I would like to get some help setting up the rotary axis on a lathe I just completed. I am using a 3 axis driver with the X running parallel to the lathe base, the Z for the router and the Y set up as the rotary axis. I have set the Y steps in the motor tuning for degrees and if I manually enter a degree value, G1 Y360, it moves the correct amount. I also created a 4 flute file and if I edit the code and insert the 0, 90, 180, and 270 degree values for the Y it works.  I get a small step/bump on the Y axis from the inch values generated by the G code, but not the correct movement.
I’m not sure if there is a way to configure Mach to convert the Y inch values generated in the G code to degrees or if you have to use the A axis to accomplish that. If that is the case how would I set it up? I have looked on the forum, but didn’t see anything dealing with this.
This is my first attempt at rotary so any help would be greatly appreciated.

Thanks,
Richard

Richard,
What are you planning on doing with the rotary on the lathe?

I am currently on a new adventure to utilize the spindle as an indexer on the lathe. The intent is to drill holes, limited decorative cutting, some minor profiling, some wierd stuff...., after a piece has been turned. It will save setups.
I am using the A axis for rotary motion.

If i didn't have some specific things in mind i would probably just mount the rotary to the  mill  ( or maybe in your case a router ) and not bother.  

You may want to have a look at the following posts since there are a number of things to consider.

http://www.machsupport.com/forum/index.php/topic,13639.msg89612.html#msg89612

http://www.machsupport.com/forum/index.php/topic,13604.msg89361.html#msg89361

http://www.machsupport.com/forum/index.php/topic,12484.msg89181.html#msg89181

http://www.machsupport.com/forum/index.php/topic,12484.msg88232.html#msg88232

http://www.machsupport.com/forum/index.php/topic,13548.msg88932.html#msg88932

http://www.machsupport.com/forum/index.php/topic,13400.msg87932.html#msg87932

http://www.machsupport.com/forum/index.php/topic,13040.msg89459.html#msg89459

I guess it can be as simple or complex as you want.
Just remember there are some 4 different feedrates, 3 feedrate modes, the gcode that needs to be appropriate, choice of screens to use.

No answers ...but some stuff  to think about,

BTW nice name sort of like mine,  
RICH

Rich,
I have seen alot of the attachments you posted. Trust me, I am not doing anything as complex as you are. I have just converted a wood lathe to cnc to basically perform like the ones you see attached as a 4th axis option on cnc router tables.
Problem is I have never set a 4th axis setup and cant seem to get it to work. When I spoke of rotary axis, I was referring to the spindle of the lathe. Probably the wrong terminology.
If you could point me to something that will walk me through setting up the A axis that would be great.

Thanks,
Richard

Richard,
In Configuration:
Motor Outputs> enable the A, assign step and direction pin, port, and define if active low or high
Motor Tuning> set the steps per unit to your calculated  steps per degree and then experiment some 

                    to find the velocity and accel values.
General Logic Config> check the box so A-axis is angular ( left side of screen)
                              > Check the approproate boxes that apply "ROTATIONAL" you will find the         

                         defintions of them in the Mill or lathe manual
Hotkeys> define what key you want to use for jogging the A axis
ToolPath> Rotations check "Use Radius for Feedrate"
                               check A rotations enabled
                               check the axis of roataion that applies                               
Backlash> put the degree value in for the A Axis if you are going to use backlash or need it

--------------------------------------------------------------------------------------------------------------
Settings Tab>Rotation Radius ( from what Greg replied in another post )

As of Version R3.042.033 this has been, not quite fixed, but greatly improved.  Previous versions it

was buggy.

The DROs on the settings page are now labelled "Rotation Radius" which is now correct.  Previously

they were labelled "Rotation Diameters" which was partly right and partly wrong.

When "Use Radius for Feedrate" is checked in toolpath setup and you have a number greater than

zero in the appropriate "Rotation Radius" DRO this turns on the rotary axis feedrate compensation.

The compensation system takes the value of the "Rotation Radius" DRO and the value of the Z axis

DRO and adds them together to ascertain what diameter the cutter is at.

Then it compensates the rotary axis feedrate to keep the tool cutting at the called for feedrate. (within

motor tuning parameters)

So if you are using the centre of rotation for Z zero (which I always try to do) then have a near zero

number (0.01) in the "Rotation Radius" DRO and the Z axis DRO value will be used for the

calculation.

If on the other hand you have Z zero at the outer circumference of the job, enter that radius in the

"Rotation Radius" DRO, then this value plus whatever Z DRO is, will be used for the feedrate

calculation.

I said "not quite fixed" because Brian was going to fix the issue of a "Rotation Radius" DRO value of

zero turning the compensation system off, but he must have forgotten.

