Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: escowizard on February 02, 2009, 06:54:57 PM
-
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
-
OK, This is very interesting so far.
Now I have selected T1, and in my tool selections put in the dia. of .1875 for my end mill.
See the prog below,
Under "Config" then "Toolpath Config" I have these checked so I can view the actual cam being cut.
Show Lathe Object X
A Rotations Enabled X
Axis of Rotations = Z-Axis
Now when the endmill moves to the first cut @ x.965 the Y does offset to +.094
This is good so far, then as the EM moves up the rise, it gets too close to the corner and then
goes beyond the dia. like it should to allow for the EM dia.
Then it runs over the x1.910 rad and beyond like it should. Then down the return good. then it follows
the x .965 rad back home but goes too far into the first rise. ??
I notice it does not allow for x comp on the x .965 at all but does on the x 1.910 rad.
So its comping the Y ok except the first rise top and only comping the x at the top.
I did up a cam with two diff rise segments and the comp was confusing because of needing G41 then G42 then ....you see what I mean?
SO if you get time, try this out and see if it does the same on yours and what your thoughts are about it.
( 111111 )
( CC2 Cam )
( D4 )
G90
G0 Z0
G1 A10.0 Y0 F200
G42
G1 A0 X 0.965 F100 ( .945 )
G1 Z-2.5 F200
G1 Z-2.650 F5
M01
Z-2.800 F5
G91
F200
N 4 A 35 X 0.945 Y.094
N 6 A 50 F200
G41
N 7 A 20 X -0.9449
G40
N 9 A 255
G90
G0 Z0
G1A380X2.5Y0F200
G0 A360
G92 A0
M30
Thank you
-
Followup
Why is it that when the EM moves to the first cut, the comp moves the Y to +.094 (which is ok and works) but when
the EM rises up to the top of the cam, the Y ends up at Y-.094 ?
I mean its like Mach3 thinks its on the other side of the cam and not still on the same rise. That makes it cut too deep
into the cam at that point.
Must be because I am using the rotary, huh?
-
YOU might need to read up on the use of tool radius comp. THere is a set proccedure to its use.
ALSO in this particular use you cannot use mixed axis XY moves will in comp AND use the A xis as well. IF you do it will not COMP your moves correctly based on the use of the A AXIS in place of the Y axis. You would need to position the Y axis to account for the initial comp value BEFORE you move the X into position to start the cut.
HOPE that helps, (;-) TP
-
Hmmm
I had set it up like the help file said however the tool path started good but cut too deep into the bottom dia. and then
cut off the return part of the cam.
I was dubbing around with trying to get it to act the way I wanted but what you see was the best I could get at the time.
I will have to mess with it some more later.
Thanks