G0Z0.23
N130X13.85
N140Z0.065
N150G1X10.3
N160G0Z0.165
N170X13.4534
N180G1X13.73Z0.0267
N190Z-1.575
N200G0X13.83Z-1.525
N210Z1.1
N211G97S50M75
N220G28U0W0T0500M9
N230M1

N240G0G28U0W0
N250G50X22.554Z12.71S400
N260T1100M74
N270G97S50M3
N280G99X10.4Z1.1T1111M8
N290Z0.165
N300G96S121
N310G71U0.1R0.05
N320G71P330Q360U0W0F0.012
N330G0X11.3366
N340G1X11.06Z0.0267F0.012
N350Z-1.3
N360X10.96
N370G0Z1.1
N380G97S50M75
N390G28U0W0T1100M9
N400M5
N410M12
N420M0

N430M11
N440G0G28U0W0
N450G50X20.014Z19.115S400
N460T0500M74
N470G97S50M3
N480X14.85Z-0.0883T0505M8
N490X13.85
N500G96S126
N510G99G1X13.6734Z0.0F0.011
N520X10.3
N530G0Z1.1
N540G97S50M75
N550G28U0W0T0500M9
N560M1

N570G0G28U0W0
N580G50X22.554Z12.71S400
N590T1100M74
N600G97S50M3
N610G99X9.8Z1.1T1111M8
N620Z0.1
N630G96S105
N640G71U0.1R0.05
N650G71P660Q700U0W0F0.0105
N660G0X13.0606
N670G1X12.784Z-0.0383F0.0105
N680Z-1.779
N690X11.1366
N700X10.96Z-1.8673
N710G0Z1.1
N720G97S50M75
N730G28U0W0T1100M9
N740M5
N750M12
N760M30
%