Lathe simple GCode / compensation
03 Sep 2014 23:38 #50698
by emcPT
Lathe simple GCode / compensation was created by emcPT
Hello. I have been running Linuxcnc lathe for a nice period of time and normally I can get things running as they are supposed to.
Currently I want to machine a very simple shape, but due to the compensation it is not letting me to.
The following code fails due to the compensation (the common gauge error), and I am not seeing correctly how to solve it.
Tool is outside machining, radius 0.4, tooltip direction 2 (linuxcnc tool tip direction)
Taking the compensation out, the code is accepted.
The output should be the outside of the picture attached.
I understand the problem, that is related with the intersection of the two lines that create a less than 90 degrees on the top, but at the same time is not clear to me to solve it (and still use the compensation ON that will be necessary).
Any ideas?
Thank you
Currently I want to machine a very simple shape, but due to the compensation it is not letting me to.
The following code fails due to the compensation (the common gauge error), and I am not seeing correctly how to solve it.
Tool is outside machining, radius 0.4, tooltip direction 2 (linuxcnc tool tip direction)
Taking the compensation out, the code is accepted.
(Init strings)
G21 (MM UNITS)
G18 (XZ PLANE)
G95 (UNITS PER REVOLUTION)
G7 (DIAMETER MODE)
(********************)
( OUTSIDE MACHINING )
(********************)
O9100 CALL
T1 M6
G43 (APPLY OFFSETS)
G96 D2500 S400 M4 M8
G00 X46.500 Z2
G00 Z4
F0.12
G00 G42 X45.043 Z2
G01 X43.798 Z-2.200
G01 X44.450 Z-2.200
G01 X43.798 Z-4.400
G01 X44.450 Z-4.400
G01 X43.798 Z-6.600
G01 X44.450 Z-6.600
G01 X43.798 Z-8.800
G01 X44.450 Z-8.800
G01 X43.650 Z-11.500
G01 Z-12.150
G00 X46.500
G00 G40 Z2The output should be the outside of the picture attached.
I understand the problem, that is related with the intersection of the two lines that create a less than 90 degrees on the top, but at the same time is not clear to me to solve it (and still use the compensation ON that will be necessary).
Any ideas?
Thank you
Please Log in or Create an account to join the conversation.
04 Sep 2014 06:03 #50720
by BigJohnT
Replied by BigJohnT on topic Lathe simple GCode / compensation
The error is more likely to be the inside corner not the outside corner. The error probably says near line xx and it is usually the next line. The inside corner can not be less than 90 with cutter comp as it can not reach the end of the vertical line before gouging into the next line. Try changing your code to put an arc or a short corner that can be reached by the tool.
www.linuxcnc.org/docs/html/gcode/tool_co...:cutter-compensation
JT
www.linuxcnc.org/docs/html/gcode/tool_co...:cutter-compensation
JT
The following user(s) said Thank You: emcPT
Please Log in or Create an account to join the conversation.
04 Sep 2014 19:59 #50753
by emcPT
Replied by emcPT on topic Lathe simple GCode / compensation
Thank you,
Will look into it and post the results.
Will look into it and post the results.
Please Log in or Create an account to join the conversation.
05 Sep 2014 19:22 #50804
by emcPT
Replied by emcPT on topic Lathe simple GCode / compensation
Correct, I added a radius a little larger than the tool radius and the code is now accepted, and most important, it makes sense.
Please Log in or Create an account to join the conversation.
Time to create page: 0.061 seconds