Newbie- G-CODE HELP

[jcromwell]

can someone look at this and tell me if it looks ok...fanuc oi-tc controller on a yama seiki lathe. Not use to straight g-code programming use to seimens conversational programing on a 840D, with a little g-code input. Could use a good reference for a simulator. Free or not.


O1000 (2IN OD SCH40 2TPI);
N10 G20 G40 G54 G80 G90;
N15 M98 P1;
N20 G00 X5.00 Z5.00;(SAFETY PULL OFF)
N30 S500 M13 T0101;
N40 G99
N50 G00 X2.80 Z0.00;
N60 G01 X 1.80 Z0.00 F.005;
N70 G00 X 2.80 Z.100;
N80 G50 S500;
N90 G96 S200;
N100 G42 X2.800 Z.100;
N110 G99
N120 G71 U.03 R.025;
N130 G71 P140 Q190 U.020 W0.00 F.030;
N140 G00 X2.239 S150;
N150 G01 G99 Z.030 F.030;
N160 X2.239;
N170 Z-1.600;
N180 X2.155 Z-.375;
N190 X2.239 Z-.475;
N200 G70 P140 Q190;
N210 M98 P1;
N220 G00 X5.00 Z5.00;(SAFETY PULL OFF)
N230 S500 M13 T0202;
N240 X2.250 Z.100 S500
N250 G76 P012000;
N260 G76 X2.155 Z-1.500 P0420 Q0500 F.500;
M270 M98 P1;
N280 G00 X5.00 Z5.00;
N290 S500 M13 T0303;
N300 G00 X2.80 Z-1.350;
N310 G01 X2.169;
N320 G00 X5.00;
N330 G00 Z5.00;
N340 S500 M13 T0505;
N350 G00 X2.80 Z-1.50;
N360 G00 X2.243;
N370 G01 Z-1.58;
N380 G00 Z-1.45;
N390 G00 X-5.OO Z-5.00;
N400 M98 P1;
N410 M01;
M30;
%

[timlkallam]

Welcome to the form I see this is your first post . A quick look at your code this is what I see.

Your G71 is backing up most G71cycles only use assending or desending cuts.
Cutter comp turned on but not turned off .
G76 cycle first line incomplete .
Spindle speed to slow .

Tell us what your doing so we could write you a program .
include stock size thread size types of tools you are using.
a print would be best.

[g-codeguy]

Originally Posted by jcromwell can someone look at this and tell me if it looks ok...fanuc oi-tc controller on a yama seiki lathe. Not use to straight g-code programming use to seimens conversational programing on a 840D, with a little g-code input. Could use a good reference for a simulator. Free or not. O1000 (2IN OD SCH40 2TPI); N10 G20 G40 G54 G80 G90; N15 M98 P1; N20 G00 X5.00 Z5.00;(SAFETY PULL OFF) N30 S500 M13 T0101; N40 G99 N50 G00 X2.80 Z0.00; N60 G01 X 1.80 Z0.00 F.005; N70 G00 X 2.80 Z.100; N80 G50 S500; N90 G96 S200; N100 G42 X2.800 Z.100; N110 G99 N120 G71 U.03 R.025; N130 G71 P140 Q190 U.020 W0.00 F.030; N140 G00 X2.239 S150; N150 G01 G99 Z.030 F.030; N160 X2.239; N170 Z-1.600; N180 X2.155 Z-.375; N190 X2.239 Z-.475; N200 G70 P140 Q190; N210 M98 P1; N220 G00 X5.00 Z5.00;(SAFETY PULL OFF) N230 S500 M13 T0202; N240 X2.250 Z.100 S500 N250 G76 P012000; N260 G76 X2.155 Z-1.500 P0420 Q0500 F.500; M270 M98 P1; N280 G00 X5.00 Z5.00; N290 S500 M13 T0303; N300 G00 X2.80 Z-1.350; N310 G01 X2.169; N320 G00 X5.00; N330 G00 Z5.00; N340 S500 M13 T0505; N350 G00 X2.80 Z-1.50; N360 G00 X2.243; N370 G01 Z-1.58; N380 G00 Z-1.45; N390 G00 X-5.OO Z-5.00; N400 M98 P1; N410 M01; M30; %

I'm not familiar with that lathe or particular flavor of Fanuc, but some observations anyway. G20 shouldn't be necessary. It is a default G-code. I don't know of anyone that switches back and forth between metric and inch. Doing so will change your tools geometry values, but the new values won't be right.

If your P1 subprogram is like the one on Hardinge lathes, then G40, G80, G90 & G99 are also unnecessary as they are in the P1 subprogram. Most likely they will also be the default commands upon powering up, but are included in P1 as safety measures in case you forget to switch back to them after changing them for a particular operation.

Blocks 80 & 90 should go after block 50 in order to increase the RPM as the tool faces off. Limiting max RPM to 500 may be a bit on the slow side, but I don't know the material or your setup. S150 for turning is low, but I have run jobs with SFM a lot lower than that. Depends on material. G00, G01 and G99 are modal. Use them once until you need to change them for their complimentary command: G99 to G98, G00 to G01, etc.

I've never used G41/G42, but it might possibly need to be in affect before the G71 cycle. I think you need to actually move the tool on the G42 block so it will be in affect before calling up the G71. However any comment of mine concerning G41/G42 is a guess. As Tim said, most controls aren't going to allow a change in X direction within the G71 cycle.

.03 is a pretty shallow roughing cut, but again it depends on material and setup. I'm running .032 DOC at F.007 for a Waspaloy job.

You should have a Q-value in the first G76 block if you want to specify the minimum DOC. I'm assuming this is an inch program in which case F.500 is a mighty course thread. :-) Also Z.1 is definitely not enough clearance for the Z-axis to accelerate for that course of a thread.

I don't know what tool 5 is, but it should crash. Clear the part before making the X-5. move. Trailing zeros are unnecessary. Consider using an M01 after every operation. I like to leave a blank line between operations. Makes the program easier to read.

No doubt I've missed some things. It's past this old farts bedtime. :-)

Do as Tim asks, and we can offer more help.