G33 for Mach3 Lathe only? or Mill also? or UCCNC too?

If you have a question about the software please ask it here.

G33 for Mach3 Lathe only? or Mill also? or UCCNC too?

Postby dammogreen » Fri Jan 12, 2018 11:22 pm

Does G33 only work with Mach 3 LATHE?

Or maybe G33 also works with UCCNC software (mill) ? I realize it's always in the XY plane . (although can be made non-parallel too either..not expecting to need that)

Or can it be used with a vertical mill that is using a rapidturn type 4th axis mounted horizontally on the mills bed..with the spindle axis parallel to the x axis?

I am wanting to do tapered threads on my 4th axis spindle. I'd be OK with "tricking" rewiring/configuring the 4th axis and z so they are now horizontal. (swap axis as needed)

I have gang "lathe" tooling mounted to the vertical/z spindle head. Requires x an y moves to select each tool.
dammogreen
 
Posts: 41
Joined: Thu Jan 11, 2018 10:24 pm

Re: G33 for Mach3 Lathe only? or Mill also? or UCCNC too?

Postby cncdrive » Sat Jan 13, 2018 2:18 am

G33 works in UCCNC, it is spindle syncronised motion and it works in the XZ plane.
How it works is documented in the UCCNC manual like other g-codes aswell.
And what works with Mach3 is documented in the mach3 manual. Especially there is no G33 code in Mach3, but there is G32 which is very similar to the G33 in the UCCNC.

The copy of the G33 documetation from the UCCNC 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.


The G33 always works on the XZ plane.
The UCCNC also has Swapaxis function with which you could swap the axis pins.
cncdrive
Site Admin
 
Posts: 2361
Joined: Tue Aug 12, 2014 11:17 pm

Re: G33 for Mach3 Lathe only? or Mill also? or UCCNC too?

Postby dammogreen » Sat Jan 13, 2018 2:41 am

Thanks I've ordered a Ub-1 to go with it, I'll let you know how it all goes.

I guess I will have to use UCCNC rather than MACH3 Lathe, because with Mach3 Lathe I won't be able to move both the x an y axis to move my gang tooling on the mill...and in Mach3 mill, there will be no G32...?
Last edited by dammogreen on Sat Jan 13, 2018 2:46 am, edited 1 time in total.
dammogreen
 
Posts: 41
Joined: Thu Jan 11, 2018 10:24 pm

Re: G33 for Mach3 Lathe only? or Mill also? or UCCNC too?

Postby cncdrive » Sat Jan 13, 2018 2:44 am

OK, if you will need any help feel free to comment on the forum or ask us in email.

BTW, here is how the G33 works, just 2 demo videos:



cncdrive
Site Admin
 
Posts: 2361
Joined: Tue Aug 12, 2014 11:17 pm

Re: G33 for Mach3 Lathe only? or Mill also? or UCCNC too?

Postby cncdrive » Sat Jan 13, 2018 2:47 am

And here how it works on a lathe:

cncdrive
Site Admin
 
Posts: 2361
Joined: Tue Aug 12, 2014 11:17 pm

Re: G33 for Mach3 Lathe only? or Mill also? or UCCNC too?

Postby dammogreen » Sat Jan 13, 2018 2:53 am

Yes i've seen those two videos and read in the manual how G32 can seamlessly change the pitch ...clever!

I guess I will have to use UCCNC rather than MACH3 Lathe, because with Mach3 Lathe I won't be able to move both the x and y axis to move my gang tooling on the mill...and in Mach3 mill, there will be no G32...?
dammogreen
 
Posts: 41
Joined: Thu Jan 11, 2018 10:24 pm

Re: G33 for Mach3 Lathe only? or Mill also? or UCCNC too?

Postby Derek » Sat Jan 13, 2018 1:36 pm

Keep in mind there isn't a turn module for UCCNC yet.
Derek
 
Posts: 297
Joined: Mon Sep 05, 2016 9:57 am

Re: G33 for Mach3 Lathe only? or Mill also? or UCCNC too?

Postby dammogreen » Sat Jan 13, 2018 2:53 pm

Thanks, I've been aware of that.

Since G33 works in UCCNC (mill/default) I should be fine without a specific lathe mode.
dammogreen
 
Posts: 41
Joined: Thu Jan 11, 2018 10:24 pm


Return to Ask a question from support here

Who is online

Users browsing this forum: No registered users and 5 guests