G72 difficulty on Citizen L12X

[jgrasty]

I have a new Citizen L12X Swiss machine and am moving a large number of parts from a Mazak live tooled lathe to it. I have a problem with what I believe to be a correct tool path using G72 that the L12X control gives me an error when I run high speed check on the program. The code in question is (value in #500 = 0.0):

N4002
T0400 (TURN HOUSING THRU THREAD)

G0 G41 X0.4543 Z-0.0500 T04
G0 Z0
M97 (MAIN SPINDLE SPEED FLUCTUATION OFF)
G50 S6000
G96 S1000

G72 W0.0400 R0.0200
G72 P4020 Q4021 U0.016 W-0.008 F0.0040
N4020 G1 X0.4543 Z0.1540
X[0.0960 + #500] (CYL 0)
N4021 Z-0.0500
G0 X0.4543

Error from the control is: P204 E cmnd fix cycle error (MRC) 0 0 $1

The Mitsubishi manual says this error means one of the parameters of the G72 call is incorrect, but I can't find any problem at all. This code is lifted straight off my Mazak, though on the Mazak, I cut in the negative direction and on the L12X in the positive direction.

Ideas?

 

[sinha]

Please post the drawing

 

[jgrasty]

Here's the part. The portion done by the G72 code above is shown in the drawing as 0.098" diameter. The rest is done with a series of G1 calls.

 

[sinha]

N4020 G1 X0.4543 Z0.1540

Delete X, and Z should be negative, for machining on main spindle.

 

[sinha]

Z finishing allowance should be positive.

 

[DouglasJRizzo]

I'm surprised you're using G71/G72 on a Swiss style at all..

 

[angelw]

Delete X, and Z should be negative.

Z finishing allowance should be positive.

All that is correct, for the OP is cutting in the Z+ direction. The X0.4543 being the same as the OP's X Start position before executing the G72 Cycle would invoke the Type 2 Cycle, if the Control has that.

G0 G41 X0.4543 Z-0.0500 T04
G0 Z0

Starting at Z0.0 and finishing at Z-0.0500 may be causing an error and although specifying an X Value in the "P" referenced Block should just invoke Type 2 G72 Cycle, if your control doesn't have this option, an alarm will be raised, therefore, omitting X in that Block would be a likely test.

Regards,

Bill

 

[sinha]

.

Starting at Z0.0 and finishing at Z-0.0500 may be causing an error

It is not clear whether machining is being done in +Z or -Z direction, and how the workpiece is clamped.

 

[angelw]

.

It is not clear whether machining is being done in +Z or -Z direction, and how the workpiece is clamped.

Hello Sinha,
The OP's program starts at Z Zero, Face Roughs to Z+0.154 and finishes at Z-0.0500. The part would be held in a RH Spindle.

Regards,

Bill

 

[sinha]

I

Hello Sinha,
The OP's program starts at Z Zero, Face Roughs to Z+0.154 and finishes at Z-0.0500. The part would be held in a RH Spindle.

Regards,

Bill

In such a case, the program appears to be correct, unless type 2 is not available.

I will suggest some radial clearance at the start point.
He has G0 G41 X0.4543 Z-0.0500 T04
May try X0.5 in this block.
I had faced a similar problem long time back, though on an emulated Fanuc.

 

[TeachMePlease]

G72-Face rough cutting cycle. Basicly the same as G71 but cutting in X axis motion down
and Z-

G72W.05R.04
G72P100Q200U.015W.002F.012S4000

1st G72
W.05 = Cutting amount in Z axis per cutting pass
R.04 = Amount of pull out of Z axis after each pass to retract back for
the next cut.

2nd G72
A = Program number used for the finish shape
P100= If not using 'A' then P = the starting line number of the finish shape
program.
Q200= If not using 'A' then Q = the ending line number of the finish shape
program.
U.015 = Amount to leave in X axis for finishing
W.002 = Amount to leave in Z axis to leave for finishing
F.012 = Feed rate for roughing. Even if a feed is in N100-N200, this feed is
used.
S4000 = Spindle speed used for roughing, even if S is in N100-N200 this S is
used.

It's almost definitely the W-.008. Just make it .008.

 

[jgrasty]

It appears to be a parameter issue, I am investigating and will report back.

 

[jgrasty]

It was a parameter problem. Citizen suggested setting user parameter 8014 (G71 delta-D) to 0 and now the code above works as expected.

 

[sinha]

What is the description of this parameter?