[Asheen]

Hi,

I just bought a leadwell ltc 10ap cnc lathe. It uses fanuc series ot control. I am still learning how to use it. I am having a problem with the tool offsets when i am boring. the roughing cut works fine. I programmed it to leave 0.1mm on the face for finishing and 1mm on the diameter. I have measured after roughing. the size is right. The final cut bores 2mm bigger than the size in the program and cuts 0.4mm past the final length. if i dont use tool compensation it cuts the correct size. but it does not chamfer the edges. Where am i going wrong?

[machinehop5]

Sounds like tool position not set correctly.
CNC Lathe Tool Nose Radius Compensation - CNC Training Centre

[Asheen]

Sounds like tool position not set correctly.
CNC Lathe Tool Nose Radius Compensation - CNC Training Centre

I watched the video in the link above. I changed the tool tip number to 2. And the radius value to 0.4mm. I did this on the geometry screen and the wear screen. But it is still not working. It is still doing the same thing on the last cut

[Superman]

Put up your code...
...my guess is you are using the wrong g-code for inside turning
rear turret OD tool = G42
rear turret ID tool = G41
front turret OD tool = G41
Radius is the nose radius of the tip... tool tip number is different for ID vs OD

[Asheen]

Put up your code...
...my guess is you are using the wrong g-code for inside turning
rear turret OD tool = G42
rear turret ID tool = G41
front turret OD tool = G41
Radius is the nose radius of the tip... tool tip number is different for ID vs OD

%
O0000
(PROGRAM NAME - 77B0044)
(DATE=DD-MM-YY - 04-04-19 TIME=HH:MM - 17:26)
(MCX FILE - C:\USERS\USER\DOWNLOADS\77B0044.MCAM)
(NC FILE - C:\USERS\USER\DOCUMENTS\MY MCAM2018\LATHE\NC\77B0044.NC)
(MATERIAL - MILD STEEL MM - 2024)
(TOOL - 6 OFFSET - 6)
(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG 12 04 04)
G28 U0. V0. W0.
T0606
G0 X52. Z1. M8
G50 S2500
G96 S200 M03
G72 W1. R.5
G72 P100 Q110 U0. W.2 F.25
N100 G0 G41 Z0. S200
G1 X0.
N110 G40 Z1.
G0 X52.
G0 X52. Z1.2
G71 U1. R.5
G71 P120 Q130 U1. W.2 F.25
N120 G0 G42 X46. S275
G1 Z-.094
G3 X47. Z-.9 R.9
G1 Z-42.5
N130 G40 X52.
G0 Z1.2
M9
G28 U0. V0. W0. M05
T0600
M01
(TOOL - 7 OFFSET - 7)
(OD RIGHT 55 DEG INSERT - DNMG 15 06 04)
G28 U0. V0. W0.
T0707
G0 X52. Z1. M8
G50 S2500
G96 S200 M03
G70 P100 Q110
G0 X52.
Z1.2
G70 P120 Q130
G0 Z1.2
M9
G28 U0. V0. W0. M05
T0700
M01
(TOOL - 2 OFFSET - 2)
(DRILL 20. DIA.)
G28 U0. V0. W0.
T0202
G97 S1313 M03
G0 X0. Z5. M8
Z2.
G1 Z-51.009 F.25
G0 Z5.
M9
G28 U0. V0. W0. M05
T0200
M01
(TOOL - 11 OFFSET - 11)
(ID ROUGH MIN. 20. DIA. - 80 DEG. INSERT - CCMT 09 T3 04)
G28 U0. V0. W0.
T1111
G0 X18. Z1.25 M8
G50 S2500
G96 S200 M03
Z1.
G71 U1. R.5
G71 P140 Q150 U-1. W.2 F.2
N140 G0 G41 X36. S200
G1 Z-.094
G2 X35. Z-.9 R.9
G1 Z-15.
X31.055
G2 X29.379 Z-15.572 R.9
N150 G1 G40 X18.
G0 Z1.
Z1.25
M9
G28 U0. V0. W0. M05
T1100
M01
(TOOL - 9 OFFSET - 9)
(ID FINISH MIN. 20. DIA. - 55 DEG. INSERT - DCMT 11 T3 04)
G28 U0. V0. W0.
T0909
G0 X18. Z1.25 M8
G50 S2500
G96 S200 M03
Z1.
G70 P140 Q150 F.1
G0 Z1.
Z1.25
M9
G28 U0. V0. W0. M05
T0900
M30
%

[machinehop5]

Is this handwritten Program or CAM post Processor genarated G Code?

[Asheen]

Is this handwritten Program or CAM post Processor genarated G Code?

