G3 command stops the process <G98 vs G99>

[mikechung]

Using Fusion 360 to post process using a few post processing files from Autocad and other sources
They are all very similar with a common problem, all stop when a G3 command is read.
The lathe cutting is a very simple turn with a round top. Cuts all the linear cuts till it reaches the top with a curve G3.
All other items I have design and used all stop. The Pawn sample supplied from Centroid does work.
I list some code as an example
Any ideas please ?
Don't see any major messages on screen
Screens attached

;;N98 G3 X24.2 Z-12.2 I-12.2 K-1.565 stops
;;N99 G1 Z-40.076 stops

;;N105 G3 X24. Z-10.635 I-11.2 K-5.084 stops
;;N106 G1 X26. Z-9.635

;;N110 G3 X22. Z-7.116 I-10.2 K-6.874
;;N111 G1 X24. Z-6.116

And this one at the start , no idea what this is

;;N24 G1 Z3.5 F1. stops

Hi
I have asked Autocad and Centroid but have no answer for my problem

[tblough]

It's not stopping because of the G3. It's stopping because of the G99 feed per rev command. You either don't have a spindle encoder, or your are losing steps because your Z-axis cannot move at 3mm per revolution. My guess is the former since you *should* be able to move at 1mm/rev.

[mikechung]

Hi, thanks for your quick reply.
Can you advise me how I change this?
Is this done in the fusion 360 program in the creating menus under machining , turn profile and then follow the conversation tabs tool, stock etc
I new to cnc and fusion, but have many years experience in IT and mechanical creation
https://www.vertogen.eu
Thank you
Mike chung

[tblough]

I'm not an F360 user, but I figure it is located on the dialog where you define your tool and set the speed and feed rate. There should be a button to select either mm/min or mm/rev where you input your desired federated.

[Centroid_Liviu]

Centroid took a look at the code and verified it would run. But there was no current report and as such could not troubleshoot this further. Looking at your report you sent, you have a spindle encoder setup in the software. Is a spindle encoder physically connected? Is it 2000 line / 8000 counts?

[cncsnw]

Given that the screen shot shows it is in G99 mode (feedrate driven by spindle revolutions), and the displayed spindle RPM is zero, it is no surprise that the message window says "Moving..." but the axes are not moving. The control is waiting for some rotation from the spindle encoder.

As Tom points out, if you do not actually have a spindle encoder connected, then you must be certain to program all of your feedrates in feed-per-minute (G98 mode).

[cnckeith]

there several example programs that do not require encoder feedback to run and use G98, they come with the CNC12 installer and are located in the ncfiles directory. and there are ones that do require an encoder and use G99. for example PAWN.CNC does not require and encoder and PAWN-enc.CNC does require and encoder. you can open them and see the difference etc..

[mikechung]

It's not stopping because of the G3. It's stopping because of the G99 feed per rev command. You either don't have a spindle encoder, or your are losing steps because your Z-axis cannot move at 3mm per revolution. My guess is the former since you *should* be able to move at 1mm/rev.

Hi
Thanks for your help, your advise worked perfectly

Just letting you know you where correct with the solution.
I replaced the G97 command with G96 S1000 M03
Now completes the program I send you.
I started 4 Weeks ago from Scratch when I bought a used small lathe hardly used.
Now I can design on Fusion 360 and run the Gcode successfully and start making parts.
Thanks
Mike Chung
https://www.vertogen.eu

[mikechung]

Centroid took a look at the code and verified it would run. But there was no current report and as such could not troubleshoot this further. Looking at your report you sent, you have a spindle encoder setup in the software. Is a spindle encoder physically connected? Is it 2000 line / 8000 counts?

Just letting you know you where correct with the solution.
I replaced the G97 command with G96 S1000 M03
Now completes the program I send you.
I started 4 Weeks ago from Scratch when I bought a used small lathe hardly used.
Now I can design on Fusion 360 and run the Gcode successfully and start making parts.

Thanks
Mike Chung
https://www.vertogen.eu

[mikechung]

Given that the screen shot shows it is in G99 mode (feedrate driven by spindle revolutions), and the displayed spindle RPM is zero, it is no surprise that the message window says "Moving..." but the axes are not moving. The control is waiting for some rotation from the spindle encoder.

As Tom points out, if you do not actually have a spindle encoder connected, then you must be certain to program all of your feedrates in feed-per-minute (G98 mode).

Just letting you know you where correct with the solution.
I replaced the G97 command with G96 S1000 M03
Now completes the program I send you.
I started 4 Weeks ago from Scratch when I bought a used small lathe hardly used.
Now I can design on Fusion 360 and run the Gcode successfully and start making parts.

Thanks
Mike Chung
https://www.vertogen.eu