[jorgehrr]

Hello every one -

I never used these G codes G70 and G71.

I'm running out of memory in my machine. I need to rewrite some jobs and can cycles are the answer. I am familiar with can cycles except this one.

Can someone describe each step of them??

Thank you all:

cheers:

[cdlenterprises]

On a Haas control, G71 is a canned cycle to rough an O.D. or I.D. contour (as opposed to G72 which is a facing cycle). G70 is a finishing cycle that can be called after a G71, G72, or G73 cycle to finish the respective profile. While I've never used them personally, basically you would write the code for the finish profile and then use the canned cycle parameters to dictate depth of cut, feedrate, # of passes, etc. Hope this helps. :cheers:

[jorgehrr]

Thank you

It did.

[Geof]

One thing to watch with these canned cycles is how they deal with tool nose compensation. On the Haas tool compensation is ignored when G71 is active, I don't know about other machines

[jorgehrr]

I'll keep that in mind

thank you

[positiverake]

What control do you have? this is for a two line format, this will turn a 3.0 dia down to 1.0 dia and back 2.0, simple exe.

N1(R.TURN)
G50S2500M8
G0T0101
G96S350M3
G54
X2.1Z.1
Z.01
G1X-.06F.008
G0Z.05
X2.
G71U.1R.02
G71P100Q200U.04W.005F.01
N100G0X1.
G1Z-2.F.006
N200X2.
G0X8.Z6.
M1

N3(F.TURN)
G50S3000M8
G0T0303
G96S500M3
G54
X1.1Z.1
Z0
G1X-.03F.006
G0Z.05
X2.
G70P100Q200
G0X8.Z6.
M30

FIRST G71 LINE:
G71=INSTATES ROUGHING CYCLE(PARAMERTER LINE)
U=DEPTH OF CUT ON A SIDE
R=AMOUNT OF PULL OFF FOR EACH PASS

SECOND G71 LINE:
G71=INSTATES ROUGING CYCLE
P=N NUMBER FOR START OF PROFILE,CAN BE ANY NUMBER,JUST MAKE SURE NOT TO HAVE THE SAME NUMBER SOMEWARE ELSE IN THE PROGRAM!
Q=N NUMBER FOR END OF PROFILE (SAME LIMITS AS ABOVE)
U=AMOUNT OF FINISHING STOCK TO BE LEFT ON X DIA.
W= AMOUNT OF FINISHING STOCK TO BE LEFT ON Z.
F=FEED

G70 LINE:
G70=INSTATES THE FINISHING CYCLE
P=N NUMBER START OF PROFILE TO FINISH
Q=N NUMBER END OF PROFILE TO FINISH
L= SOME CONTROLS USE THIS FOR REPEATING THE FINISH CYCLE,L1 WILL RUN 1 TIME, L2 WILL RUN 2 TIMES ECT.. IF YOU LEAVE IT OUT IT WILL RUN ONE TIME.

IN THIS EXE. I FACED THE PART FIRST(PERSONAL PREFRENCE)
WITH THE G70 CYCLE, IT IS IMPORTANT TO START THE CYCLE AT THE SAME PLACE AS THE G71 CYCLE STARTS BECUSE THATS WERE THE MACHINE WILL GO AFTER THE CYCLE.

THESE ARE GREAT MULITIPLE REPETITIVE CYCLES, I USE THEM ALL THE TIME
IF YOU USE THEM FOR BORING,EVERY THING IS THE SAME EXCEPT THE THE U VAULE FOR FINISHING STOCK IS NEGATIVE (U-.04)

HOPE THIS HELPS, YOU CAN E-MAIL ME IF YOU NEED T0.

[jackson]

or if your like me i use one tool to rough and finish
N2000
(CNMG 430)
G0G54T101
G50S4000
G96S800M3
X2.6Z0M8
G1X0F.004
G0X2.5Z.1
G71U.1R.025
G71P1Q2U.02W.002F.016
N1G0X1.28
S800
G1Z.001F.02
G1X2.313Z-.2086
Z-.5F.004
N2X2.5
G0Z.1
G70P1Q2
G0Z5.M9
M1

[jorgehrr]

Thank you all

I am on my way

:cheers:

[tobyaxis]

You guys forgot this Format for G71, G72, and G73.

N1
G0G20G40G90G97G99M5
G28U0V0W0B0M9
G50S2000M41
M1
N1(R-F/T CNMG432)
G28U0V0W0B0T0100
T0101M8
G96S250M3
G0X1.05Z0.1
G72P10Q15W.003D400F.008
N10G0G41Z0
N15G1X0F.004

G0G40X1.05Z.1
G71P20Q25U.006W.003D700F.015
N20G0G42X0.
G01Z0. F.005
X0.4375
X0.5625
Z-0.37
G02X0.6875Z-0.495R0.125
G01X0.7403
X0.8125Z-0.62
Z-1.425
N25X1.05

G0G40G97Z.1M9
G28U0V0W0B0T0100
M1


Call your cutter comp in the Canned Cycle and Cancel it at the end Sequence Block.

