Mori SL-25B program help.

[Johnhudson]

Machine has OT control,
My issue is call up T0101 and it rapids toward the chuck, I am not using G50,
Use T0100 and it works(kinda, not in auto coming from previous tool. It over travels in X and Z, Reset
Goto that line and presto it is good.(until the next tool change).
This code works and runs, But is not how I like it, (moving to the work piece in rapid with turret moving)

G0 T0101 X6.5 Z1.
G97 S400 M03
G0 G54 X6.492 Z.15 M8
G50 S1000
G96 S700
G99 G1 X2.7 F.012
X2.8 Z.2
M9
G28 U0. W0. M05
M01

(This works but not in auto)
( over travels during rotation)
G0 T0100 (Reset to here, it works)
G97 S400 M03
G0 G54 X6.492 Z.15 M8 T0101
G50 S1000
G96 S700
G99 G01 X2.7 F.012
X2.8 Z.2
M9
G28 U0. W0. M05
M01
Was thinking it is a parameter issue
But not sure.
Any ideas
Thanks in advance
John Hudson

 

[TeachMePlease]

What's your Z offset in T1?

 

[sinha]

When you command T0101, the offset is incorporated either by moving the tool or by changing the coordinate display, depending on a parameter.

 

[alphonso]

Just me, but I cancel the tool offsets before going home. I think the parameter Sinha refers to is 0013.2. 0 shifts coordinate without moving tool.

 

[Johnhudson]

What's your Z offset in T1?

T1 is Z zero face of part,

 

[Vancbiker]

....... (moving to the work piece in rapid with turret moving.......

By this, are you saying that the turret is rotating to the T01 position while the Z axis is moving? If so, there may be a PMC (Diagnostic) parameter that enables or disables that behavior. I seem to recall that Mori had that on the AL and CL series machines with the 0T control, but don't remember about the SL series.

 

[Johnhudson]

By this, are you saying that the turret is rotating to the T01 position while the Z axis is moving? If so, there may be a PMC (Diagnostic) parameter that enables or disables that behavior. I seem to recall that Mori had that on the AL and CL series machines with the 0T control, but don't remember about the SL series.

Yes exactly what is happening,
I Am just not comfortable with
Rapiding towards the work piece
With the turret unlocked and moving.

 

[Vancbiker]

You'll need to do a read through the PMC (Diagnostic) parameters in the back of the ladder diagram manual and see if there is a bit that needs to be changed to make it not do that.

When I helped a tier 1 auto supplier with a couple projects on Mori AL2 lathes, that function was activated so that cycle time was reduced. Typically it is set so that the turret finishes indexing before starting to move.

 

[Delw]

I just code it this way then I dont have to worry about it. ot control 88 miyano twin turrets

G50S1500
G30
M01
;
N2700
G00 T2700 M08
G96 S80 M03
G00 X-1.0 Z1.0 T2727 M28
X-0.2299 Z0.0501
X-0.2416
G01 Z-0.49 F0.002
X-0.2399
G00 X-0.2299 Z-0.4858
Z0.0501
X-0.2516
G01 Z-0.0427
X-0.2493 Z-0.0446
G03 X-0.248 Z-0.0471 R0.005
G01 Z-0.49
X-0.2416
G00 X-0.2316 Z-0.4858
Z0.0501
X-0.2616
G01 Z-0.034
X-0.2516 Z-0.0427
G00 X-0.2416 Z-0.0385
Z0.0501
X-0.2716
G01 Z-0.0253
X-0.2616 Z-0.034
G00 X-0.2516 Z-0.0298
Z0.0501
X-0.2816
G01 Z-0.0167
X-0.2716 Z-0.0253
G00 X-0.2616 Z-0.0211
Z0.0501
X-0.2916
G01 Z-0.008
X-0.2816 Z-0.0167
G97 Z4.0
G00 T2700
M01
;
M9
M29
M25
M30

 

[Johnhudson]

I just code it this way then I dont have to worry about it. ot control 88 miyano twin turrets

What does your M28 do?
It works that way for me until the next tool change then over travels.
Reset. Goto that line and its runs
Until the next tool change.

 

[Delw]

What does your M28 do?
It works that way for me until the next tool change then over travels.
Reset. Goto that line and its runs
Until the next tool change.

M28 is for high pressure coolant in our case or seconary coolant in most caes.
REASON FOR THE X- IS i AM USING BOTTOM TURRET.

we dont send home after any tools. only time I send it home is when I start the machine up. I dont use g54 or g50s except for max spindle speed.
my bottom line was screwed I just grabs a quick one that I hadnt used.

Ill fix it better

G50S1500
G30
M01
;
N2700
G00 T2700 M08 (CALLS TOOL UP)
G96 S80 M03
G00 X-1.0 Z1.0 T2727 M28 (CALLS TOOL OFFSET WHILE MOVING INTO POSITION)

Blah Blah Blah

G97 G00 Z4.0 (this is my tool change position as I have 2 turrets normally) I would go. G00 G97 X6.0 Z6.0
G00 T2700 (CANCELS TOOL OFFSET)
M01
;
M9
M29
M25
M30

IF YOU SEND THE MACHINE HOME AFTER YOU RUN TOO, YOU MUST CANCEL TOOL OFFSET 1ST. IF YOU DONT YOUR GOING TO OVER TRAVEL

 

[Delw]

You know what Im a dumbass.
send your machine off the switches (ie BEFORE you call up a tool offset) and Cancle it befor you go home.
sorry
i dont ever take machine home.

 

[Fancuku]

G50 S1000
G54
G00 T0100 M8
G96 S700 M3
G00 X6.492 Z.15
G99 G1 X2.7 F.012
X2.8 Z.2
M9
G28 U0. W0.
M01

That's what I do on older lathes with Fanuc controls.

 

[FrankieB]

For my own knowledge, do you to use a g00 to call up a tool with this machine?

 

[Johnhudson]

Update:
Parameter 14 needs to be bit 4
Fanuc helped me out.