Need help understanding a program Fanuc 6t on a Mazak lathe

[mgb1974]

I am trying to write a post for a Mazak Lathe with a Fanuc 6t controller. I do not have much experiance with CNC lathes(mostly all mill). Here is the example program:

%
:0001
( PLAN#9020 OP#20 )
N002 G20
N004 G50 X-50000 Z225000
N006 G00 T0101
N008 G97 S0100 M41
N010 M03
N012 G00 X12.098 Z6.
N014 Z4.134 M08
N016 G50 S0175
N018 G96 S0100
N020 G99
N040 G01 X12.8086 F.006
N050 G02 X12.8666 Z4.1621 I0. K.029
N060 G01 X12.8834 Z4.434
N070 G00X12.0834
N080 X12.298 Z4.234
N090 G01 Z3.672
N100 G00 X11.498 M09
N110 Z6.
N200 G97 S0100
N202 G00 X-50000 Z225000
N204 G00 T0100
N206 M01
N208 G50 X-50000 Z225000
N210 G00T0101
N212 G97S0100M41
N214 M03
N216 G00 X8.878 Z6.
N218 Z.589 M08
N220G50S0175
N222G96S0100
N230G01X9.504F.006
N240G00X9.004Z.689
N250X9.078
N260G01Z-.031
N270G00X8.878M09
N280Z6.
N300G97S0100
N302G00X-50000Z225000
N304G00T0100
N306M01
N308G50X-50000Z225000
N310G00T0202
N312G97S0100M41
N314M03
N316G00X11.91Z6.
N318Z3.678M08
N320G50S0175
N322G96S0100
N324G01X12.8498F.004
N330X12.8194Z3.5648
N340X12.7696Z3.4478
N350X12.7052Z3.3301
N360X12.5446Z3.0832
N370X12.4828Z2.9899
N380G03X12.4048Z2.9414I-.0674K.0143
N390G01X12.3066Z2.9192
N400X12.1494Z2.6972
N410X12.0728Z2.5976
N420G03X11.6202Z2.1219I-4.0267K1.624
N430X10.5136Z1.4405I-2.57K1.5216
N440G01X10.3584Z1.3688
N450G02X9.5335Z.8261I2.0677K-1.9995
N460G01X9.4362Z.7362
N470X9.4056Z.7057
N480X9.3838Z.683
N490 G00 X8.7838 M09
N500 Z6.
N600 G97 S0100
N602 G00 X-50000 Z225000
N604 G00 T0200
N606 M30
%

-First off anybody have the M and G code list for this controller/lathe?

-Second whats the deal with N004,N202 and so on i see that in every program and through out this one?

-3, whats line N006 T0101? is that tool one?

I am sure I will have more question but this is the basics.

thanks

[beege]

No list of G and M codes for the 6T here.

N006 ? An "Nword is just a line number, and depending on the age of the machine, may not be required, but then it may.

T0101 - Tool position 1, offset #1

Any specific questions about the codes listed in this program?

[mgb1974]

I meant what N006 line means? the X-50000 Z225000

[dcoupar]

N004 G50 X-50000 Z225000 - zero preset command.

Usually the distance from the part zero to the tool tip (when X and Z are home). Note that there's a matching G00 X-50000 Z225000 at the end of each tool. My guess is these were generic numbers that got edited (in pairs) each time the job was run.

The operator would touch each tool off the OD, add the X machine position to the the diameter of the part and record that value, touch off the face, record the Z machine position, then edit the G50 and matching G00 block to the new numbers.

[vipansam]

yes i have got G code list for 6T but M codes are machine manufactuers special expect some M codes like M3 (sp. cw), M4( sp. ccw), M1(op. stop), M0(op. stop w/o condition), m2(prog. stop), M30(prog. stop), m8(coolant start), m9(coolant stop) .
2. In N4 this is coordinate setting for offsets.
3. T0101 is tool no. 1 with its offset no 1 .
vipan katyal

[mgb1974]

Originally Posted by vipansam yes i have got G code list for 6T but M codes are machine manufactuers special expect some M codes like M3 (sp. cw), M4( sp. ccw), M1(op. stop), M0(op. stop w/o condition), m2(prog. stop), M30(prog. stop), m8(coolant start), m9(coolant stop) . 2. In N4 this is coordinate setting for offsets. 3. T0101 is tool no. 1 with its offset no 1 . vipan katyal

Vipan,
Is it possible to attach that here or list them here?

Its a Mazak lathe if you have the M codes by chance?

thanks!

