G-Code Problem on my Fanuc Oi Hardinge Lathe

[Josh-PTP]

Hey guys,

I am having a little problem with a tool nose radius program on my lathe. The tools radius is .031" Here is the part of the program that is giving me problems. I keep getting a 041 alarm. Thanks for any help.......



N1
M98P1
T0101(80 DIAMOND TOOL RADIUS = .031 TOOLNOSE QUADRANT = 3))
G97S800M13
G00X1.4Z.0
G50S2500
G96S600
G99
G01G99X0.F.005
G00Z.1
G00X1.55Z.1
G42X1.45Z.05
G99
G71U.05R.015
G71P100Q200U.03W.01F.005
N100G0X1.0
G01G99Z0.F.005
X1.191,R.03
X1.375Z-.875
Z-1.0
X1.4
N200G0X1.45
G70P100Q200
M98P1



Thanks for any help........

[jorgehrr]

To turn compensation on, the machine must move at least the distance of the nose radius in X and Z. For easy calculations, back away from the start point 0.1 in Z and 0.2 in X.
To turn compensation off, we feed the cutter completely off the work and then make a move larger than the nose radius while calling G40.

Check your decimal points I see a (,) somewhere in there.

Cheers.

[g-codeguy]

Originally Posted by Josh-PTP Hey guys, I am having a little problem with a tool nose radius program on my lathe. The tools radius is .031" Here is the part of the program that is giving me problems. I keep getting a 041 alarm. Thanks for any help....... N1 M98P1 T0101(80 DIAMOND TOOL RADIUS = .031 TOOLNOSE QUADRANT = 3)) G97S800M13 G00X1.4Z.0 G50S2500 G96S600 G99 G01G99X0.F.005 G00Z.1 G00X1.55Z.1 G42X1.45Z.05 G99 G71U.05R.015 G71P100Q200U.03W.01F.005 N100G0X1.0 G01G99Z0.F.005 X1.191,R.03 X1.375Z-.875 Z-1.0 X1.4 N200G0X1.45 G70P100Q200 M98P1 Thanks for any help........

I have a couple questions. 1) Why are you even bothering to use tool nose radius compensation? 2) I see you are using Hardinge safe index programs, so why all the G99 codes? It is modal and should be in the safe index program.

If you got rid of the G42, you could shorten the program by a couple more blocks

[cogsman1]

I believe if you add a G40 on the N200 line it will run the way you have it written. During a canned cycle it will retract and tool comp doesn't like that.

[xyzer]

HMMMMM...our Fanucs won't use cutter comp in a canned cycle.

I see a couple of issues, Don't forget the tool type settings and tool radius in the geometry screen. It may be a tad longer but you can see the G42 install and cancel

G0X1.45Z.05
G71U.05R.015
G71P100Q200U.03W.01F.005
N100G0X1.0
G01Z0.
G1X1.137Z0.0
G03X1.1966Z-.0269R.03
"X1.191,R.03(WON'T WORK)" iF IT WAS AT 90 DEG IT WOULD NEED R-.03
G1X1.375Z-.875
Z-1.0
N200X1.45
G0X1.5Z.1
G42X1.45Z.05
G0X1.0
G01Z0.
G1X1.137
G03X1.1966Z-.0269R.03
G1X1.375Z-.875
Z-1.0
X1.45
G0G40X1.5Z.1

[tobyaxis]

Originally Posted by Josh-PTP Hey guys, I am having a little problem with a tool nose radius program on my lathe. The tools radius is .031" Here is the part of the program that is giving me problems. I keep getting a 041 alarm. Thanks for any help....... N1 M98P1 T0101(80 DIAMOND TOOL RADIUS = .031 TOOLNOSE QUADRANT = 3)) G97S800M13 G00X1.4Z.0 G50S2500 G96S600 G99 G01G99X0.F.005 G00Z.1 G00X1.55Z.1 G42X1.45Z.05 G99 G71U.05R.015 G71P100Q200U.03W.01F.005 N100G0X1.0 G01G99Z0.F.005 X1.191,R.03 X1.375Z-.875 Z-1.0 X1.4 N200G0X1.45 G70P100Q200 M98P1 Thanks for any help........

You need to set the TNR in the Tool Geometry Page and the Tool Tip Designation or your comp won't work. Setting the tool at least 2 times the radius away from the cutting point too.

Originally Posted by xyzer HMMMMM...our Fanucs won't use cutter comp in a canned cycle. I see a couple of issues, Don't forget the tool type settings and tool radius in the geometry screen. It may be a tad longer but you can see the G42 install and cancel G0X1.45Z.05 G71U.05R.015 G71P100Q200U.03W.01F.005 N100G0X1.0 G01Z0. G1X1.137Z0.0 G03X1.1966Z-.0269R.03 "X1.191,R.03(WON'T WORK)" iF IT WAS AT 90 DEG IT WOULD NEED R-.03 G1X1.375Z-.875 Z-1.0 N200X1.45 G0X1.5Z.1 G42X1.45Z.05 G0X1.0 G01Z0. G1X1.137 G03X1.1966Z-.0269R.03 G1X1.375Z-.875 Z-1.0 X1.45 G0G40X1.5Z.1

XYZer,

The reason your comp isn't working is one or both of these reasons.

1) Your using a control that is older than 1984.

2) You need to call the TNR Comp in the Canned Cycle or it won't work.

