Type II G71 Stock Removal on Fanuc 0i-TB

[lowehardware]

I am trying to turn 270 degrees of a sphere on the end of 1.125" bar stock using Type II G71 and it isn't working. I'm getting an overcutting alarm 41 for the tool nose radius compensation. Here is the program below. Any help is greatly appreciated!!! (Tool nose is .0312 with imaginary tool nose 3)

G0T0404(TURNING TOOL)
G96S650M03
G0X1.145Z0.
G1X-0.05F.004M08
G0X1.125 Z0.05
G71U.06R.02
G71P101Q201U.01W0F.006
N101G0G42X0.Z.05
G1Z0.F.003
G03 X0.7071 Z-0.8536 R0.5
G01 X1.125
N201G0G40Z0.05
G70P101Q201
G80M09

[dcoupar]

I would try something like this:

G0 T0404(TURNING TOOL)
G96 S650 M03
G0 X1.145 Z0.
G1X-0.05 F.004 M08
G0 X1.125 Z0.05
G71 U.06 R.02
G71 P101 Q201 U.01 W0F.006
N101 G0 G42 X0. Z.05
G1 Z0. F.003
G03 X0.8012 Z-0.7992 R0.5
G02 X0.4279 Z-0.8536 R0.034
N201 G01 X1.125
G70P101Q201
G0 G40 X6.0 Z6.0
G80M09

[lowehardware]

thanks a bunch dcoupar, but do you mean to have the G02 line read this?:

G02 X0.8558 Z-0.8536 R0.034

[dcoupar]

Yes. That is to keep the TNR from causing interference in the corner.

[lowehardware]

The only way I could get it to work was by having the N201 line have G40 in it like I originally had. Why would the canned cycle not work without the line there?

I had to N201G0G40 back to the start point. I noticed you didn't return the tool back to the start point in your canned cycle yet the Fanuc book tells you to do this.

Thanks a lot!

[lowehardware]

Are there parameter settings to adjust with this case?

[dcoupar]

lowehardware,

None of my Fanuc manuals say to return the tool to the start point. What manual are you looking at? Also, please post the program that you finally got to work.

[SeymourDumore]

Well, since this thread was started twice, I'll copy my response from the other one.

Without going deeper into the code and geometric accuracy, I think your Q block is incorrectly placed.

G00 T404 (TURNING TOOL)
G96 S650 M03
G00 X1.145Z0.
G01 X-0.05 F.004 M08
G00 X1.125 Z0.05
G71 U.06 R.02
G71 P101 Q201 U.01 W0 F.006
N101 G00 G42 X0. Z.05
G01 Z0. F.003
G03 X0.7071 Z-0.8536 R0.5
N201 G01 G40 X1.125 <---- N201 moved to here.
G00 Z0.05
G70 P101 Q201
G80 M09

Actually sort of surprized that you're not getting a "Non Monotonous" error.
In TypeII roughing your X may vary in the + or - direction, but your Z must still be monotonous either + or - direction. That N201 sent it back to Z.05 withing the cycle.
Now, depending on the control itself, you may still get an overcut at the back. Note that your G03 ends at Z-.8536, and then you move only up in X.
The way I've changed your code would probably overcut on the Haas, because in this block:
G01 G40 X1.125 would move the tool in the Z direction by +.0312 as well.
I'm pretty sure Fanuc does the same thing, or perhaps worse by moving by 2X tool R in the +Z direction.
So, the way I'd do this cycle is to make a clearance move at the back of the radius, perhaps a little more than your tool R.

G00 T404 (TURNING TOOL)
G96 S650 M03
G00 X1.145Z0.
G01 X-0.05 F.004 M08
G00 G42 X1.125 Z0.05 <--- Note the comp-on BEFORE the cycle
G71 U.06 R.02
G71 P101 Q201 U.01 W0 F.006
N101 G00 X0. Z.05
G01 Z0. F.003
G03 X0.7071 Z-0.8536 R0.5
G01 Z-.8856
N201 G01 X1.125
G70 P101 Q201
G00 G40 X1.125 Z.05 <--- Ramp-off move here.
G80 M09

Please note that the code may not be all kosher. I never use G70 due to all the minor radiuses and edgebreaks during the finish pass, but with G71 or G72 I always comp-on prior to, and comp-off after the cycle. Better control over exact tool position at each step.

And to re-iterate, sending the tool back to the start point is not only not needed, but should not even be possible due to the non monotonous Z motion.

[lowehardware]

Dcoupar, you're right. My manual doesn't tell me to return to the start point. I'm going to modify things a bit and see where I go from here. I can post a similar program I used to make a part which isn't as simple as the example I used for this thread.

I always end up shifting arcs around so I don't overcut. Then I don't use a G70 but run a new toolpath for the finish cut.

Thanks also to SeymourDunmore. When I need to make the part again I'll mess around with your method.

[cogsman1]

Your code was not too bad to start with but you are turning on comp with a move in the wrong direction. Try this.


G0T0404(TURNING TOOL)
G96S650M03
G0X1.145Z0.
G1X-0.05F.004M08
G0X1.125 Z0.1 (*********)
G71U.06R.02
G71P101Q201U.01W0F.006
N101G0X0 (*********)
Z.05 (*******)
G01G42Z0F.003 (********)
G03 X0.7071 Z-0.8536 R0.5
G01 X1.125
N201G0G40Z0.05
G70P101Q201
G80M09

[lowehardware]

is that even Type II? in the N101 line you have to specify Z0.1 (where the tool starts) Correct?

[SeymourDumore]

Actually it doesn't matter where you turn on that comp. IN fact I'd suppose that cogsman's method won't even work in this instance, as the toolR is .0312 and the move from Z.05 to Z0 is less than the .062 required, and would likely cause overcut on Fanuc OR "Tool too big" error on Haas.

lowehardware
The next time you get this or similar part where you're forming a sphere, see if you can re-define your tool to be Dir8 rather than Dir3.
The really cool thing about it is that it truly uses the tool as it was a ball forming a ball, and you can dial in OD and sphericity variations easily.
Also, your comp-on and off moves become easier to manage, as you can plunge-in and retract in a straight move in front and back of the ball.
You can use the same tool as right now, all you have to do is add -.0312 to your Z offset and change the tool definition to 8.
I do turn a decent amount of balls, and this method gives me straight plunges for roughing and finishing, AND I can dial in the part to be spherical within .0002.