Post the g-code.
Hi,
I have two problems.
Firstly on some jobs, the mill ramps down outside the tool path, and then follows tool path OK.
Also on some jobs, the mill doesn't follow the tool path and I have to hit the EStop.
I am attaching picture of what I mean.
The G Code is OK because I have checked it on a friend`s machine.
I really would appreciate any help.
Many thanks.
Regards
Nick
Similar Threads:
Post the g-code.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Hi Gerry,
Thanks for quick reply.
Here is G Code
Nick
Hi Gerry,
If you didn't get the attachment, G Code is as follows:-
M06 T1
G42 D1
G17
G00 X0 Y0 Z25
M03 S23500
G04 P3
G00 X-19.65 Y25.65 Z25
G00 Z3
F60
G01 X-19.65 Y25.65 Z-0.5
F200
G01 X-7.35 Y25.65
G01 X-7.35 Y-25.65
G01 X-19.65 Y-25.65
G01 X-19.65 Y25.65
F60
G01 X-19.65 Y25.65 Z-1.0
F200
G01 X-7.35 Y25.65
G01 X-7.35 Y-25.65
G01 X-19.65 Y-25.65
G01 X-19.65 Y25.65
F60
G01 X-19.65 Y25.65 Z-1.5
F200
G01 X-7.35 Y25.65
G01 X-7.35 Y-25.65
G01 X-19.65 Y-25.65
G01 X-19.65 Y25.65
G00 X-19.65 Y25.65 Z25
(second aperture)
G00 X7.35 Y25.65 Z25
G00 X7.35 Y25.65 Z3
F60
G01 X7.35 Y25.65 Z-0.5
F200
G01 X19.65 Y25.65
G01 X19.65 Y-25.65
G01 X7.35 Y-25.65
G01 X7.35 Y25.65
F60
G01 X7.35 Y25.65 Z-1.0
F200
G01 X19.65 Y25.65
G01 X19.65 Y-25.65
G01 X7.35 Y-25.65
G01 X7.35 Y25.65
F60
G01 X7.35 Y25.65 Z-1.5
F200
G01 X19.65 Y25.65
G01 X19.65 Y-25.65
G01 X7.35 Y-25.65
G01 X7.35 Y25.65
G00 X7.35 Y25.65 Z25
G00 X0 Y0 Z25
M5
M30
I appreciate your help!
Regards
Nick
No, it's not OK.The G Code is OK because I have checked it on a friend`s machine.
Do you have a diameter in the tool table for tool #1?
The code is using G42 incorrectly, which is probably causing the issue.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Hi Gerry,
The diameter for tool number 1 is 2mm
Thanks
Nick
Your friends machine probably has a diameter of 0 in the tool table.
You can't use G42 like your doing. That is the problem.
You need to provide more info for this one.Also on some jobs, the mill doesn't follow the tool path and I have to hit the EStop.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Hi Gerry,
Thanks for quick reply.
Ref using G42, what should I be doing?
Concerning the other problem, the picture I sent shows that the tool just went away from the tool path, and you have the g Code file.
What other information do you need?
Many thanks for your help, I really appreciate it!
Nick
You can't call G41/G42 before you do any moves.Ref using G42, what should I be doing?
And you need to do lead in and lead out moves, so the compensation is applied before you start cutting.
When using G41/G42, you don't want to start in the corner, as that generally won't leave any room for the lead in.
This is also caused by the G42. Because the compensation is never turned off, it doesn't really know where the tool is supposed to finish. That's why you ned a lead out move.Concerning the other problem, the picture I sent shows that the tool just went away from the tool path, and you have the g Code file.
What other information do you need?
It's also good practice to turn the comp off and back on between features, with lead in and lead out moves for each feature.
How was this code created?
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Is there a good reason to use G41/G42 codes today? I presume they were handy in the good old days of handwritten g-code, but a CAM program can just generate toolpaths for a specific tool. Or am I missing something here?
Yes, there is.
At work, on our router, most of the time we have resharpened tools in the machine, of various sizes.
Some days we may run over 1000 unique parts.
Some days we need to run parts that were programmed years ago.
With G41/G42, all parts are programmed using the standard tool size, but can be run at any time, with any sized tool that's in the machine, and the parts are always the correct size.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Hi Gerry,
Thanks for the reply.
The code was generated by myself using CNCCookbooks G Wizard, G Code Editor.
Some jobs involve more intricate tool paths, so I wanted to teach myself using this programme.
For simpler jobs, I use MACH3 Mill Wizard.
I shall try out your suggestions.
Many thanks.
Nick
Hi there,
I am using CNCCookbooks G Wizard G Code Editor to help me write my own code.
Some of the jobs are more intricate than this, so I wanted to learn code myself.
I am finding this programme OK, but clearly not fool proof as it would have showed me an error in this instance.
For simple jobs I am using MACH3 Mill Wizard, which is really easy to use.
Nick
Hi Gerry,
I just wanted to thank you for helping with this.
I find if there are several features on the job, I need only to turn cutter compensation off at the end of the job, not after each feature.
But I turn cutter compensation on before each feature is started.
Your help was invaluable as I am using my CNC router for commercial jobs.
thank you so much once again!
Regards
Nick
While it may work that way, it's not the proper way to program cutter comp.I find if there are several features on the job, I need only to turn cutter compensation off at the end of the job, not after each feature.
But I turn cutter compensation on before each feature is started.
If you're not turning it off, then you shouldn't have to turn it back on.
But I highly recommend turning it off and on for each operation.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Hi Gerry,
OK - will do.
Once again, many thanks.
Regards
Nick