LinkBack URL
About LinkBacks
Post your program here so we can see what might be causing the error. Also, what are the values in the T and R for that tool?
| | |
Error 041 Hello!
I have a Fanuc 21i-T. When I use the G42 code in my G71 ..G70 caned loop this error message occur '' 041 Interference in NRC ''
What's the problem?
Best regards
Jean-Denis
Post your program here so we can see what might be causing the error. Also, what are the values in the T and R for that tool?
Hello!
Dcoupar
This is my program
%
O0102 (INSERT 48 66363 )
N10 G20 G50 S3000
N20 T0101 (CONTOUR )
N30 G97 G0 X,375 Z,04
N35 S1800 M03
N40 G71 U,03 R,02
N50 G71 P60 Q100 U,01 W,005 F,008
N60 G0 X,170
N70 G1 Z0 F,005
N80 X,250 Z-,04
N90 Z-,32
N100 X,188
N110 Z-,375
N120 X,25
N130 X,375 Z-,405
N135 G42
N140 G70 P60 Q130
N145 G40
N150 G0 X2 Z4
N160 T0202 ( FILET 1/4-20 NC )
N170 G97 GO
N180 G0 X,27 Z,1 S600 M03
N190 G76P010060Q00R00
N200 G76 X,181 Z-,36 P325 Q90 F,05
N210 GO X2
N220 G0 Z4
N230 T0404 (RAINURE + COUPER)
N240 GO Z-.56
N250 X,39
N260 S1000 M03
N270 G1 X,08 F,005
N280 G0 X.39
N290 Z-1.06
N300 G1 X-.1 F.005
N310 G0 X2
N320 Z4 M30
The value of T=2 and R = .032
Many Thanks.
Jean-Denis
Jean,Originally Posted by jdgromi
1. You start the G71 cycle with a an X only move in line N60. This will invoke Type I G71 cycle, in which only monotonous X direction moves are allowed, no pocketing, yet the moves between N60 and N100 show a change in direction of X. This would have no bearing on the error message you have, but its not the correct way to program G71. G71 Type II allows pocketing and is invoked by programing any combination of X or U and Z or W on the N60 line.
2. From what I can see from your program, the moves between N90 and N120 forms a groove that has a width of 0.055. As can be seen in the picture contained in the attached zip file, there will be considerable interference with the work during various moves. The Green circle represents move N90, the Blue circle move N100 and the Red circle move N110. I suspect that this will be the reason for the error.
G42_Error.zip
3. From your program, it would seem that the program is for an OD profile and the G42 would indicate that the tool is on the right side of the work's center line, viewed looking toward the chuck. If that the case, then I believe that the T value should be 3. T=2 would be for a boring bar.
Regards,
Bill
Last edited by angelw; 01-06-2011 at 01:30 AM. Reason: Edit point 2 with regards to reason for error.
ERROR 041 Hello!
Thank Bill
Your answer was correct.
I had two major errors, my tools radius was to hight and my T value was wrong too.
I have an other question:
How can I program my G71 in type II. You wrote that G71 allows pocketing. How can I write line N60 for to do that?
Best Regards
Jean,
All you have to do is have a two axis move on that first line. The Z doesn't have to actually be a move, but the control must see an X and Z word, or the equivalent incremental representation. In the example below you will see that the Z value in the N60 line is exactly the same as the Z value where you parked the tool prior to calling the G71. You could also have programed X0,170 W0,0, and this would have invoked G71 Type II.
With your original program, and ignoring the tool nose radius issue, your workpiece would have been stuffed during the roughing cycle before the finishing pass. The picture in the attached zip file shows the tool path for the roughing and finishing in Red and Green respectively. I've used a smaller tool radius in the roughing for clarity so that you can see the two paths, other wise the first part of the program would have only shown the one color. You will see in the picture where the roughing tool came down on the Z+ side of the groove. This is because the 6 and 9 o'clock points on the tool radius are the points that are programed.
I'm not a fan of using tool radius compensation with a lathe. It's necessary with a machining center, because you need that to control the size of the part, but with a lathe, this is not the case. Further, with a lathe machining towards the chuck and the tool on the right hand side of center line, G42 would be used to offset to the right away from the center line. When the tool is returning to the Z start to take the next cut, the tool will still keep to the right of the programmed path, but offsetting to the right is now towards the center line, with disastrous results if the tool was not retracted a sufficient distance to avoid interference with the work, or G42 canceled or swapped with G41.
Programming the true position of the tool with respect to tool nose radius comp is easy, even if done manually, and with the low priced or free CAM packages available to do this for you, I see little argument for using tool radius comp with a lathe.
G42_Error2.zip
Regards,
Bill
%
O0102 (INSERT 48 66363 )
N10 G20 G50 S3000
N20 T0101 (CONTOUR )
N30 G97 G0 X,375 Z,04
N35 S1800 M03
N40 G71 U,03 R,02
N50 G71 P60 Q100 U,01 W,005 F,008
N60 G0 X,170 Z0,04 (This will invoke G71 Type II)
N60 G0 X,170 (This will invoke G71 Type I only)
Last edited by angelw; 01-07-2011 at 03:28 AM.
065 illegal command Hello! Bill
When I had included in my program this line "N60 G0 X,170 Z0,04 (This will invoke G71 Type II), this error occure: 065 illegal command in G71-G73. Perhaps a bad setting of my controler???? I don't konw.
Best regards
Jean-Denis
Jean,
Its probable that your control does not have G71 Type II. Its an option, but its a fairly basic option and most Fanuc controls from 6TB onwards had G71 Type II without it specifically being requested when the machine was ordered. In fact, late model control manuals simply refer to the two Types without reference to Type II being an option.
Regards,
Bill
Posting Permissions
| | |
