please help me fix my code! PLEASE

[goodplastics]

I am trying to make a sample file for scanvec amiable so they can make a post for the fanuc 0mb control so common to CNC mills. My mill is a 1991 Fanuc drillmate T - model 10 with a 0Mb Fanuc control, anyone with the same machine would be able to help, but most 0mb controls are the same I figure. I have created a simple 5" x 5" square with 1/2" radius corners and a 1/2" hole in the center. The toolpathing is conventional milling around the outside of the square, 2 passes with a 1/2" end mill. Then with the same tool, peck drill a hole with 4 passes and a peck lift of .1"... The g-code it spits out is very wrong! I expected to see g83 instead of all the z movement. Could someone please correct this code so I can send it back to scanvec amiable as a comparison to their wrong code? I do know that the % sign at the begining needs to be removed, but it seems like lots of other stuff is missing, I'm not well versed enough in g-code to know what's wrong. Any help would be greatly appreciated!
Thanks,
Jason


%
O1234
N10 G90 G54 G17 G40
N20 la la l a100
N30 / (1/2" end mill )
N40 T6 M6
N50 S5000 M3
N60 G0 X7.66 Y6.979
N70 Z0.1
N80 G1 Z-0.5 F50
N90 G3 X6.91 Y7.729 R0.75 F100
N100 G1 X2.91
N110 G3 X2.16 Y6.979 R0.75
N120 G1 Y2.979
N130 G3 X2.91 Y2.229 R0.75
N140 G1 X6.91
N150 G3 X7.66 Y2.979 R0.75
N160 G1 Y6.979
N170 G0 Z0.1
N180
N190 G1 Z-1. F50
N200 G3 X6.91 Y7.729 R0.75 F100
N210 G1 X2.91
N220 G3 X2.16 Y6.979 R0.75
N230 G1 Y2.979
N240 G3 X2.91 Y2.229 R0.75
N250 G1 X6.91
N260 G3 X7.66 Y2.979 R0.75
N270 G1 Y6.979
N280 G0 Z0.1
N290 G5 X4.91 Y4.979 Z1. R-1. S0. P4. P0.1 F50. D0. S5000.0
0
0
0
R0.5 R0.
N300 M5
N310 G91 G28 Z0
N320 M30

[Mitsui Seiki]

Originally Posted by goodplastics I am trying to make a sample file for scanvec amiable so they can make a post for the fanuc 0mb control so common to CNC mills. My mill is a 1991 Fanuc drillmate T - model 10 with a 0Mb Fanuc control, anyone with the same machine would be able to help, but most 0mb controls are the same I figure. I have created a simple 5" x 5" square with 1/2" radius corners and a 1/2" hole in the center. The toolpathing is conventional milling around the outside of the square, 2 passes with a 1/2" end mill. Then with the same tool, peck drill a hole with 4 passes and a peck lift of .1"... The g-code it spits out is very wrong! I expected to see g83 instead of all the z movement. Could someone please correct this code so I can send it back to scanvec amiable as a comparison to their wrong code? I do know that the % sign at the begining needs to be removed, but it seems like lots of other stuff is missing, I'm not well versed enough in g-code to know what's wrong. Any help would be greatly appreciated! Thanks, Jason

Is this what you want?
%
O1234
N10G80G40G49
N20 T6 M6
N30 M1
N40 (1/2" end mill )
N50 G0 G90 G54 G17 X7.66 Y6.979 S5000 M3
N60 Z0.1
N70 G1 Z-0.5 F50
N100 G3 X6.91 Y7.729 R0.75 F100
N110 G1 X2.91
N120 G3 X2.16 Y6.979 R0.75
N130 G1 Y2.979
N140 G3 X2.91 Y2.229 R0.75
N150 G1 X6.91
N160 G3 X7.66 Y2.979 R0.75
N170 G1 Y6.979
N180 G0 Z0.1
N190 G1 Z-1. F50
N200 G3 X6.91 Y7.729 R0.75 F100
N210 G1 X2.91
N220 G3 X2.16 Y6.979 R0.75
N230 G1 Y2.979
N240 G3 X2.91 Y2.229 R0.75
N250 G1 X6.91
N260 G3 X7.66 Y2.979 R0.75
N270 G1 Y6.979
N280 G0Z0.5
N290 G0 X4.91 Y4.979
N300 G83 Z-1. R0.1 Q0.125 F50. S5000.0
N310 G0 G80 Z1.
0
0
0
R0.5 R0.
N320 M5
N330 G91 G28 Z0
N340 M30