That is why you must use a near zero value in the "Rotation Radius" DRO and not zero.

Hope this is clear and helps.

Greg

So, the radius entered is really the location of Z zero relative to the axis of rotation?
Yes that is correct Gerry
-------------------------------------------------------------------------------------------------------------------------


The should all work fine using the Mill Screen . The lathe screen set in the link is currently missing

the Rotation Radius DRO.

Hopefully Greg or Gerry will take a read of this and coment appropriately.

BTW, I am not doing anything too complicated and I am trying to unconfuse "myself" on the

displayed feedrates relative to all the different modes, etc.

Probably forgot something,

RICH   

If your 4th axis is your lathe spindle, it will need some feedback from a servo motor with encoder or a stepper motor.

This is needed to know where it is positioning in relation with the bed or cutter.

Since you spoke about router, you probably need a stepper motor to run your lathe spindle.

I think the setup will be very similar to a standard 4th axis setup.

So if you can mount a stepper motor to the spindle, just follow the links posted in previous thread.

I am not sure if this what you need but take a look at these video

Jeff

http://www.youtube.com/watch?v=2igmcZNX6XQ

http://www.youtube.com/watch?v=aMKScg_k_Q8

http://www.youtube.com/watch?v=aYTeszyncv0

http://www.youtube.com/watch?v=3Rqo0yA-050

http://www.youtube.com/watch?v=nvw3doJiAV4

http://www.youtube.com/watch?v=S4b11mQpht8

http://www.youtube.com/watch?v=CvazK3rAPU4



 

Rich,
I think this is what I was looking for. Let me give it a shot and I will let you know how it turns out, no pun intended.

Thanks,
Richard

Rich,
Making some progress. Using your instructions, I now have the A axis active and the motor tuning calibrated and can rotate the spindle using code that I manually input.
There were two areas I ran into a problem.
First was the Rotational settings in the Gen Config. I could not find anything in the manual for the Rot 360 Rollover, or the Ang Short Tot on G0 options. That’s not to say they are not in there, I just couldn’t find them, so I left both unchecked.
Second, when I go to the settings page and enter a value into the Rotational Radius DRO, to activate the feederate compensation, the value clears as soon as I leave the page or click on anything else on that page.?? Not sure why that is happening.   

Richard

Richard,
Your not alone on not finding something as there are a couple of manuals and you need to look at all of them at times.
 Sometimes info only mentioned once, there are references to pages that were wrong, and as previuosly posted they  don't reflect changes.
 There is no "single" place to look for an easy grasp of all that is associated with a rotary axis.
 I am working on a Rotary Table How To write up which consolidates a whole bunch of info.
There are a lot of good postings about roatry  / 4th axis, but, you need to spend a lot of time searching for specifc info and application
 through all the replies to the postings.

ROT 360 ROLLOVER - when checked the A axis Dro wll display from 0-360 degrees and then start over at 0.
If not checked the A axis DRO will be additive such that 2 revolutions will display 720 degrees.

ANG SHORT  ROT ON G0-The axis will move in the shortest possible move to a new position, such that if
at 0 degrees and you jogged to 359 deg then it would just rotate   -1 degree.

ROTATIONAL SOFT LIMITS - if checked will apply "software"  limit switches to the rotary axis. 

When you input the value for A ROTATION RADIUS are you keeping the curser in the box and hitting the enter key? 
Works here. BTW, the standard lathe screen set dosn't have that DRO. Thus you need to use Mach Mill.

When playing around i suggest you don't do a rapid with an A axis rotation and axis move like:
G00 A360 X20     that corrupted one of my lathe xml's which then affected all the lathe profiles / xml's. 

RICH

Rich,
Thanks for the info on the settings. I am going to write it in the manual for future reference. I think I need to check the second option, sounds like it will speed up the cuts.
I didnt enter the info in the rotational radius correctly, so I will go back and enter it. I finally got the lathe working correctly last night. I had issues with the post processor in the cam program. It said it was a Y-A conversion, but it actually was doing an X-A conversion. Once that was corrected I ran several programs doing air cuts and it seemed to be working correctly. I guess the true test will come today when I actually cut something.
I really appreciate the help. I spent the better part of a week looking for basic information on line and although I found alot of information, most was well beyond the basics. I would like to see your write up when it is finished, its something needed for us beginners.

Thanks Again,
Richard

I hate to step in this thread but I have to ask.........

Rich, how can you possibly be a master of corruption and a bug slayer too?

How do you do it? LOL

Rich, you can delete this post if you want to. 

Richard, all of the docs should be comeing up to speed soon. Version 4 will be much easier to create docs for and I'm going to get Rich a brand new Pen. 

Thanks guys, this is a good thread with good people.

Brett