Here is an example:

%
O0086
G0 G40 G97 G99 T0 M5
G28 U0 W0 M9
G50 S2000 M41
M1

N1(REMOVE SKIN/R-FACE/TURN)
G28 U0 W0 T0
T101 M8
G96 S475 M3
G0 G42 X3.99 Z.3
G1 Z-1.3 F.01
X4.05 F.015
G0 G40 X4.1 Z.2
G72 P10 Q15 W.005 D400 F.008
N10 G0 G41 Z0
N15 G1 X0 F.004

G0 G40 X4.0 Z.1
G71 P20 Q25 U.02 W.002 D850 F.01
N20 G0 G42 X1.0
G1 Z0 F.0025
X1.325 F.003
G3 X1.375 Z-.025 R.025 F.0025
G1 Z-.75 F.004
X2.75 F.0035
X3.975 Z-.9141 F.0025
G1 Z-1.08 F.004
N25 X4.1 F.0035

G0 G40 Z.1 M9
G28 U0 W0
G97
T0
M1

N2(F-FACE/TURN/U-CUT)
G28 U0 W0 T0
T303 M8
G96 S650 M3
G0 G41 X1.5 Z0
G1 X0 F.004

G0 G40 X4.1 Z.1
G70 P20 Q25
G0 G40 Z.1

(U-CUT)
G1 X1.3755 Z-.725 F.05
Z-.755 F.004
G4 U1.0
G1 Z-.75 F.006
X2.8 F.003

G0 G40 Z.1 M9
G28 U0 W0 M5
G97
T0
M1

N3(DRILL)
G28 U0 W0 T0
T505 M8
G97 S400 M3
G0 X0 Z.25
G1 Z-2.25 F.0072
Z.05 F.2

G0 G40 Z.1 M9
G28 U0 W0
G97
T0
M1

N4(R-BORE )
G28 U0 W0 T0
T707 M8
G96 S400 M3
G0 G40 X.75 Z.1
G71 P40 Q45 U-.02 W.002 D320 F.0075
N40 G0 G41 X1.214
G1 X.814 Z-.1 F.003
Z-1.3 F.005
N45 X.75

G0 G40 Z.1 M9
G28 U0 W0
G97
T0
M1

N5(F-BORE)
G28 U0 W0 T0
T707 M8
G96 S550 M3
G0 G40 X.75 Z.1
G70 P40 Q45

G0 G40 Z.1 M9
G28 U0 W0
G97
T0

M30
%

BTW: Look at the notes in the Fanuc Manual. It will explain everything.

[xyzer]

Originally Posted by tobyaxis Look at the notes in the Fanuc Manual. It will explain everything.

tobyaxis

My problem was I learned on a pre 84 controller and hate reading the manual! Nice detail to know!

I still see somthing wrong with.
X1.191,R.03
X1.375Z-.875

Should be

G03X1.1966Z-.0269R.03
G1X1.375Z-.875

Or it is a new feature with the newer controllers?
I do know the alarm number can say one thing and the problem is something else!

Dave

[tobyaxis]

Originally Posted by xyzer tobyaxis My problem was I learned on a pre 84 controller and hate reading the manual! Nice detail to know! I still see somthing wrong with. X1.191,R.03 X1.375Z-.875 Should be G03X1.1966Z-.0269R.03 G1X1.375Z-.875 Or it is a new feature with the newer controllers? I do know the alarm number can say one thing and the problem is something else! Dave

Some of the Controlers might do this while others won't. It all really depends on the Machine Tool Builder and what they specified as options with their machine.

You might want to call Fanuc, or your machine builder. There could be a Parameter setting that needs to be changed.

[adamant]

try it like this

N1
M98P1
T0101(80 DIAMOND TOOL RADIUS = .031 TOOLNOSE QUADRANT = 3))
G97S800M13
G00X1.55Z.1
G71U.05R.015
G71P100Q200U.03W.01F.005
N100G0G42X1.0
G01Z0.F.005
X1.191,R.03
X1.375Z-.875
Z-1.0
X1.4
N200G0G40Z.1
G70P100Q200
M98P1


It helps to get rid of the junk.

[adamant]

Originally Posted by xyzer tobyaxis My problem was I learned on a pre 84 controller and hate reading the manual! Nice detail to know! I still see somthing wrong with. X1.191,R.03 X1.375Z-.875 Should be G03X1.1966Z-.0269R.03 G1X1.375Z-.875 Or it is a new feature with the newer controllers? I do know the alarm number can say one thing and the problem is something else! Dave

The ,R is correct for his control.

It is used for "blueprint programming"

,A for angle

,C for chamfer.

,R for radius.


Oh yeah and I looked at my P1 program for safe indexing and it had G40 and G99 in it........course I wrote it a long time ago and could not remember what all it had in it.

Anyhows the last line in the G71 cycle should be GOZ.1 instead of an X dim.

[xyzer]

Originally Posted by adamant try it like this X1.191,R.03

I had to load the program in a newer controller to see if it really worked. My controller doesn't like the "," in the line. alarms 053 I think it was "to many charactures in line"?! I found the "GOZ.1 instead of an X dim".

[tobyaxis]

Originally Posted by adamant The ,R is correct for his control. It is used for "blueprint programming" ,A for angle ,C for chamfer. ,R for radius. Oh yeah and I looked at my P1 program for safe indexing and it had G40 and G99 in it........course I wrote it a long time ago and could not remember what all it had in it. Anyhows the last line in the G71 cycle should be GOZ.1 instead of an X dim.

Don't forget "I+-" and "K+-" for Chamfer Quadrants in 6T Controls.