[nickrogers]

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

[ger21]

Post the g-code.

[nickrogers]

Hi Gerry,
Thanks for quick reply.
Here is G Code
Nick

[nickrogers]

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

[ger21]

The G Code is OK because I have checked it on a friend`s machine.

No, it's not OK.

Do you have a diameter in the tool table for tool #1?

The code is using G42 incorrectly, which is probably causing the issue.

[nickrogers]

Hi Gerry,
The diameter for tool number 1 is 2mm
Thanks
Nick

[ger21]

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.

Also on some jobs, the mill doesn't follow the tool path and I have to hit the EStop.

You need to provide more info for this one.

[nickrogers]

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

[ger21]

Ref using G42, what should I be doing?

You can't call G41/G42 before you do any moves.
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.

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?

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.

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?

[CitizenOfDreams]

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?

[ger21]

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.

[nickrogers]

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

[nickrogers]

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

[nickrogers]

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

[ger21]

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.

While it may work that way, it's not the proper way to program cutter comp.
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.

[nickrogers]

Hi Gerry,
OK - will do.
Once again, many thanks.
Regards
Nick