Having problems cutting arcs with Fanuc 11M

[carlosdcerna]

I am having trouble with a Burgmaster 150 VTC milling center with a fanuc 11m control. We are trying to get the machine up and running and cutting 1" diameter circles was the last test we were going to run. At the end of the circle the machine seems to do some overcutting. You can see it in the pic bellow:

We are pretty sure it is not a backlash issue or a servo calibration issue. We think it must be a parameter that is not set correctly.

This is part of the nc program:

O0000(FICA CIRCULO 2)
(DATE=DD-MM-YY - 13-04-09 TIME=HH:MM - 11:46)
(MCX FILE - C:\MCAMX3\MCX\CIRCLE.MCX)
(NC FILE - C:\USERS\ANDRES\DESKTOP\FICA CIRCULO 2.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T5 | 1/2 SPOTDRILL | H5 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
N104 T5 M6
N106 G0 G90 G54 X0. Y0. S3500 M3
N108 G43 H5 Z.1
N110 G99 G83 Z-.125 R.1 Q.008 F20.
N112 G80
N114 S3000 M3
N116 X.0281 Z.25
N118 Z.1
N120 G1 Z-.0125 F10.
N122 G3 X-.0281 R.0281 F20.
N124 X.0281 R.0281
N126 G1 X.0563
N128 G3 X-.0563 R.0563
N130 X.0563 R.0563
N132 G1 X.1125
N134 G3 X-.1125 R.1125
N136 X.1125 R.1125
N138 G1 X.1688
N140 G3 X-.1688 R.1688
N142 X.1688 R.1688
N144 G1 X.225
N146 G3 X-.225 R.225
N148 X.225 R.225
N150 G1 X.2813
N152 G3 X-.2813 R.2813
N154 X.2813 R.2813
N156 G1 X.0281
N158 Z-.025 F10.
N160 G3 X-.0281 R.0281 F20.
N162 X.0281 R.0281
N164 G1 X.0563
N166 G3 X-.0563 R.0563
N168 X.0563 R.0563
N170 G1 X.1125
N172 G3 X-.1125 R.1125
N174 X.1125 R.1125
N176 G1 X.1688
N178 G3 X-.1688 R.1688
N180 X.1688 R.1688
N182 G1 X.225
N184 G3 X-.225 R.225
N186 X.225 R.225
N188 G1 X.2813
N190 G3 X-.2813 R.2813
N192 X.2813 R.2813
N194 G1 X.0281
N196 Z-.0375 F10.
N198 G3 X-.0281 R.0281 F20.
N200 X.0281 R.0281
N202 G1 X.0563
N204 G3 X-.0563 R.0563
N206 X.0563 R.0563
N208 G1 X.1125
N210 G3 X-.1125 R.1125
N212 X.1125 R.1125
N214 G1 X.1688
N216 G3 X-.1688 R.1688
N218 X.1688 R.1688
N220 G1 X.225
N222 G3 X-.225 R.225
N224 X.225 R.225
N226 G1 X.2813
N228 G3 X-.2813 R.2813
N230 X.2813 R.2813
N232 G1 X.0281
N234 Z-.05 F10.
N236 G3 X-.0281 R.0281 F20.
N238 X.0281 R.0281
N240 G1 X.0563

As you can see in the program the last circle in every step is cut by cutting two 180 degree arcs followed by a linear G01 move towards the center of the cicle. This is when the over cutting occurs.

We have tried cutting four 180 degree arcs(2 circles) without the linear move and the machine cuts them perfectly.

Can anybody help me find a solution to this problem?

[johnono]

have you tried programming it in incremental instead of absolute? could change the last cut, i think is where youre problem is?

[beege]

Also try using I instead of R, at exactly 180° I'm not sure the machine can figure out what to do. Also using I and no X, you can get a full circle out of one line of code, shortening it a bit

[sathma]

instead of this
N236 G3 X-.0281 R.0281 F20.
N238 X.0281 R.0281
try this
N236 G3 X-.0281 R-0.0281 F20.
If the circle is more then 180 deg, R must be in negative value
Sathma

[sinha_nsit]

From Fanuc manual:
"If an arc having a central angle approaching 180 is specified with R, the calculation of the centre coordinates may produce an error. In such a case, specify the centre of the arc with I, J, K."

And when you do use I, J, K method, the centre must be correctly specified. Otherwise, "if the end point is not on the arc, the tool moves in a straight line along one of the axes after reaching the end point."
In case of excess difference in start and end radii (defined by parameter 3410 on 0i series), an alarm would be generated.

[carlosdcerna]

We dont think its an error in cnc programming. We have tried using 2 CAM prgrams using both radius and i,j arc programming and nothing. Now my technician says it could be more of a mechanical issue. Maybe mechanical play in the machine tool. Anybody have any suggestions on where to start looking for the problem on the machine tool?

[Dan Fritz]

The first thing I'd check is the tool holder fit to the spindle. Does the tool holder taper fit the spindle taper? Does the drawbar pull the tool into the taper all the way? What about the tool holder itself? You're not using a collet holder with an endmill, are you ?

If you're using a proper endmill holder, and your tool holder is fitting the spindle OK, look for a servo following error problem by machining with a VERY SLOW feedrate. If the tool tracks OK with a low feedrate, try it at a normal feedrate with a very shallow depth of cut. This will indicate if the lateral forces on the tool are at play here. If the tool cuts a proper circle with a shallow depth of cut, but not with a normal one, assume that tool forces are moving something around. If the tool does not cut a proper circle with a shallow depth of cut (low tool load) at a normal feedrate, assume that your servos need work. It's possible that your servos are badly adjusted, or that your position loop gain is too low.