[cnc-king]

Originally Posted by goodplastics I am trying to make a sample file for scanvec amiable so they can make a post for the fanuc 0mb control so common to CNC mills. My mill is a 1991 Fanuc drillmate T - model 10 with a 0Mb Fanuc control, anyone with the same machine would be able to help, but most 0mb controls are the same I figure. I have created a simple 5" x 5" square with 1/2" radius corners and a 1/2" hole in the center. The toolpathing is conventional milling around the outside of the square, 2 passes with a 1/2" end mill. Then with the same tool, peck drill a hole with 4 passes and a peck lift of .1"... The g-code it spits out is very wrong! I expected to see g83 instead of all the z movement. Could someone please correct this code so I can send it back to scanvec amiable as a comparison to their wrong code? I do know that the % sign at the begining needs to be removed, but it seems like lots of other stuff is missing, I'm not well versed enough in g-code to know what's wrong. Any help would be greatly appreciated! Thanks, Jason % O1234 N10 G90 G54 G17 G40 N20 la la l a100 N30 / (1/2" end mill ) N40 T6 M6 N50 S5000 M3 N60 G0 X7.66 Y6.979 N70 Z0.1 N80 G1 Z-0.5 F50 N90 G3 X6.91 Y7.729 R0.75 F100 N100 G1 X2.91 N110 G3 X2.16 Y6.979 R0.75 N120 G1 Y2.979 N130 G3 X2.91 Y2.229 R0.75 N140 G1 X6.91 N150 G3 X7.66 Y2.979 R0.75 N160 G1 Y6.979 N170 G0 Z0.1 N180 N190 G1 Z-1. F50 N200 G3 X6.91 Y7.729 R0.75 F100 N210 G1 X2.91 N220 G3 X2.16 Y6.979 R0.75 N230 G1 Y2.979 N240 G3 X2.91 Y2.229 R0.75 N250 G1 X6.91 N260 G3 X7.66 Y2.979 R0.75 N270 G1 Y6.979 N280 G0 Z0.1 N290 G5 X4.91 Y4.979 Z1. R-1. S0. P4. P0.1 F50. D0. S5000.0 0 0 0 R0.5 R0. N300 M5 N310 G91 G28 Z0 N320 M30

I dont think you will be able to see a g83 in your mill tool paths because the soft ware looks at drillilng and milling as two different operations, and the tool selection will be different in the software.



is this what you are looking for?
%( has to be here if it is fanuc)
O1234
N10 G90 G54 G17 G40
N20 la la l a100( what is this ?)
N30 (1/2" end mill )
N40 G49 T6 M6 ( our robos need the g49 before it will make a tool change)
N50 S5000 M3
N60 G0 X7.66 Y6.979
N70 G43 Z0.1 H6
N80 G1 Z-0.5 F50
N90 G3 X6.91 Y7.729 R0.75 F100
N100 G1 X2.91
N110 G3 X2.16 Y6.979 R0.75
N120 G1 Y2.979
N130 G3 X2.91 Y2.229 R0.75
N140 G1 X6.91
N150 G3 X7.66 Y2.979 R0.75
N160 G1 Y6.979
N170 G0 Z0.1
N180
N190 G1 Z-1. F50
N200 G3 X6.91 Y7.729 R0.75 F100
N210 G1 X2.91
N220 G3 X2.16 Y6.979 R0.75
N230 G1 Y2.979
N240 G3 X2.91 Y2.229 R0.75
N250 G1 X6.91
N260 G3 X7.66 Y2.979 R0.75
N270 G1 Y6.979
N280 G0 Z0.1
N290 G5 X4.91 Y4.979 Z1. R-1. S0. P4. P0.1 F50. D0. S5000.0
0
0
0
R0.5 R0.( G5 is a manufacturer assigned code, on our robos g5.1 turns on high speed machining) )
N300 M5
N310 G91 G28 Z0
N320 M30[/QUOTE]
%

[rsmachine]

