[cncozz]

Hello all,

I was wonder if anyone can help me with the problems I am having. I am trying to put a champfer on the id of this part and I keep get the error code 052 CODE IS NOT G01 AFTER CHF/CNR. The machine is a hardgine conquest and the fanuc is series 18-T. I have tried G1 command after the ,c command and still got the same error. So here is the code i'm using. Any response is greatly appreciated. Thanks!

N09(ROUGH & FINISH BORING)
G97S500M13
M98P1
T0909
X5.950Z.200
G50S1000
G96S800
G1G41X6.000Z.050F100.
G99
G71U.015R.025
G71P200Q250U-.008W.005F.008
N200G0X6.150
N210G1G99Z-1.225F.005
N220X6.250
N230X6.150,C.070
N240Z-.100
N250G1X6.000
G70P200Q250
M98P2
M01
M30

[jorgehrr]

N220X6.250
N230X6.150,C.070
N240Z-.100

I see a (,) before C, also try C-.070 instead.

Cheers

[cncozz]

N220X6.250
N230X6.150,C.070
N240Z-.100

I see a (,) before C, also try C-.070 instead.

Cheers

I tried this and got the same error. Thanks for trying

[cnc-king]

Hello all,

I was wonder if anyone can help me with the problems I am having. I am trying to put a champfer on the id of this part and I keep get the error code 052 CODE IS NOT G01 AFTER CHF/CNR. The machine is a hardgine conquest and the fanuc is series 18-T. I have tried G1 command after the ,c command and still got the same error. So here is the code i'm using. Any response is greatly appreciated. Thanks!

N09(ROUGH & FINISH BORING)
G97S500M13
M98P1
T0909
X5.950Z.200
G50S1000
G96S800
G1G41X6.000Z.050F100.
G99
G71U.015R.025
G71P200Q250U-.008W.005F.008
N200G0X6.150
N210G1G99Z-1.225F.005
N220X6.250
N230X6.150,C.070
N240Z-.100
N250G1X6.000
G70P200Q250
M98P2
M01
M30

your problem seems to be the G41 before the rgh cycle if i can remember correctly you have to activate cutter comp before the finish cycle which is your g70 also you never turned cutter comp off.

[extanker59]

OK, I haven't programmed this way in years but here's my 2 cents.
Try this:

T0909
X5.950Z.200
G50S1000
G96S800
G1X6.000Z.050F100.
G99
G71U.015R.025
G71P200Q250U-.008W.005F.008
N200G0X6.2
N210G1G41X6.25 Z.025F.01
N220Z-1.225F.005
N230X6.150 C.070
N240Z-1.325
N250G1G40X6.000
G70P200Q250
M98P2
M01
M30

I hope I'm recalling it correctly. I think you have to use cutter comp in the body, not before? You also have to cancel in the body too. I've not done the C.070 before, so no clue. Let us know what works. Now I'm curious.
Chris

[cnc-king]

hardinge lathes with fanuc control requires the , before the R A or C value
eg ,R ,C ,A

if you prefer not to use them then you have to program the chamfer radius etc.

eg CHAMFER .005

G1G42 Z0 F.005
X.5
X.51 Z-.005
Z-1.
STUFF

G40 ***


RADIUS .005

G1G42 Z0 F.005
X.5
G3 X.51 Z-.005 R.005
Z-1.
STUFF

G40 ***

the rgh canned cycle does not the cutter comp

[dcoupar]

Does your Hardinge have a C axis? My Fanuc 18T manual says use I or K if your machine has a C axis. If not, check Prm 3405 bit 4.

[cncozz]

hey! Thanks for everyones help and input. I found a code a used for a prototype awhile and just used that code. So here it is. This code works! Thanks again everyone!


N09(ROUGH & FINISH BORING)
G97S500M13
M98P1
T0909
X5.950Z.200
G50S1200
G96S800
G1G41X5.950Z.050F100.
G99
G71U.150R.025
G71P200Q240U-.015W.005F.012
N200G0X6.500
N210G1G99Z0.F.006
N220X6.150,C.60
N230Z-1.220
N240X5.950
G70P200Q240
M98P2
M01
M30
%

[cogsman1]

Glad you got through it. What I see is that the line following the ",C" was not in the direction to allow the machine to calculate the end point of the chamfer so you got an alarm. That is why the "Prototype" code worked for you.

[CNCRim]

6.225-6.125=.1 and you chamfer is .07*2=.14. That's is why you get an alarm. the max for that chamfer you can put is .1, which is .05

Addition, you Z depth N240 not depth enough.

[g-codeguy]

Have to say the program in your first post made no sense to me. Your last one does. I will say tho that G99 is modal. No need for the second one. Actually the G99 may be in the P1 program. Can't remember if Hardinge put it in their example, but I have it in ours. That way I never need a G99 in the program. I then program G98 for the very few times it gets used.

I like the Hardinge Safe Index Programs, and use them on other brands of lathes if they can run that way. Being lazy, I've made a couple minor changes.

I loaded the Safe Index programs in the 9001-9004 M-code calls so that 1) operators can't make changes to them, or accidentally delete them, and 2) so that I need only type M91-M94 to replace the M98P1 thru M98P4 calls. Hey...it saves 4 keystrokes on every operation!

I didn't originally put the P999 program in a 9000 protected program so that the setup man could make the necessary changes to the 'X' & 'Z' home positions. This was before I learned how to use variables. I've left it that way since everyone is already use to it, but would put it in a protected program and use variables for the home positions if I were starting over again.

I also have my Barstop operation loaded as P9010 for calling with a G-code. So

N100G200 (Barstop)
M1

is my barstop operation in the program.

My cut-off operation is

N800G222 (CUT-OFF)
M30

I assign all the program variables in the 100 series variables at the beginning of the program.

I also have master programs for families of parts. The lathe operators are being forced to learn. Can't say the same for the milling ones. I don't program for them.

The one older foreman complains every time I do something new, but he soon learns, and usually will admit what I've done does make it easier for him and the guys on the floor. Saves me some work. They may not know where to change the feedrate for the cut-off tool in a normal program, but when I have

#104=.002 (FEEDRATE)

most can understand that. Especially if I explain it to them every week or two.

Sorry I got carried away. Seems like one thing led to another.

[magnamannan]

hi somebody can explain me how can i use the canned cycles? (I use an okuma lathe U10 control) thanks.

[g-codeguy]

hi somebody can explain me how can i use the canned cycles? (I use an okuma lathe U10 control) thanks.

I would ask on the Okuma forum.