I used mastercam to generate the code. Then I punch it manually into the machine

[machinehop5]

%
O0000
(PROGRAM NAME - 77B0044)
(DATE=DD-MM-YY - 04-04-19 TIME=HH:MM - 17:26)
(MCX FILE - C:\USERS\USER\DOWNLOADS\77B0044.MCAM)
(NC FILE - C:\USERS\USER\DOCUMENTS\MY MCAM2018\LATHE\NC\77B0044.NC)
(MATERIAL - MILD STEEL MM - 2024)
N10 G21
(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG 12 04 04)
N20 G28 U0. V0. W0.
N30 G50 X250. Y0. Z250.
N40 G0 T0101
N50 G18
N60 G97 S1683 M03
N70 G0 X52. Z1. M8
N80 G50 S2500
N90 G96 S200
N100 G72 W1. R.5
N110 G72 P100 Q110 U0. W.2 F.25
N120 N10 G0 G41 Z0. S200
N130 G1 X0.
N140 N20 G40 Z1.
N150 G0 X52.
N160 G0 X52. Z1.2
N170 G71 U1. R.5
N180 G71 P120 Q130 U1. W.2 F.25
N190 N30 G0 G42 X46. S275
N200 G1 Z-.094
N210 G3 X47. Z-.9 R.9
N220 G1 Z-42.5
N230 N40 G40 X52.
N240 G0 Z1.2
N250 M9
N260 G28 U0. V0. W0. M05
N270 T0100
N280 M01
(TOOL - 12 OFFSET - 12)
(OD RIGHT 55 DEG INSERT - DNMG 15 06 04)
N290 G28 U0. V0. W0.
N300 G50 X250. Y0. Z250.
N310 G0 T1212
N320 G18
N330 G97 S2500 M03
N340 G0 X52. Z1. M8
N350 G50 S2500
N360 G96 S200
N370 G70 P100 Q110
N380 G0 X52.
N390 Z1.2
N400 G70 P120 Q130
N410 G0 Z1.2
N420 M9
N430 G28 U0. V0. W0. M05
N440 T1200
N450 M01
(TOOL - 126 OFFSET - 126)
(DRILL 20. DIA.)
N460 G28 U0. V0. W0.
N470 G50 X250. Y0. Z250.
N480 G0 T12726
N490 G18
N500 G97 S1313 M03
N510 G0 X0. Z5. M8
N520 Z2.
N530 G1 Z-51.009 F.25
N540 G0 Z5.
N550 M9
N560 G28 U0. V0. W0. M05
N570 T12600
N580 M01
(TOOL - 72 OFFSET - 72)
(ID ROUGH MIN. 20. DIA. - 80 DEG. INSERT - CCMT 09 T3 04)
N590 G28 U0. V0. W0.
N600 G50 X250. Y0. Z250.
N610 G0 T7272
N620 G18
N630 G97 S3600 M03
N640 G0 X18. Z1.25 M8
N650 G50 S2500
N660 G96 S200
N670 Z1.
N680 G71 U1. R.5
N690 G71 P140 Q150 U-1. W.2 F.2
N700 N50 G0 G41 X36. S200
N710 G1 Z-.094
N720 G2 X35. Z-.9 R.9
N730 G1 Z-15.
N740 X31.055
N750 G2 X29.379 Z-15.572 R.9
N760 N60 G1 G40 X18.
N770 G0 Z1.
N780 Z1.25
N790 M9
N800 G28 U0. V0. W0. M05
N810 T7200
N820 M01
(TOOL - 82 OFFSET - 82)
(ID FINISH MIN. 20. DIA. - 55 DEG. INSERT - DCMT 11 T3 04)
N830 G28 U0. V0. W0.
N840 G50 X250. Y0. Z250.
N850 G0 T8282
N860 G18
N870 G97 S2500 M03
N880 G0 X18. Z1.25 M8
N890 G50 S2500
N900 G96 S200
N910 Z1.
N920 G70 P140 Q150 F.1
N930 G0 Z1.
N940 Z1.25
N950 M9
N960 G28 U0. V0. W0. M05
N970 T8200
N980 M30
%

added Block numbers only to above

[machinehop5]

missing minus sign (-) first thing check for...


PS ...RS232 Cable soon in your future

DJ

[Asheen]

It’s working now. Thanks. I had left out a minus sign when I punched it in the machine and I had the wrong number for the tool tip in the offset screen. I bought a rs232 cable. But I think the pin configuration was wrong. I’m getting one made up with the correct configuration. It should be ready in a few days. Thanks for the help. In really appreciate it

[Superman]

Machinehop5.... your renumbering has just stuffed the program
.... it uses P & Qs which are the start and finish profiles for the roughing & finishing cycles..... the original format was ideal & much simpler to follow

Asheen..... why use cutter comp ?
.... it can complicate a simple program, as it can be easier to control sizes by altering offset values
.... Mcam can output "long" code ( no cycles ) that would suit your chosen tip radius.... change tip rad = repost Mcan with correct tool geometry
.... cutter comp should only be used for larger tip rads on larger radii & tapers... comp really messes up if you don't use sufficient retract clearances

[sinha_nsit]

You do not need V0 in G28 on a 2-axis machine. I was expecting that it would throw an alarm.

[machinehop5]

Machinehop5.... your renumbering has just stuffed the program

Maybe stuffed....but when discussing a Program how the hell do you know which Line someone is talking about. Bonehead reply Superdude

[machinehop5]

It’s working now. Thanks. I had left out a minus sign when I punched it in the machine and I had the wrong number for the tool tip in the offset screen. I bought a rs232 cable. But I think the pin configuration was wrong. I’m getting one made up with the correct configuration. It should be ready in a few days. Thanks for the help. In really appreciate it

Great to hear was something simple. Thanks for follow up.