G-Code error

[geppo_it]

good day Tom,
after a long pause I finally finished my lathe, mechanically and electrically.
Everything works smoothly: external buttons, handweels, rotary tool changer, spindle and so on.
Problems come when I try to launch a job and that is:

I open path file (TR_PROFILO_1.txt), it's all right.

I flag "Simulate", "run" and the path is executed and displayed in the graphics window without errors (Simulation.png)

I press Run button and I get G-Code error (run error.png)

The strangest thing is that if I run the same path with the "Single step" button most of the time I can get
to the end without errors, while sometimes I get the G-Code error as in automatic.
I'm sure I'm doing something wrong but I can't figure out what.
Some advice?

Beppe

Similar Threads:

• Need Help - Amada RG 80 Error code 315 / Alarm code 315
• Error codes for SCM Record 310 NT Router Error code 075-MACHINE OFF
• Help!!! Renishaw probe error code 2181 workpiece detection probe error (A24.5)
• Need Help!- Has anyone ran into this error? Parasolid ® Kernel Interface Error: KI Error Code:58
• g code error with image to g-code

[mactec54]

good day Tom,
after a long pause I finally finished my lathe, mechanically and electrically.
Everything works smoothly: external buttons, handweels, rotary tool changer, spindle and so on.
Problems come when I try to launch a job and that is:

I open path file (TR_PROFILO_1.txt), it's all right.

I flag "Simulate", "run" and the path is executed and displayed in the graphics window without errors (Simulation.png)

I press Run button and I get G-Code error (run error.png)

The strangest thing is that if I run the same path with the "Single step" button most of the time I can get
to the end without errors, while sometimes I get the G-Code error as in automatic.
I'm sure I'm doing something wrong but I can't figure out what.
Some advice?

Beppe

Why is N50 N55and N60 like that remove it and see if it runs

Also, what is G97 being used for it is not needed unless you are to cancel a G96 so this should be also removed

[TomKerekes]

Hi Beppe,

It's indicating an axis is disabled. Do you have another Axis besides X and Z defined in your coordinate system? Such as Y? Use KMotion.exe Axis Screen to check which axes are enabled.

Post your INIT C Program so we can see how your are defining your Coordinate System. Also any M6 or M8 Programs you have and how they are configured.

[geppo_it]

Lines 50-55-60 are a simple comment, the error occurs first: on the first G0. As for the G97 I will try to remove it but the interpreter will have to know that we are at constant revolutions and not at constant advancement.
Also I do not explain why the simulation doesn't detect errors since, presumably, the interpreter is the same.

Beppe

[geppo_it]

Hi Tom,
I'm at home right now, 9:15 pm here. In the morning I will copy everything you asked for and publish it.
However, I have a screenshot, captured after the error, of the status of the axes; find it attached

Beppe

[TomKerekes]

Hi Beppe,

That shows 0, 1, 2 enabled. What is Axis 1?

Maybe you are including Axis 3 (S?) as an A Axis?

[mactec54]

Lines 50-55-60 are a simple comment, the error occurs first: on the first G0. As for the G97 I will try to remove it but the interpreter will have to know that we are at constant revolutions and not at constant advancement.
Also I do not explain why the simulation doesn't detect errors since, presumably, the interpreter is the same.

Beppe

Comments like that in a program are not needed

A G97 cancels a G96 you don't have any G96 in the program, so it would not be needed unless the control defaults to G96 then you would need the G97 to cancel it

You have a G99 per revolution feed

It seems you have other problems though

[geppo_it]

good day Tom and Mactec54,

thanks for your interest.
The problem comes because, after finishing the tool change operation, I disable the turret motor driver. This is because, having a mechanical lock on the turret, I did not consider it necessary to keep the motor active. However, this has the consequence that, over time, a small position error becomes a large following error and the axis is disabled. Obviously, corrected this, everything works fine.

Tom, yes u right: I configured Axis 2 as Spindle and Axis 3 as A Axis. Is that wrong?
(Axis 0 as X and Axis 1 as Z)

Beppe

[geppo_it]

well guys,

just enough time to launch another path and another type of error appeared.
I generated the path with HSMWorks: with IK declarations the simulation practically stops on the first G2 it encounters; with the R statement the simulation goes a little further but still stops.
Since I have tried different post processors always getting the same type of error, I think there is something to fix in the Kflop setting ...
Or am I wrong??

Beppe

[geppo_it]

no one has any idea where the error might come from?

[TomKerekes]

HI Beppe,

Regarding Radius Post:If you do the math the distance between the start and end points of the arc is > 3mm. So a circle with radius 1.35 can't possibly fit on both the begin and end. If you configure Diameter Mode (where all the X distances are cut in half) then it works for me.

Regarding IK Post:In Diameter mode if I double the I values such that it is real distance to center rather than half distance units then it works.

Do you want KMotionCNC to operate in Diameter or Radius mode for X?

Is your CAD system set to output Diameters or Radii?

[geppo_it]

hi Tom,

I configured Diameter mode and now everything is working fine. I just have to check if the CAD system gives me the right displacements to obtain the desired diameters.

Thanks, Beppe