Hello all

I don't know if a couple of you remember me or not but I make automatic screw machine flat cams on my BP with Mach3.
I use a rotary table 4Th axis.
Now I would like to use radius comp with the rotary  but with the rotary I use degrees for its movement because that's the way cams are made and
read.
I need to or would like to setup for using radius comp with my 3/16 carbide end mill using the degrees of the rotary as the comp part.
The other axis used is X & of course Z.
The X controls the diameter or radius of the cam and the rotary turns the degrees.

So, can this be done or is it my pipe dream ? Lil

Mach3 has been flawless for several years now. Started out with Mach2.

It sounds an interesting problem, but I can't quite picture what your are trying to do.

Tool compensation is usually fixed to a linear axis, and Mach3 adds (or subtracts) the relevant distance from the one on the axis. I can't see how you can apply this to a rotary axis. Rotary axis rotate, I can't see where the radius comp comes in.

See my setup     http://www.scanalex.com/CNC.html    as the table rotates from a smaller diameter to a larger one, you
need to allow for the end mill diameter. Because a screw machine cam is all based from the center point of the cam, the rotational of the degrees needs to make up the diff when the end mill clears the top of the rise and needs to start milling a large radius.  If you don't, then the end mill will cut off the top of the start rise and at the bottom of a rise or drop the end mill
will not truly be in the right position.
Picture the X moving the end mill out to make a bigger diameter as the A rotates. If the rise on the screw machine needs to
be 30° then if you rotate the table 30° and move the x out to the next diameter, the end mill will be leaving too much at the bottom of the rise and may be ok at the top.
Then you need to do the flat or dwell on the cam. If its 5° of dwell or flat diameter, and the A axis rotates it only 5°, the next move to a smaller diameter would cut off part of the top dwell. You would only end up with 3-4° of flat or dwell.

See what I mean?  I hope. lol

Hello again
So I take it that this is not just something that I have missed in my setup?

Thats too bad. I wish it was that simple.

If anyone has any thoughts on this, I would really appreciate the help.

ESCO let me do some testing(;-) Never looked at mach COMP that way. I know what you are doing so I will give it a whirl and see what pops up. Have you ever thought of converting it to standard 3axis interpolation?? IF you are really in need of tool comp(and I can see where it would be very handy) that may be all that mach can do.

(;-) TP

I do appreciate your efforts.
I would prefere not to go the standard route because my files can be used for reference by most any screw
machine guy.
Even the design layouts for the cams I do are user friendly so no one has to say "how did he do that"?  lol

Esco I think it will work IF you acount for the SHIFT in Y before you apply the comp.

G0 X0Y0Z0

X-1
Z-1

G1 A360
Z0

DOes a circle 1" diam on tool centerline.

G0x0 Y1 Z0
G41 P1
X-1
Z-1
A360
Z0
G40

Does a 2" circle
IT appears the offset IS being applied.

You just have to account for the initial offsetting of Y before you apply the offset and start cutting. AND never move Y(;-) until you have completed the cut. IF you change directions and then use G42 the Y offsetting will be in the opposite direction.

HOPE That helps, (;-)

Hmmm
I will have to give that a try. Below is what I am doing using the multi pass function. See the link to youtube for the cam
that the below prog is making.

(   ******************   )            
(   Feed Cam       )            
( D6      )            
                  
G90                  
G0   Z0               
G1   A20.0      F200         
G1   A0      X   3.25   F100   ( 3.230 final pass )
G1   Z-2.5            F200   
G1   Z-2.650            F10    
M01                  
   Z-2.800            F3   
/   Z   -2.955   F5         
/   Z   -3.060   F5         
                  
G91                  
G1               F60   
                  
                  
                  
N   4   A   20.76         
N   5   A   22.79   X   -0.702   F40
N   7   A   137         F60
N   8   A   143.9   X   0.192   
N   10   A   14.03         
N   11   A   21.52   X   0.51   F40
N   13               
            G90      
            G0 Z0        
            G1A380X3.3F200      
            G0 A360      
            G92 A0      
            M30      
Video of this cam can be seen here.

http://www.youtube.com/watch?v=i9DzEsOPGwo

YEP the use of comp would allow a cleanup cut without recoding the cam. Just make a simple change in the Comp value and rerun the same code.

(;-) TP

I will try it on one tomorrow. I will keep you posted.
Thanks