[woffler]

Would some one care to share a G33 thread example so i can modify a post for Bob Cad , i am currently using Mach and changing to UCCNC .
Mach uses a G32 and UCCNC needs a G 33 and a K word for pitch angle according to the documentation ,just trying to see what it looks like.


Thank You

[OlfCNC]

I think the G33 syntax is pretty straightforward.
Copy from the manual:

Spindle Syncronised motion : G33
Program G33 X... Z... K... Q... to perform a spindle syncronised motion, where the X parameter is
the final position of the X-axis, the Z parameter is the final position of the Z-axis. The K parameter
is the pitch per revolution and the Q parameter is the start angle in degrees.
For the spindle syncronised motion an incremental encoder with A, B and Index channels has to be
installed onto the spindle and the spindle encoder has to be setup in the software.
When executing a G33 command, the motion controller will first waiting for the index channel
signal from the spindle encoder and will syncronise the feedrate to the rotational speed.
The start angle (Q parameter) defines the angle between the encoder index signal and the motion
controller measures the set angle after the index signal and starts the motion at this angle.
The G33 motion is always on a straight line just like with G1, but it is always on the XZ plane and
the feedrate is continously syncronised to the spindle speed and taking the pitch (K) parameter into
account. The syncronised motion always ends at the programmed X and Z coordinates.
If both the X and Z coordinates are programmed for the G33 command and if both coordinates
differs from the starting coordinates then the thread will be cut on a cone on the XZ plane and the
thread will then not be parallel to the Z not the X axis. The pitch is then calculated on axis which
makes the longer movement.
If more G33 commands follows eachother and if the start angle is not programmed or only
programmed for the first G33 command then the rest G33 commands will be syncronised with the
previous G33 command which makes it possible to cut a continous thread even with changing pitch.

[vmax549]

It uses the same format as LinuxCNC does.

(;-) TP

[woffler]

Thanks for that example , i will send it in with the post and let them figure this one out , i believe they will have to write a Macro and call it to get the post to output it.

[OlfCNC]

I think what the post should do are:

1.) Turn the spindle on.
2.) Move to the thread start point with a proper lead in (G1 with proper feedrate)
3.) Do a G33 with programmed pitch (K) and the endpoint (X and/or Z).
4.) Lead out at the end (G0).
5.) Repeat from point 2. changing the depth, deeper X or Z depending on which axis is the depth of the thread.

[woffler]

Thanks Olf , that explains it very well and it should be a good example to follow them to modify my post ,i really appreciate all the answers and reply's ,i have been waiting a long time to get rid of Mach 3 and all of it's fault's .

[OlfCNC]

No probs.
I think you should start with some manually written code to get familiar with the syntax.
Try to write some basic G33 codes with feed in in the start and feed out at the end and check how that works.
If that works you will be more familiar with it and then you could create a post processor with more confidence.

[vmax549]

Why not simply use the G76 function in UCcnc. That is what it is for to program threading (;-) .

Much easier that trying to write a Post to define a threading cycle.

(;-) TP