G71 - Fanuc 6T - Not steadily (de)increasing in X

[bdphillips03]

Thought this may be better suited in this forum:

Trying to run a G71 canned cycle and keep getting the above alarm. This is probably simple but I just don't get it. Thanks for the help. If this should be in another forum please let me know where. Brian

:0005
G28U0W0
N0001
G00T0101
G50X3.500Z3.00
G00X1.6Z0.05
G97S900M04
G71P1000Q2000U0W0D1500F0.003
N1000G00X1.55
G01Z0.0
G01X1.1876Z-0.5
G01X1.25Z-0.642
G03X1.3664Z-0.942R0.5147
G03X1.0822Z-2.0604R4.6712
G02X1.1251Z-3.007R3.8931
G03X0.875Z-3.142R0.1254
N2000G01X0.975
G00Z0.05
G00X1.5Z3.0T0100M09
G28U0W0
M05
M30
%

[Geof]

I have not looked at your code in detail but I think what you are getting would be called a "non-monotonous" X motion on a Haas machine. What it means is that one of your lines has the X reversing direction.

G71 and G72 have what is called type 1 and type 2 motion (on a Haas at least) and with type 1 you are only allowed to go in the negative direction.

Look for a move that is trying to make the X go positive, i.e. less negative.

[mike cncmachine]

line n10000 should be your smallest x move

[dcoupar]

It looks to me as you're doing an ID roughing op, right?

The X values increase and decrease in the profile definition, so you need to run a "Type II" roughing cycle, which requires BOTH an X and Z move in the 1st block of the finish shape definition (N1000)

I also tweaked your start and end points (the tool was gouging at the bottom of the profile.

Try this:

%
O0005
G28U0W0
N0001
G00T0101
G50X3.500Z3.00
G00X0.85Z0.05 (START POINT CHANGED)
G97S900M04
G71P1000Q2000U0W0D1500F0.003
N1000G00X1.55Z0.05 (BOTH X AND Z HERE)
G01Z0.0
G01X1.1876Z-0.5
G01X1.25Z-0.642
G03X1.3664Z-0.942R0.5147
G03X1.0822Z-2.0604R4.6712
G02X1.1251Z-3.007R3.8931
G03X0.875Z-3.142R0.1254
N2000G01X0.85 (END POINT CHANGED)
G00Z0.05
G00X1.5Z3.0T0100M09
G28U0W0
M05
M30
%

[bdphillips03]

Thanks for the fix. Found out by trying to run it that I can't use type II cycles with this lathe. When I tried to run the new code. Does this mean I will have to use I,K,X,Z ; I,K,U,W commands to turn the radi?

[Andre' B]

Originally Posted by bdphillips03 Thanks for the fix. Found out by trying to run it that I can't use type II cycles with this lathe. When I tried to run the new code. Does this mean I will have to use I,K,X,Z ; I,K,U,W commands to turn the radi?

How about a few G71's to get rid of most of the material.
And then program the full path, put it in a WHILE loop with a G52 and step it into the part. It will work just like a G73 but no complaints about nonmonotonic (sp?) motion.

O0005
G28U0W0
N0001
G00T0101
G50X3.500Z3.00
G00X0.85Z0.05 (START POINT CHANGED)
G97S900M04

(PUT IN ROUGHING G71 CYCLES)

(CHANGE THESE AS NEEDED)
#100=0.002(X FINISH)
#101=0.500(X ROUGH)
#102=0.050(STEP SIZE)

#104=[-#101-#100](OFFSET)
WHILE[#101GT0.0]DO1
N1000G0G52X[#104]
G00X1.55Z0.05 (BOTH X AND Z HERE)
G01Z0.0
G01X1.1876Z-0.5
G01X1.25Z-0.642
G03X1.3664Z-0.942R0.5147
G03X1.0822Z-2.0604R4.6712
G02X1.1251Z-3.007R3.8931
G03X0.875Z-3.142R0.1254
G01X0.85 (END POINT CHANGED)
N2000G0Z0.1
#101=#101-#102
#104=[-#101-#100]
END1

(LAST ROUGH PASS)
#104=-#100
G70P1000Q2000

(FINISH PASS)
#104=0.000
G70P1000Q2000

(SPRING PASSES IF NEEDED)
G70P1000Q2000
G70P1000Q2000

G00X1.5Z3.0T0100M09
G28U0W0
M05
M30

[dcoupar]

He doesn't have the Type II canned cycles option. I'd be real surprised if he has User Macros...

[bdphillips03]

Yep, checked my book when I got home. The lathe doesn't support G52. Here is the list of what it will do. I really appreciate the help you all are giving me!! I have attached a dxf of the part (profile) I am making. My orginal code leaves out the two small vertical lines and the small horizontal line. Then the long horizontal line is connected to the first radius. Do you all think I should just break the G71 cylces down into individual radi? Thanks again!! Brian

The following "G" codes are supported:

G00 Rapid traverse mode
G01 Feed rate mode
G02 Circular interpolation clockwise
G03 Circular interpolation counterclockwise
G04 Timed pause in program
G20 Inch mode
G21 Millimeter mode
G22 Software stroke limit on
G23 Software stroke limit off
G28 Return to home position in called axis
G29 Return from reference point
G32 Plain threading cycle
G40 Tool nose compensation cancel
G41 Tool nose compensation left
G42 Tool nose compensation right
G50 Set 0,0 position and maximum spindle speed
G70 Canned cycle, Finishing cycle
G71 Canned cycle, OD roughing cycle
G72 Canned cycle, Face roughing cycle
G73 Canned cycle, Profiling cycle
G74 Canned cycle, Face grooving cycle
G75 Canned cycle, OD grooving cycle
G76 Canned cycle, Thread cutting cycle
G90 Cutting cycle A
G92 Thread cutting cycle
G94 Cutting cycle B
G96 Constant surface speed mode, G97 cancel
G97 Constant RPM mode, G96 cancel
G98 Feed spec. in inches per minute, G99 cancel
G99 Feed spec. in inches per revolution, G98 cancel

The following auxiliary codes are supported:

D Depth of cut, etc., in canned cycles, other uses
E Lead specification in long format (optional)
F Feed rate specification
I X direction radius offset in circular interpolation
K Z direction radius offset in circular interpolation
L Repeating factor
N Line numbering
P Subroutine call out and canned cycle usage
Q Canned cycle usage
R Radius designation in circular interpolation
S Spindle speed specification, surface speed spec.
T Tool and tool length offset compensation (optional)
U Incremental movement specification, part diameter
W Incremental movement specification, length of part
X Absolute movement specification, diameter of part
Z Absolute movement specification, length of part