the program I am trying to run alarms out in graphics. It says the cutter Diameter to big for cutter comp to be applied. I am cutting around the outside of a part using Gibbscam. I have changed the lead in lead out to rediculously big numbers and it still can not do it. Could this be a postprocessor issue? If so is any one here using gibbscam with a haas minimill, that would have a post they can share?
Thread: cutter comp error
Results 1 to 11 of 11
-
04-19-2006, 01:35 AM #1
Registered
- Join Date
- Apr 2006
- Posts
- 100
cutter comp error
-
04-19-2006, 02:02 AM #2
Gold Member
- Join Date
- Jul 2005
- Posts
- 12177
Are there any G03 moves? Also have you tried using a smaller tool dia.? A tool too big for the radius of a G03 will alarm out.
-
04-19-2006, 02:34 AM #3
Registered
- Join Date
- Apr 2006
- Posts
- 100
It is doing it on a G01 move? I am not sure why it doesn't like this, there are no inside corners. it is also doing it on small tools as well.
-
04-19-2006, 02:47 AM #4
Registered
- Join Date
- Aug 2005
- Posts
- 578
post up the code...
-
04-19-2006, 02:51 AM #5
Registered
- Join Date
- Apr 2006
- Posts
- 100
Error
( OPERATION 2 ROUGHING )
( WORKGROUP )
( TOOL 1 .5 FINISH ENDMILL )
G0G90X2.64Y-1.
Z-.055
G41G1X2.5882Y-1.3F20.D1 (errors here)
Y-1.
X2.64F45.
Y-.9568
G2X2.5882Y-1.I-.5184J.5694
G1X2.4367Y-.8011
G2X2.2265Y-.8967I-.3151J.4137
G1X1.2274Y-1.1025
G2X1.109Y-1.113I-.105J.5093
G1X.1671Y-1.0888
G2X-.2937Y-.7823I.0134J.5199
G1X-.5541Y-.2036
G2X-.5425Y.2474I.4742J.2133
G1X-.2541Y.8086
G2X.2208Y1.0907I.4625J-.2377
G1X1.1658Y1.0682
G2X1.2824Y1.0521I-.0124J-.5198
G1X2.2672Y.8
G2X2.3492Y.7715I-.129J-.5038
G1X2.4507Y1.
G2X2.64Y.8803I-.3125J-.7038
G1Y1.
X2.4507
X2.3492Y.7715
G2X2.6581Y.2836I-.211J-.4753
G1X2.6415Y-.4
G2X2.4367Y-.8011I-.5199J.0126
G40G0Z.7
X2.64Y-1.
Z-.14
G41G1X2.5882Y-1.3F20.D1
Y-1.
X2.64F45.
Y-.9568
G2X2.5882Y-1.I-.5184J.5694
G1X2.4367Y-.8011
G2X2.2265Y-.8967I-.3151J.4137
G1X1.2274Y-1.1025
G2X1.109Y-1.113I-.105J.5093
G1X.1671Y-1.0888
G2X-.2937Y-.7823I.0134J.5199
G1X-.5541Y-.2036
G2X-.5425Y.2474I.4742J.2133
G1X-.2541Y.8086
G2X.2208Y1.0907I.4625J-.2377
G1X1.1658Y1.0682
G2X1.2824Y1.0521I-.0124J-.5198
G1X2.2672Y.8
G2X2.3492Y.7715I-.129J-.5038
G1X2.4507Y1.
G2X2.64Y.8803I-.3125J-.7038
G1Y1.
X2.4507
X2.3492Y.7715
G2X2.6581Y.2836I-.211J-.4753
G1X2.6415Y-.4
G2X2.4367Y-.8011I-.5199J.0126
G40G0Z.7
X2.64Y-1.
Z-.225
G41G1X2.5882Y-1.3F20.D1
Y-1.
X2.64F45.
Y-.9568
G2X2.5882Y-1.I-.5184J.5694
G1X2.4367Y-.8011
G2X2.2265Y-.8967I-.3151J.4137
G1X1.2274Y-1.1025
G2X1.109Y-1.113I-.105J.5093
G1X.1671Y-1.0888
G2X-.2937Y-.7823I.0134J.5199
G1X-.5541Y-.2036
G2X-.5425Y.2474I.4742J.2133
G1X-.2541Y.8086
G2X.2208Y1.0907I.4625J-.2377
G1X1.1658Y1.0682
G2X1.2824Y1.0521I-.0124J-.5198
G1X2.2672Y.8
G2X2.3492Y.7715I-.129J-.5038
G1X2.4507Y1.
