Lathe - Interference issue - Mits control

Guys, could someone please run ( or just simulate if possible ) this code on a Mitsubishi control:

%
O110 (COMPTEST)
(FINISH OD - VNMG331)
(ENTER .0156 FOR TOOL NOSE R!!!)
G28 U0 W0
G00 G97 T101 S600 M03
G00 G42 X0.465 Z0.08
G96 S360 M08
G01 X0.465 Z0. F.003
G01 X0.641 Z0.
G03 X0.6508 Z-0.0039 R0.005
G01 X0.736 Z-0.19
G01 X0.7 Z-0.21
G01 X0.7 Z-0.748
N100 G01 X0.72 Z-0.748 (***)
N110 G03 X0.736 Z-0.756 R0.008 (***)
G01 X0.736 Z-0.873
G01 X0.7845 Z-0.873
G03 X0.8005 Z-0.881 R0.008
G01 X0.8005 Z-2.405
G01 G40 X0.9605 Z.1 F.1
M09
M05
G28 U0 W0
M30
%

My problem: My NL2000 with the MSX-850 control will error out due to interference on blocks 100 and 110.
And yet, a Duraturn with the Oi-Tc or a Haas will run it fine and produces the expected results.

The tool nose is set to Dir 3, and the Nose-R is .0156 in all cases.

The above code is good, and I have finished my parts ( with some finesse ) so this is more for a research and figure out what I can do to
perhaps change some of the parameters on the Mits so it will work as expected.
Please note that even though the geometry is dancing on the razor's edge that's possible with a .0156 rad tool, it IS IN FACT possible and solvable!
The Fanuc does it, Haas does it, I don't see any reason why a Mits shouldn't!

I will run it on our 0i-TD but I won't be in for a couple days yet. Does your mits have a conversational side to the control. We had a Cincinnati that had "Shop Floor Programming" that made it pretty finicky on shit like this. But I also worked on a GE Mark Century 2000 that I swear would run whatever you fed it. Lol...

Brent

You are trying to make an arc with a radius smaller than the nose radius. Also, the step before the arc is too small, compared to nose radius, which would cause backward motion. No machine would do it unless there is some parameter to ignore these anomalies.

I ran this code in one of our Mazak lathes. Ran fine with cutter-comp turned off. (Parentheses around the G42.) Using a .0156" radius in quadrant 3, it would not run. Putting a .008" radius and the program would run. (Part looks like a barbed hose-fitting...?)


Sinha is correct. N100 is the problem. The radius of .0156" would require an X-positive move of at least .0312" or greater. There's basically no way to generate that code with a .0156" nose-radius tool. Either step down to a .008" radius tool, or you'll have to run without cutter-comp, and fake-in the G3 radii, by adjusting the start/stop points, and programming using a larger? radius.

sinha said:

You are trying to make an arc with a radius smaller than the nose radius. Also, the step before the arc is too small, compared to nose radius, which would cause backward motion. No machine would do it unless there is some parameter to ignore these anomalies.

Click to expand...

I think you've misunderstood the code. This is an outside radius, so the tool rad doesn't matter.
However, I am an idiot!!
Your comment about the step before the arc being too small is correct!!!

Just as Jashley said, it should be a min. .0312 diameter move in X, and I ( the retard ) saw the move from X.7000 to X.7200 as a .02 radial move, so it should be possible.
The problem lies in N100 exclusively.

Now... why did the Oi and the Haas run it?
Yes, the radius was a bit truncated, but ran nonetheless....

SeymourDumore said:

I think you've misunderstood the code. This is an outside radius, so the tool rad doesn't matter.
However, I am an idiot!!
Your comment about the step before the arc being too small is correct!!!

Just as Jashley said, it should be a min. .0312 diameter move in X, and I ( the retard ) saw the move from X.7000 to X.7200 as a .02 radial move, so it should be possible.
The problem lies in N100 exclusively.

Now... why did the Oi and the Haas run it?
Yes, the radius was a bit truncated, but ran nonetheless....

Click to expand...

You are right. I overlooked the fact that it is an outside arc, which is always made correctly. Thank you for correcting me.

As regards the step being too small, the control may ignore the step. I will look into the fanuc manual and confirm.

sinha said:

As regards the step being too small, the control may ignore the step. I will look into the fanuc manual and confirm.

Click to expand...

I did look into the Fanuc Operator's Manual. It does discuss the case of step being smaller than the tool radius.
Unfortunately, the description as well as the associated figure is so vague that it is difficult to understand what they mean. The only thing I could understand is that the control would not try to position the tool correctly at both the step corners. As a result, machining would continue without reversing the direction of the toolpath. There would be no alarm. However, some uncut material at the step would be left. But, there would be no overcutting.

sinha said:

I did look into the Fanuc Operator's Manual. It does discuss the case of step being smaller than the tool radius.
Unfortunately, the description as well as the associated figure is so vague that it is difficult to understand what they mean. The only thing I could understand is that the control would not try to position the tool correctly at both the step corners. As a result, machining would continue without reversing the direction of the toolpath. There would be no alarm. However, some uncut material at the step would be left. But, there would be no overcutting.

Click to expand...

That almost sounds like the parameter settings would force the control to feed straight up to the tangent-point of the G3 radius, and then execute the G3 arc/move...

Jashley73 said:

That almost sounds like the parameter settings would force the control to feed straight up to the tangent-point of the G3 radius, and then execute the G3 arc/move...

Click to expand...

This exactly would happen on a Fanuc. But, there is no reference to any parameter. So, this might be happening unconditionally.