[teamjnz]

Hello,

Sorry I posted the original in the wrong forum

I am having troubles... I have been CNC turning parts for years. I buy a used small CNC lathe, 1998 Femco with a Fanuc O-T control. I score a small first job. Now I try and run the machine for the first time and it doesn't like the canned cycles.

Please help... Could it be the a turned off parameter??

The alarm reads 010 P/S. My books says "unusable G code commanded" It bombs out when it reads the G71 line and the G76 line. I can work around the G71 rough cycle but I need to be able to thread the part.

Here is the code
(ROUGH OD PROFILE)
G00X1.Z.03
G71U.1R.015
**G71P1000Q1001U.01W.005F.007
N1000G00X.6794
G01Z-.0059F.02
X.784Z-.044
Z-.465
X.8072
G03X.8892Z-.506R.041
G01Z-.975
X.938
N1001X1.
G0Z1.

and the threading cycle too

(FINISH THREAD)
T0303
G97S1000M03
G00G99X1.Z.25M08
G0X.984Z.2
G76P011060Q0010R0010
**G76X.744Z-.4095R0P0200Q0047F.059
G00X.968Z.2577
G0Z1.


I am drowning.. please help
__________________

[timlkallam]

Just a shot in the dark whats the g99 on the lathe used for, could the alarm be because of the g99. The g99 is return to R level for fixed caned cycle . I have never seen a lathe that uses g99. Take out the g99 and see what happens reboot the machine sence g99 is modal.

The R in the g76 code needs a . point

[teamjnz]

Thanks for the input Tim.

G99 for the lathe is feed per revolution and G98 is feed inches per minute. These codes are different for the mill in the canned drilling cycles.

I was able to produce a G92 thread cycle. I am confused why this the G92 cycle works and the G76 does not. The thread relief is small and the G92 starts retracting to soon and doesn't give me full thread before the shoulder.

Any other input would be nice.

[ChattaMan]

I don't do turning but I seem to recall reading somewhere that older controls use just a single line input for G71/76.
Don't know the format for the block info but try a "search" for G71 single line input.

[ChattaMan]

O1000(Program number)
N1 G50 S2500(Max speed)
N2 T0101
N3G96 S600 M3(Speed in SFM for 1018 Steel)
N4 G0 X4.0 Z.1 M8(Rapid to OD of part, .1" away from face, turn coolant on)
N5 G71 U.15 R.02(U=cutting depth, R= pullaway distance after each cut)
N6 G71 P7 Q9 U.05 W.005 F.015(P7 tells the control to look at N7 and Q9 to look at N9, this is how we give the motions describing the part.
U is the amount of stock left for finishing on the OD, W is the amount left on the shoulder.
N7 G0 X2.0
N8 G1 Z-1.0
N9 X4.0
N10 G0 X6.0 Z6.0 M9(Rapid back to a position clear of the part, turn coolant off)
N11 M30( End of program)
Notes: The 6T version has a single line and so do various Yasnac controls, they look like this:
N5 G71 P7 Q9 U.05 W.005 D1500 F.015(D= depth of each pass and has to be given as a value
without a decimal point)
This cycle is normally followed by G70( Finish Cycle) after tool change to a finish tool. Rapid to the
same position for the start of the G71, then program G70 P7 Q9.

[dcoupar]

Whether your control uses 1-line or 2-lin multiple repetitive cycles depends on parameter TAPEF (see attached).

1=F10/F11 Format (1-line)
2=F0 Format (2-line)

[bullandbladder]

I've had this happen. The canned cycles need to be switched on by someone who knows where to look (I had a service engineer with me who had good contacts)

[CNCRim]

The alarm reads 010 P/S. My books says "unusable G code commanded" It bombs out when it reads the G71 line and the G76 line. I can work around the G71 rough cycle but I need to be able to thread the part.

Since "unusable G code" alarm, I have a feel the machine don't has option G71 to G76. Long hand program is only choice.

[SanDiegoCNC]

Hello,

Sorry I posted the original in the wrong forum

I am having troubles... I have been CNC turning parts for years. I buy a used small CNC lathe, 1998 Femco with a Fanuc O-T control. I score a small first job. Now I try and run the machine for the first time and it doesn't like the canned cycles.

Please help... Could it be the a turned off parameter??

The alarm reads 010 P/S. My books says "unusable G code commanded" It bombs out when it reads the G71 line and the G76 line. I can work around the G71 rough cycle but I need to be able to thread the part.

Here is the code
(ROUGH OD PROFILE)
G00 X1. Z.03

G71 P1000 Q1001 U.01 W.005 D0.03 F.007

N1000 G00 X.6794
G01 Z-.0059 F.02
X.784 Z-.044
Z-.465
X.8072
G03 X.8892 Z-.506 R.041
G01 Z-.975
X.938
N1001 X1.
G0 Z1.

and the threading cycle too

(FINISH THREAD)
T0303
G97S1000M03
G00G99X1.Z.25M08
G0X.984Z.2
G76P011060Q0010R0010
**G76X.744Z-.4095R0P0200Q0047F.059
G00X.968Z.2577
G0Z1.


