[qtgalb]

We recently received a mori seiki sl7 lathe with fanuc 6t controller and do not have a programming manual. Since this controller does not have geometry, how can we set-up a work coordinate closer to the part without sending the machine home at every tool change? Any input or example would be greatly appreciated. Thanks.

[actionman]

Try G50X---Z--- at beginning of each tool
and the same number at end of each tool but change G50 to G00 at end
the X--- Z--- represents the tool touch point on face of part for Z(usually different for each tool)
X--- is touch off known dia. add that to X on screen(the point is to tell the machine where center is
see ex.


%
:0069(TEST)
(R TURN)
G50X9.724Z5. ( tool touch points )
G0T0101
G97S700M3
G0G99X2.1Z.1M8
G71P100Q200U.02W.002D400F.01
N100G0X0
G1Z0.F.003
X1.2616
G3X1.2908Z-.006R.0206
G1X1.3649Z-.0431
G3X1.377Z-.0577R.0206
G1Z-.375
X1.795
X1.875Z-.415
Z-.8
X2.05
N200X2.1
G0Z.1M9
G0X9.724Z5. ( return point )
G0T0100 (clear offset )

M1 (F TURN )
N55G50X8.673Z5.006 (next tool )
G0T1010
G97S550M3
G0G99X2.06Z.1M8
G70P100Q200
G0Z.1M9
G0X8.673Z5.006
G0T1000
M1

hope this helps
Joe

[qtgalb]

Joe, thank you very much for your example. I will give it a try and let you know.

Angelo

[hiiesalu]

I Use A G50 As Follows With Block Skip (/)
When Setting Up Switch Off Block Skip And Start Each Tool At G28u0.w0. / This Sets Your G50 And Goes Home You Do Not Have To Manuall Move Turret Home"faster Setup"/ Must Keep G 50 Xz Same For All Tools/ When You Run Job Allow Program To Run Thru First G50 And Turn On Block Skip/ If You Interrupt Cut
Turn Off Block Skip Start At Any G28u0.w0.
Should You Forget To Turn Off Block Skip Turret Will Travel Away
From Not To Work Overlimit Will Turn On But No Crash(works For Me)g50 Remains Till Reset Or Machine Is Turned Off
Once All My Tool Offsets Are Made They Never Have To Be Changed
I Only Change The Z Amount On The G50 (usally Not X)
I Set My Turret Face To Chuck Face Measure The Distance Say 20.0
And Call This Z Zero Now If My Part Extends 2.0" From The Chuck My
Z Is 18.0 Or G50z18.00x10. And So On (remember All Tools G50 Xz The Same)
This Works On My Older Fanuc 6t (not Explained Here, If You Have A Work Shift Function On A Newer Fanuc Its Better To Use It)
Program Example
%
:0069
/g28u0. W0. Block Skip
/g50x10.z20. Block Skip Keep G50 The Same For All Tools
G0t100 Index To Tool 1
97m3s700
Gog99x2.0z.0t0101 Offset In The Move
G1x.of.004 Face Part
Z.050
Gotox5.0z5.0 Clear Offset Index Point Without Going Home
/g28u0. W0. Block Skip (to Run Tool 2 Only Start Here Blk Skip Off
/g50x10.z20. Block Skip
G0t200 Indx Tool 2
G97m3s700
G0g99x2.0z0.t0202 Offset In The Move
G1z-1.0f.004
X2.1
G0t0x4.0z3.0 Clear Offset Index Closer

[scappini]

is there a G30 on your lathe with perhaps mechanical dogs you can move around??


Cheers :cheers:

[hiiesalu]

My Ikegai does not have a G30 or dogs to move, and I used to have to move
all the way home to index, Newer machines with 6T controllers have a work shift in the offset page and you use this as a master Z if you have this then this is the best way.

Push the offset twice and you should see: Work Shift
00 Z0.0000
X0.0000
If you do not have this then you use a G50

[cacrawfo]

Hello,
If you have a 6T-B version of the controller with custom Macro B, you can set up a trick little Macro to "fake" tool and work offsets even thought the controller does not have it.
If you only have the 6T-A version, you still may have a second or even third "return refference point check" that you can set and use as if it were the G28 return. You just have to be extremely carefull and write redundancies into your program to make restarting tools safe for operators.

A second refference return might work like this:

Chose your first tool and touch it off just like normal. Zero your displays in position screen that shows U and W to reflect the current position of the tool in relation to your chosen Z zero and x diameter. Send this tool to your chosen safe index position. Make it something easy like X 5.0 Z 6.0 Set this as your return refference point check. (not sure of the code) Your G50 for this particular tool will be x5.0 and z6.0

Now use this new position as your new intermediate home postion. Set your next tools G50 in refference to it, and after you use each tool, send it to x5.0 and z6.0 instead of G28 U0 W0. Cancel any wear offset. Now you can command the code for "second return refference point check" and the machine will compair the current position against what it has stored for the refference check. It does this in Machine Position, which is completely seperate of the offset position, or current position. If you have messed something up, it will alarm out and refuse to move. If the position matches up, (which it should!) it means you have returned the turret to your new intermediate home position and you can continue.
It is just like using G28 U0 W0, but instead of testing the machines positon against the home switches, you are testing it against the Machine Position. For this reason, you may want to G28 return the machine at the begining of each cycle. Maybe where a part is loaded, etc. That will prevent any problems if the machine misses a few counts on an encoder every once in a while untill it adds up...

Cheers!
Carl Crawford

[Chappy]

I run an Ikegai AX30N lathe and use what I call a home program which I keep in memory. I usually touch off on the part with the finish turn tool and move the machine out 8 inches manually and zero origin. I then run the home program which is as follows:
G40 G28 U0
G28 W0
M00
G04 X1.0
G00 W-44.5143
U-.74
M30
I then Press Cycle Start, and the machine moves to zero return. I then change the value W-44.5143, which could be any value, to what the value is in the position screen. If the W value in the position screen is W43.6157, I change the W-44.5143 to W-43.6157. Press reset and Hit Cycle Start twice and when the machine moves to within 8 inches of the part it should stop. Zero origin the U value in the position window. On my machine the U-.74 means my X value in the machining program is (G50 X17. Z8). If the X value in the machining program was X14, the U Coordinate in the home program would be U-3.74. At the end of the program cycle a G00 Command reads G00 X17. Z8. M09; and the machine moves 8 inches away from the part instead of returning to zero everytime. Sort of complicated but play with it and see what you think.
Chappy