okuma mu6300 turning function. Machine wont move past block no alarms

[lowcountrycamo]

Hi Guys,

I am running the Turning function (quadturn) on an MU6300 universal mill for the first time.   Postabilty post.   When the program gets to the first G95 G01 block the machine stops.   There is a distance to go but machine will not go further.  No alarms,  Single block off, feed 100%.   Hitting cylce start again does nothing.  
 

Thanks,

steve austin

 

G00 G18 G20 G40 G80 G90
G30 P10
M509
M531
N1
(MITS TURNING HOLDER DDJNR3225P15 - INSERT DNMG432RP .0312CR)
(OPERATION NO - 18)
(OPERATION TYPE - FINISHING)
IF [VTLCN EQ 19 ]  NT19
T19 M06 (OD 55 DEG LEFT)
NT19
G15 H1
G30 P10
M19 RS=0
M508
G00 G18 G90 A0.
M540
G450 SB=280
G197 SB=280 M503
G431 X1
G433 H1019 X1
X-.9996 Y0. Z9.7256 M08 T7
G196 SB=280 X1 M503
G42 Z9.6955
G95 G01 Z9.5955 F.007  <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<----- stops here
Z9.3155
X-1.0113 Z9.2925
X-1.0522 Z9.2864
G40 X-1.1936 Z9.3571
G00 Z9.7256
M505
G30 P2 M09
G432
M01

[ajmer]

check if machine is set to inch/min

0.007"/min looks like it is not moving

 

[AHarrison1]

6 minutes ago, ajmer said:

check if machine is set to inch/min

0.007"/min looks like it is not moving

 

The G95 at the beginning of that line is Feed per revolution mode as per

https://www.helmancnc.com/okuma-mill-g-and-m-codes/

 

[crazy^millman]

Has all the unlock and lock commands for the axis been established? Has the tool been defined correctly on the Control? Is there code need to tell the machine it is turning mode and not milling mode?

[lowcountrycamo]

it turns out that I needed a Mcode, M130.  This allows the machine to feed while spindle not turning, even though the C axis is now the spindle.  There is nothing in the Turning Function Manual about this.  One of my programmers thought of it and I added it to my post.

Thanks for all the suggestions,

steve austin

[Greg Williams]

Sounds like the tool is defined as a mill tool and not a turnng tool