rotary axis

Hi, I am trying to get a rotary axis going on my CNC, I am using CNCWrapper software. I generate rounding code, run it and it stops on line 20 but doesn't give a error and the a axis continues to turn. if I try to highlight line 21 and click run from here it does nothing. Here is the code I am trying to run.

Hi

Making all sorts of assumptions for lack of any info, (is it defined as a rotary axis for a start?), you have commanded a 360 degree rotary axis to go to 19200 degrees at a very slow feed rate.

If you waited long enough the move would finish.

You will get other extremely long waits later in the code.

I have no idea what you are trying to make, none of the Z moves are negative, so by convention none of them would produce a cut into the workpiece

regards

PS

If you look long enough at the semi-legible crap that CAM produces, you also notice that it has not set the units

G00G17G90G40G49G80

So if A were defined as linear and the config was metric by default, it could take an incredibly long time to complete the move on line 20

Thanks that explains why it was going slow. I have read about inverse time mode, is it the only way to get this to work and can I just edit the code and replace the G94 with G93?

...........is it the only way to get this to work and can I just edit the code and replace the G94 with G93?

It will make it behave differently, but the main question is probably what is this code supposed to do?

It appears that at the beginning, the X axis moves 6", whilst the A axis rotates approx 60 times. This suggests a spiral cut along a 6" length, except that the Z axis is 1.729" above the workpiece throughout.
This can only work if you have touched off Z to the centreline of the workpiece, instead of the surface perhaps?
It is not the conventional way to do it certainly.

If you do use G93, just read the docs carefully and ensure that the value you use for F is one capable of being completed and that F is used on every line.
It is very easy to get confused and make a mess of it.

Whilst you are at it, add a G20 at the start and then at least it is clear the values are imperial.

regards

This code is for rounding the stock material. The z is touched off at the centerline and the units are imperial.

krrice wrote:

This code is for rounding the stock material. The z is touched off at the centerline and the units are imperial.

That makes sense, if you don't have a lathe.

You will just have to see how you get on with G93.

regards

Thank you to all that replied, I found a couple of errors on my part. First the feed rate is in degrees not (in/min) so the value I was entering was to low I ended up using 45000 for the feed rate. Second I redone my config file for the rotary axis and found I had not entered the correct value for (steps/degree) which was 4.7777. The software works fine for rounding and machining.