I am drowning.. please help
__________________

Try single line G71 canned cycle.

G71 P1000 Q1001 U.01 W.005 D0.03 F.007

What kind of material are you cutting? And the OD tolerance? If its a critical part dimensionally speaking (tenths), I'd run at least two or more passes across the OD, cutting the same amount on each pass. This can be done when you call up the G70 and set your 'U' and 'W' values accordingly.

Example with 3 passes with the G71 U0.009 and W0.003:

G70 P1000 Q1001 U0.006 W0.002 F0.004
G70 P1000 Q1001 U0.003 W0.001
G70 P1000 Q1001 (final dimension, no need to use U or W)

I'll assume that you already know this bit of knowledge but I'll state it anyway for those who are reading this post and may not know... You can put several G70 lines below each other and the machine will not alarm out. This is because it will start at the G71 lap starting point (X1.0 Z0.03) when it reads each G70 line. Hence, no crash.


Now to the threading...

M24 (THREAD TAPER OUT OFF)
(M23 = THREAD TAPER OUT ON)
G76 X0.744 Z-0.4095 K0.000 D0.002 F0.059
(K = MAJOR DIA MINUS MIN DIA / 2)
(D = THREAD DEPTHS OF CUT)
(FEEDRATE = 1 / # OF THREADS)


Hope this helps you out. Let me know how it goes for you.

Patrick

[jamie0579]

Try single line G71 canned cycle.

G71 P1000 Q1001 U.01 W.005 D0.03 F.007

What kind of material are you cutting? And the OD tolerance? If its a critical part dimensionally speaking (tenths), I'd run at least two or more passes across the OD, cutting the same amount on each pass. This can be done when you call up the G70 and set your 'U' and 'W' values accordingly.

Example with 3 passes with the G71 U0.009 and W0.003:

G70 P1000 Q1001 U0.006 W0.002 F0.004
G70 P1000 Q1001 U0.003 W0.001
G70 P1000 Q1001 (final dimension, no need to use U or W)

I'll assume that you already know this bit of knowledge but I'll state it anyway for those who are reading this post and may not know... You can put several G70 lines below each other and the machine will not alarm out. This is because it will start at the G71 lap starting point (X1.0 Z0.03) when it reads each G70 line. Hence, no crash.


Now to the threading...

M24 (THREAD TAPER OUT OFF)
(M23 = THREAD TAPER OUT ON)
G76 X0.744 Z-0.4095 K0.000 D0.002 F0.059
(K = MAJOR DIA MINUS MIN DIA / 2)
(D = THREAD DEPTHS OF CUT)
(FEEDRATE = 1 / # OF THREADS)


Hope this helps you out. Let me know how it goes for you.

Patrick

jamie0579, simply switch off the tool nose radius compensation command after stock removal G40, then use G33 thread cutting command.Hope this was useful.

[jamie0579]

simply switch off your tool nose radius command ( G40 ), then use G33 thread cutting. G76 is a tapping code not threading you must use G33.Let me know if this was any help as i have encountered this myself,and redited the programme with G33.

[jamie0579]

You have too switsh off your tool nose radius compensation command, which is G40 and but also acctivate it at the beginning of your roughing cycle, which is G41, as for the treading cycle try using G33 thread cuttting this is a more stable thread cutting command as G76 is commonly used as a tapping command,please let me know if this was useful.

[SanDiegoCNC]

jamie0579, simply switch off the tool nose radius compensation command after stock removal G40, then use G33 thread cutting command.Hope this was useful.

??Huh??

[SanDiegoCNC]

simply switch off your tool nose radius command ( G40 ), then use G33 thread cutting. G76 is a tapping code not threading you must use G33.Let me know if this was any help as i have encountered this myself,and redited the programme with G33.

I'm sure you realize that, depending on the machine, G codes do vary. For instance, a G71 on most machines is a lap turning cycle. But on an Okuma, it is a threading cycle. Teamjnz's code used the G76 for threading. I used a different posting style of the same G76 code because he is using an older model lathe (1999). Please also notice the following...

M24 (THREAD TAPER OUT OFF)
(M23 = THREAD TAPER OUT ON)
G76 X0.744 Z-0.4095 K0.000 D0.002 F0.059
(K = MAJOR DIA MINUS MIN DIA / 2)
(D = THREAD DEPTHS OF CUT)
(FEEDRATE = 1 / # OF THREADS)

On a tapping cycle, I wouldn't call out a 'K' or 'D' value and I sure wouldn't start tapping in 'X0.744'.

Thanks.

[SanDiegoCNC]

Here's a real example program that has several different lap cycles going on in it. I wrote this program for a Haas SL10 (Model year 2005).