Originally Posted by goodplastics I am trying to make a sample file for scanvec amiable so they can make a post for the fanuc 0mb control so common to CNC mills. My mill is a 1991 Fanuc drillmate T - model 10 with a 0Mb Fanuc control, anyone with the same machine would be able to help, but most 0mb controls are the same I figure. I have created a simple 5" x 5" square with 1/2" radius corners and a 1/2" hole in the center. The toolpathing is conventional milling around the outside of the square, 2 passes with a 1/2" end mill. Then with the same tool, peck drill a hole with 4 passes and a peck lift of .1"... The g-code it spits out is very wrong! I expected to see g83 instead of all the z movement. Could someone please correct this code so I can send it back to scanvec amiable as a comparison to their wrong code? I do know that the % sign at the begining needs to be removed, but it seems like lots of other stuff is missing, I'm not well versed enough in g-code to know what's wrong. Any help would be greatly appreciated! Thanks, Jason % O1234 N10 G90 G54 G17 G40 N20 la la l a100 N30 / (1/2" end mill ) N40 T6 M6 N50 S5000 M3 N60 G0 X7.66 Y6.979 N70 Z0.1 N80 G1 Z-0.5 F50 N90 G3 X6.91 Y7.729 R0.75 F100 N100 G1 X2.91 N110 G3 X2.16 Y6.979 R0.75 N120 G1 Y2.979 N130 G3 X2.91 Y2.229 R0.75 N140 G1 X6.91 N150 G3 X7.66 Y2.979 R0.75 N160 G1 Y6.979 N170 G0 Z0.1 N180 N190 G1 Z-1. F50 N200 G3 X6.91 Y7.729 R0.75 F100 N210 G1 X2.91 N220 G3 X2.16 Y6.979 R0.75 N230 G1 Y2.979 N240 G3 X2.91 Y2.229 R0.75 N250 G1 X6.91 N260 G3 X7.66 Y2.979 R0.75 N270 G1 Y6.979 N280 G0 Z0.1 N290 G5 X4.91 Y4.979 Z1. R-1. S0. P4. P0.1 F50. D0. S5000.0 0 0 0 R0.5 R0. N300 M5 N310 G91 G28 Z0 N320 M30

I think you guys are missing some important steps in helping to fix this program.


Here is how I do it, and it should work just fine in your mill:

%
O1234
N10 G0 G17 G40 G40 G49 G80 G90
N20 T6 M6
N30 (1/2" ENDMILL)
N40 G0 G90 G54 X7.66 Y6.979 S5000 M3
N50 G0 G43 Z0.1 H6 M8
N60 G1 Z-0.5 F50.
N70 G3 X6.91 Y7.729 R0.75 F100.
N80 G1 X2.91
N90 G3 X2.16 Y6.979 R0.75
N100 G1 Y2.979
N110 G3 X2.91 Y2.229 R0.75
N120 G1 X6.91
N130 G3 X7.66 Y2.979 R0.75
N140 G1 Y6.979
N150 G0 Z0.1
N160 G1 Z-1. F50.
N170 G3 X6.91 Y7.729 R0.75 F100.
N180 G1 X2.91
N190 G3 X2.16 Y6.979 R0.75
N200 G1 Y2.979
N210 G3 X2.91 Y2.229 R0.75
N220 G1 X6.91
N230 G3 X7.66 Y2.979 R0.75
N240 G1 Y6.979
N250 G0 Z0.1
N260 X4.91 Y4.979
N270 G83 X4.91 Y4.979 Z-1. R.1 Q.25 F50.
N280 G0 G80 Z1. M9
N310 G91 G28 Z0 M5
N320 M30
%

A few things were missing or incorrect about this post. You need to have decimal points in your feeds or the control will read it as a last place decimal. For example if you want to feed at 2 inches per minute you would use F2. but if you put it in as F2 it will feed at .0002 of an inch per minute

Next, G43 is used to set the tools height offset, but you must have the offset number following it hence the H6 on the same line. The H6 can actually be any number you want, but it is usually a good idea to have it match the tool number.

And the percent signs need to be there at the beginning and end of every program on a Fanuc control, the control uses these to tell it where the beginning and end of the program are. Primarily when sending and receiving the program via DNC.

If you need anything else just let me know and I will help if I can.

Sean