[Dan Fritz]

Fanuc 6T G-codes:

G00 Positioning (rapid traverse)
G01 Linear interpolation
G02 Circular interpolation CW
G03 Circular interpolation CCW
G04 Dwell
G10 Offset value setting
G20 Inch data input
G21 Metric data input
G22 Stored stroke limit ON
G23 Stored stroke limit OFF
G27 Reference point return check
G28 Return to reference point
G29 Return from reference point
G30 Return to 2nd reference point
G31 Skip cutting
G32 Thread cutting
G34 Variable lead thread cutting
G36 Automatic tool compensation X
G37 Automatic tool compensation Z
G40 Tool nose radius compensation cancel
G41 Tool nose radius compensation left
G42 Tool nose radius compensation right
G50 Programming of absolute zero point (G50 X---- Y---- Z----)
(also used for Maximum spindle speed setting (G50 S----)
G65 User macro simple caling
G66 User macro modal calling
G67 User macro modal call cancellation
G68 Mirror image for double turrets ON
G69 Mirror image for double turrets OFF
G70 Finishing cycle
G71 Stock removal in turning
G72 Stock removal in facing
G73 Pattern repeating
G74 Peck drilling in Z axis
G75 Grooving in X axis
G76 Thread cutting cycle
G90 Cutting cycle A
G92 Thread cutting cycle
G94 Cutting cycle B
G96 Constant surface speed control
G97 Constant surface speed control cancel
G98 Per minute feed
G99 Per revolution feed


Standard EIA M-codes (your machine tool builder may not use some of these)

M00 Program Stop
M01 Optional (Planned) Stop
M02 End of Program
M03 Spindle CW
M04 Spindle CCW
M05 Spindle OFF
M06 Tool Change
M07 Coolant No. 2 ON
M08 Coolant No. 1 ON
M09 Coolant OFF
M10 Clamp
M11 Unclamp
M12 Unassigned
M13 Spindle CW & Coolant ON
M14 Spindle CCW & Coolant ON
M15 Motion +
M16 Motion -
M17 Unassigned
M18 Unassigned
M19 Oriented Spindle Stop
M20-29 Permanently Unassigned
M30 End of Tape
M31 Interlock Bypass
M32-35 Unassigned
M36-39 Permanently Unassigned
M40-45 Gear Changes if Used, Otherwise Unassigned
M46-47 Unassigned
M48 Cancel M49
M49 Bypass Override
M50-89 Unassigned
M90-99 Reserved for User

[CarbideBob]

Interesting programming method.
Mixed decimal and least increment (no decimal point) programming. I hate it when people do this. Some controllers force it for certain instructions though.

G50 is just like G92 for a mill. Have you used G92 on mill?
On a lathe you call up the tool and offset at the same time.
T0101 is like T01 H01 D01 on a mill.
T0100 is tool number one with no offsets. Note that they call this before returning to home.
Bob

[mgb1974]

Thanks for all the help guys. The other programmer isnt to good and isnt willing to help so I am stuck to figure it out on my own.

Let me make sure I understand this, Line N004 G50 x-50000 z225000 is the zero point of the program. This would be -5.0Inches in X and z is 22.5inches(radius??). T
Then on line N202 it is rapiding back to the zero point set at line N004?
Can I just use decimal instead of mixing incremental and decimal?

Thanks again!

[g-codeguy]

Originally Posted by mgb1974 Can I just use decimal instead of mixing incremental and decimal?!

I would think so, but am not positive. Try it on the first tool. See if it works. Keep rapid feedrate down and check distance to go. Hand on feedhold. I started on old Warner & Swaseys. No decimals were allowed.

Newer machines allow you to program either way. At least ours do tho I don't understand why anyone would want to. Much easier for everyone to understand with the decimal.

EDIT: What does your manual say about the G50 block?

[Dan Fritz]

The Fanuc 6T can take decimal point formatted numbers or "trailing zero" numbers with no decimal points. It won't matter at all. Just remember that when you are in INCH mode (G20), you must put 4 digits after the "imaginary" decimal point. When you are in METRIC mode (G21), you only put 3 digits after the imaginary decimal.

1.0000 or 1.0 or 1. or 10000 = 1 inch (in G20)
1.000 or 1.0 or 1. or 1000 = 1 mm (in G21)

[mgb1974]

What is the point of these lines? Is it just a tool change? Dont get why he is turning off constant surface speed and then going to referance point then calling out a referance point again and turning Constant surface speed off again.

Can this be simplified?


N300 G97 S0100
N302 G00 X-50000 Z225000
N304 G00 T0100
N306 M01
N308 G50 X-50000 Z225000
N310 G00 T0202
N312 G97 S0100 M41
N314 M03