G2X2.64Y.8803I-.3125J-.7038
G1Y1.
X2.4507
X2.3492Y.7715
G2X2.6581Y.2836I-.211J-.4753
G1X2.6415Y-.4
G2X2.4367Y-.8011I-.5199J.0126
G40G0Z.7
X2.64Y-1.
Z-.31
G41G1X2.5882Y-1.3F20.D1
Y-1.
X2.64F45.
Y-.9568
G2X2.5882Y-1.I-.5184J.5694
G1X2.4367Y-.8011
G2X2.2265Y-.8967I-.3151J.4137
G1X1.2274Y-1.1025
G2X1.109Y-1.113I-.105J.5093
G1X.1671Y-1.0888
G2X-.2937Y-.7823I.0134J.5199
G1X-.5541Y-.2036
G2X-.5425Y.2474I.4742J.2133
G1X-.2541Y.8086
G2X.2208Y1.0907I.4625J-.2377
G1X1.1658Y1.0682
G2X1.2824Y1.0521I-.0124J-.5198
G1X2.2672Y.8
G2X2.3492Y.7715I-.129J-.5038
G1X2.4507Y1.
G2X2.64Y.8803I-.3125J-.7038
G1Y1.
X2.4507
X2.3492Y.7715
G2X2.6581Y.2836I-.211J-.4753
G1X2.6415Y-.4
G2X2.4367Y-.8011I-.5199J.0126
G0G40Z.7
-
04-19-2006, 04:28 AM #6
Moderator
- Join Date
- Mar 2003
- Posts
- 927
Change the "G0G90X2.64Y-1." to G0 G90 X2.9 Y-1.
You don't have enough X move to turn on the comp..the tool is already over the X2.5882 before you start..X2.64 - X2.5882 = .0518 you need at least 1/2 the tool diameter to turn comp on.. so X2.64 + .250 = X2.89(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
-
04-19-2006, 04:33 AM #7
Gold Member
- Join Date
- Jul 2005
- Posts
- 12177
Your first few lines are:
( TOOL 1 .5 FINISH ENDMILL )
G0G90X2.64Y-1.
Z-.055
G41G1X2.5882Y-1.3F20.D1 (errors here)
Y-1.
X2.64F45.
Y-.9568
You move to set Tool Comp is from X2.64 Y-1. to X2.5882 Y-1.3 which is okay I think.
Then you have a move to Y-1. then X2.64 followed by X-.9568
I think in a sense you are backing up and the controller is trying to maintain the Left of Toolpath orientation for the G41 but your moves are not large enough to accommodate the tool dia.
Regarding your (error here) note I have found that on the Haas controller the highlighted line when the machine alarms out is not always the line on which the error is.
-
04-19-2006, 04:48 AM #8
Moderator
- Join Date
- Mar 2003
- Posts
- 927
Picture
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
-
04-21-2006, 05:05 PM #9
Registered
- Join Date
- Apr 2006
- Posts
- 100
tool diameter values in the offset, should they be Negative? I tried inputing negative values for the tool Diameters and now more of the program works i still have a few issues but the 1/2 inch tool works.
-
04-21-2006, 05:55 PM #10
Registered
- Join Date
- Apr 2003
- Posts
- 1876
Are you programming from the center of the geometry? So you have to enter the tool's dia (or rad) into the offset?
If so you're going to have problems.
You should have the computer comp the tool instead. (So you'll have zero as the value for the dia (rad))Matt
San Diego, Ca
___ o o o_
[l_,[_____],
l---L - □lllllll□-
( )_) ( )_)--)_)
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
-
04-21-2006, 06:04 PM #11
Gold Member
- Join Date
- Jul 2005
- Posts
- 12177
I think if you have a negative value for a tool diameter and command G41 the effect you get is the same as G42 with a positive tool diameter value. This means you may finish up going around the outside of a curve instead of the inside so a tool size conflict doesn't happen. But of course your tool path is way off.
Originally Posted by mikeh78
Reply With Quote
Posting Permissions