%
O00066 (DWG# TX-10309 REV. NA)
(1 OP)
(9/16 HEX HOUSING)
(MATERIAL: 9/16 HEX)
(CURRENT PROGRAM DATE: 7 FEB 2007)
(ORIGINAL PRG DATE: 7 FEB 2007)
(CYCLE TIME= 0 M 0 S)

(TOOLS LIST)
(TOOL 1 CNGP431 0.0156 RADIUS ROUGH TURN)
(TOOL 4 OD THREADING TOOL)
(TOOL 5 CNGP 43.0 RADIUS 0.007 FINISH TURN)
(TOOL 9 SPOT DRILL)
(TOOL 6 F DRILL 0.255 DIAMETER)
(TOOL 11 0.120 WIDE CUTOFF BLADE)
(TOOL 3 PART STOP)

G20
(EXTEND STOCK 2.210)
(TOOL - 1 OFFSET - 1)
G28 U0. W0. M05
G00 T101 (CNMG-431 0.0156 RADIUS)
G97 S1600 M03
G00 G54 X0.75 Z0.2
G50 S1600
G99 G00 X0.75 Z0.1
M08
G01 X0.75 Z0.1 F0.02
G71 P30 Q40 U0.004 W0.002 D0.02 F0.004
N30 G00 X-0.04
G01 X-0.04 Z0. F0.003
G01 X0.378 Z0.
G01 X0.438 Z-0.03 (CHAMFER ON THREAD FACE)
G01 X0.54 Z-0.6
G01 X0.75 Z-0.705 (CHAMFER ON HEX)
N40 G01 X0.75
G00 X0.75 Z0.05 M09
G28 U0. W0. M05
T100
M01
G28 U0. W0. M05
G00 T404 (OD THREAD TOOL)
(1/4 NPT X 0.6 OAL)

(CHECK THREAD AFTER FINISH TOOL)

G97 S800 M03
G00 G54 X0.54 Z0.2
G50 S800
G99 G00 X0.54 Z0.15
M08
G01 X0.54 Z0.1 F0.03
G92 X0.54 Z-0.55 I0.034 F0.0555 M24
(G92 IS MODAL THREAD CYCLE)
(X0.54 IS FIRST THREAD DIAMETER)
(Z IS THE THREAD LENGTH)
(I IS THE TAPER AMOUNT OVER THE LENGTH OF THREAD)
(F IS THE FEEDRATE)
(FEEDRATE = 1 / # OF THREADS)

(EACH OF THE FOLLOWING LINES IS ANOTHER DEPTH OF CUT)
X0.525
X0.53
X0.525
X0.52
X0.515
X0.51
X0.505
X0.5
X0.495
X0.49
X0.485
X0.48
X0.475
X0.47
X0.465
X0.46
X0.455
X0.45
X0.445
X0.44
X0.435 (FINAL THREAD DEPTH)
X0.435 (SPRING PASS ON FINAL THREAD)
G00 X0.54 Z1.
M09
G28 U0. W0. M05
T400
M01
G28 U0. W0. M05
G00 T505 (FINISH PASS 0.007 RADIUS)
G97 S1600 M03
G00 G54 X0.75 Z0.1
G50 S1600
G01 X0.75 Z0.05
M08
G70 P30 Q40 F0.004
M09
G00 X2. Z1. M09
G28 U0. W0. M05
T500
M00 (CHECK THREAD)
G28 U0. W0. M05
G00 T0909 (SPOT DRILL)
(NO COOLANT NEEDED)
G97 S1000 M03
G00 G54 X0. Z0.1
G50 S1000
G01 X0. Z-0.02 F.005
G00 X0. Z0.1
G00 X2. Z1.
G28 U0. W0. M05
T900
M01
G28 U0. W0. M05
G00 T0606 (F DRILL 0.255 DIAMETER)
G97 S800 M03
G00 G54 X0. Z0.1
G50 S800
M08
(G83 Peck Drill using I,J,K)
(I=Amount of First Peck Depth)
(J=Reduced Peck Depth Amount)
(K=Minimum Peck Depth Amount)
G83 X0. Z-1.5 I0.05 J0.05 K0.1 R0.1 F0.003
G00 X0. Z0.1
G00 X2. Z1. M09
G28 U0. W0. M05
T600
M01
G28 U0. W0. M05
T1111 (0.120 WIDE GROOVE/CUTOFF)
(TOUCH OFF ON LEADING EDGE)
(PROGRAM ADJUSTS FOR OAL)
(AN EXTRA 0.005 IS LEFT FOR 2ND OP)
G97 S900 M03
G00 G54 X0.75 Z1.
G50 S900
G01 X0.75 Z-1.47 F0.1
M08
G75 X0.52 I0.015 F0.001 (PECK ROUGH CUTOFF CYCLE)
G01 X0.75 Z-1.47 F0.04
G01 X0.75 Z-1.365
G01 X0.6 Z-1.47 F0.001 (REAR CHAMFER ON HEX)
G75 X0. I0.015 F0.001 (PECK FINAL CUTOFF CYCLE)
M09
G00 X2. Z1.
G28 U0. W0. M05
T1100
M01
G28 U0. W0. M05
G00 T0303 (STOCK STOP)
G00 G54 X1. Z0.1
G00 X0. Z0.06
M05
M00 (PULL STOCK)
G00 Z1.
G00 X2.
G28 U0. W0. M05
T300
M99
M30
%