What's new
What's new

Haas Lathe 603 Non-Monotonous Error code

Sb1

Plastic
Joined
Aug 26, 2019
I am having trouble with a 603 non-monotonous code using a Haas CNC Lathe and was wondering if anyone could help me with the problem?



G20 G40 G80 G97 G99 (INCHES, CUTTER COMP OFF, CANNED CYCLE OFF,)
G28 (TURRET STARTS IN HOME POSITION)
T404 (NEUTRAL TOOL)
G50 S6000 (CAP SPINDLE SPEED RPM)
G97 S800 M03 (START SPINDLE CLOCKWISE IN RPM)
G54 G00 F.02 X.8 Z-1.063 (Safe Start Point) (M08, SET G54 AND RAPID TO STARTING POINT)
G96 S600
M08 (COOLANT ON)


G71 P10 Q70 U0.02 W0.02 D0.02 F0.01

N10 G42 (CUTTER COMPENSATION RIGHT)
N20 G01 X0.625 Z-1.063
N30 G02 X0.2 Z-1.25 R.1875
N40 G01 Z-4.250
N50 G02 X0.625 Z-4.438 R.1875
N60 G01 X0.8
N70 G40

G28 (TURRET RETURNS HOME)

G70 P10 Q80 F.005 (FINISHING PASS)

X.8 (SAFE SPOT OUT OF CAVITY)
M09 (STOP COOLANT)
G28 (GO HOME)
M05 (STOP SPINDLE)
M30 (END PROGRAM)




The bold portion is where the error occurs. Thank you in advance! (Note: I am relatively novice to CNC coding)
 

Hoss710

Cast Iron
Joined
Jun 16, 2019
The path defined by PQ was not monotonic in the Z-axis. A monotonic Path is one that does not change direction starting from the first motion block. The control is looking for the Z-axis to move in a continuous motion from the face of the part towards the chuck or from the face of the chuck towards the end of the part. You cannot change direction in the Z-axis with out defining the tool path as a type II canned cycle. If this is the case you need to add a X-axis reference on the same line as the first Z-axis move after the G71.
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
I am having trouble with a 603 non-monotonous code using a Haas CNC Lathe and was wondering if anyone could help me with the problem?



G20 G40 G80 G97 G99 (INCHES, CUTTER COMP OFF, CANNED CYCLE OFF,)
G28 (TURRET STARTS IN HOME POSITION)
T404 (NEUTRAL TOOL)
G50 S6000 (CAP SPINDLE SPEED RPM)
G97 S800 M03 (START SPINDLE CLOCKWISE IN RPM)
G54 G00 F.02 X.8 Z-1.063 (Safe Start Point) (M08, SET G54 AND RAPID TO STARTING POINT)
G96 S600
M08 (COOLANT ON)


G71 P10 Q70 U0.02 W0.02 D0.02 F0.01

N10 G42 (CUTTER COMPENSATION RIGHT)
N20 G01 X0.625 Z-1.063
N30 G02 X0.2 Z-1.25 R.1875
N40 G01 Z-4.250
N50 G02 X0.625 Z-4.438 R.1875
N60 G01 X0.8
N70 G40

G28 (TURRET RETURNS HOME)

G70 P10 Q80 F.005 (FINISHING PASS)

X.8 (SAFE SPOT OUT OF CAVITY)
M09 (STOP COOLANT)
G28 (GO HOME)
M05 (STOP SPINDLE)
M30 (END PROGRAM)




The bold portion is where the error occurs. Thank you in advance! (Note: I am relatively novice to CNC coding)

Hello Sb1,
Error 603 is certainly for a non-monotonic move in the Z-axis in a Multi-repetitive Cycle. However, the profile itself doesn't have non-monotonic Z moves per se. I believe the error is being raised by the way in which you're applying and cancelling TNR Comp within the Cycle Profile. Tool Rad Comp Start Up should occur in the P reference Block and the first definition Block of the profile should also be in the P Reference Block. Your current program doesn't have the first Block of the profile in the P referenced Block.

Regards,

Bill
 

doug925

Titanium
Joined
Nov 21, 2002
Location
Houston
Try this...

G97 S800 M03 (START SPINDLE CLOCKWISE IN RPM)
G54 G00 F.02 (M08, SET G54 AND RAPID TO STARTING POINT)
G00 Z-.99
G96 X0.8 (Safe Start Point) S600
M08 (COOLANT ON)


G71 P10 Q70 U0.02 W0.02 D0.02 F0.01

N10 G00 Z-1.0625
N20 G01 X0.575 G42 (0.2 + 0.375 = 0.575)

N30 G02 X0.2 Z-1.25 R.1875 (the math must add up exactly, NO rounding. Either program the 4th decimal, or ditch the 5 on the end of R.1875)
N40 G01 Z-4.250
N50 G02 X0.575 Z-4.4375 R.1875
N60 G01 X0.8
N70 X.9 G40
......
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
Hello Sb1,
Doug makes a good point regarding the X0.575 coordinate. Your original program profile runs successfully as a Finish Profile because of the R Format Circular Interpolation being used. The control simply moves the arc centre to accommodate the specified Start/End coordinates specified and is the reason for the non-monotonic move in the Z-axis; the following picture shows that there would be a Z+ movement before there being a Z- movement when the Circular Move is executed at the Start of the profile. The same issue exists at the Finish of the profile when there would be a Z- movement at the Start of the Radius, finishing with a Z+ movement. Another case of where I/K format would probably have indicated an error with the arc command.

HAAS-603-2.JPG

Because a G71 cycle is being used, and because your profile has non-monotonic X moves, so as to invoke Type II of the G71 Multi-repetitive Cycle, both X and Z coordinates are required to be included in the P reference Block of the Profile.


Regards,

Bill
 

Ringcn

Plastic
Joined
Dec 23, 2019
I always put rapid in z in front of the part then rapid in x staying away a little bit. Then on my first n line after my g71 I put g01 g42 with an x and z. Put the x value where I want to start my cycle in x and put the z with the same value I rapid to at the beginning. That way tool nose compensation activates and only moves in the x direction. Then I start writing my path.
 

Ringcn

Plastic
Joined
Dec 23, 2019
I think if you just moved your n20 line onto the same line as your n10 line your code will work
 








 
Top