The D in the above Canned Cycle = Depth of Cut Radially.

:rainfro:

[jackson]

You guys forgot this Format for G71, G72, and G73.

N1
G0G20G40G90G97G99M5
G28U0V0W0B0M9
G50S2000M41
M1
N1(R-F/T CNMG432)
G28U0V0W0B0T0100
T0101M8
G96S250M3
G0X1.05Z0.1
G72P10Q15W.003D400F.008
N10G0G41Z0
N15G1X0F.004

G0G40X1.05Z.1
G71P20Q25U.006W.003D700F.015
N20G0G42X0.
G01Z0. F.005
X0.4375
X0.5625
Z-0.37
G02X0.6875Z-0.495R0.125
G01X0.7403
X0.8125Z-0.62
Z-1.425
N25X1.05

G0G40G97Z.1M9
G28U0V0W0B0T0100
M1


Call your cutter comp in the Canned Cycle and Cancel it at the end Sequence Block.

The D in the above Canned Cycle = Depth of Cut Radially.

:rainfro:

Yeah i only have one machine that is set up for one line read
the rest are two most your newer fanucs are set to use two lines you can change that i belive but im just use to it

[tobyaxis]

Yeah i only have one machine that is set up for one line read
the rest are two most your newer fanucs are set to use two lines you can change that i belive but im just use to it

Personally I prefer the two line. It allows you to adjust the Return Amount. Like when you don't have the right size Boring Bar for a very small bore.
:rainfro:

[jackson]

Personally I prefer the two line. It allows you to adjust the Return Amount. Like when you don't have the right size Boring Bar for a very small bore.
:rainfro:

Ha Ha yeah i do that alot

[tobyaxis]

Ha Ha yeah i do that alot

It's nice to have options that Conversational Controls Don't, LOL.

[jackson]

I wouldnt know never had a machine or worked on a machine with conversational, but i know a few guys that call themselfs programmers because of conversatinal,

[tobyaxis]

I wouldnt know never had a machine or worked on a machine with conversational, but i know a few guys that call themselfs programmers because of conversatinal,

Yea, that is a good one. I'll save that for the Machinists Group Meeting, LOL.:rainfro:

I'd like to see this Programmed in Conversational

[jackson]

Oh, well dont you know some where out there there is some one that will try and sell that they can do it LMFAO!!!!!

[pbal]

I have two weeks experiance in cnc programming. I am writing a program to;
drill two holes 17/32 thru with a counter bore .625 deep with a .750 dia;
I am making jaws that are 1X2x6, for use on a, and run the program, on a
haas verticle mini-mill. I also need to use G81 for this, or canned cycles. here is what I've come up with so for, please, if anyone could check my program and show me errors and correct program for this. I need to use a address code Q and L if it can use them, and a P for counter bore in program. Thanks.PBal
%
T1 M6 (17/32 center drill two holes)
G90 G54 G00 X1.062 Y.941
S1438 M03
G43 H01 Z0.1 M08
G81 G99 Z-1.3 R0.1 F9
X4.94
G80 G00 Z1.0 M09
G28 G91 Z0.0 M05
T2 M6 (0750 Counter bore w/t dwell)
G90 G54 G00 X1.062 Y.941
S1273 M03
G43 H02 Z1.0 M08
G81 G99 Z-.625 R0.1 F15
X4.94

[jackson]

%
T1 M6 (17/32 center drill two holes)
G90 G54 G00 X1.062 Y.941
S1438 M03
G43 H01 Z0.1 M08
G81 G99 Z-1.3 R0.1 F9
X4.94
G80 G00 Z1.0 M09
G28 G91 Z0.0 M05
T2 M6 (0750 Counter bore w/t dwell)
G90 G54 G00 X1.062 Y.941
S1273 M03
G43 H02 Z1.0 M08
G81 G99 Z-.625 R0.1 F15
X4.94

%
O00001(part #)
(this is were i put my setup info)

N1
(17/32 C.DRILL)
T1 M6
G90 G54 G00 X1.062 Y.941 S1438 M3
G43 H01 Z0.1 M08
G81 G98 Z-1.3 R0.1 F9 (NOW YOU CAN USE G83 WICH WITH THE R AND Q VALUE WILL RETRACT TO THE TOP OF THE PART TO CLEAR CHIPS THE Q IS HOW DEEP IT CUTS BEFORE IT PECKS.G73 IS THE SAME BUT IT IS A HISPEED PECK)
X4.94
G80 G00 Z1.0 M09
G28 G91 Z0.0

N2
(.75 C.BORE)
T2 M6
G90 G54 G00 X1.062 Y.941 S1273 M3
G43 H02 Z1.0 M08
G81 G99 Z-.625 R0.1 F15(SAME AS ABOVE)
X4.94
G80 G0 Z1.M9
G91 G28 Y0Z0
M30
%

What material are you running, are you using carbid tools.

[pbal]

thanks jackson, i am running carbide, sorry my error, stock is aluminum.

[jackson]

well you need to get your RPMS higher for the 17/31 i would say S3594 F14.
on the c.bore S2544 not sure of feed not sure what tool your using