need help! first time code writer!

Hey guys, how's your Tuesday treatin' ya? Long story short, I'm a student enrolled in precision machining technology and I'm stuck between a rock and a hard spot writing the code for my NIMS CNC Lathe level one credential. I keep getting a "604 non monotonous arc" alarm when I try to run my program, and I'm pretty lost as to how to fix it. The only fix I've come up with is increasing the radius, but that won't hold up to the necessary tolerances my part needs to pass. Here's my code if yaw'll wanna take a look at it! I'm new to the industry and I've got a lot to learn, so I'll take whatever advice I can get. Thank you for your time!

%
o84848 (NIMS CNC: Turning)
(6061 T6 bar stock aluminum 4.725" x 2.250")
(*********************************************)
T101 (tool 1, offset 1)
G50 S2500 (clamped)
G97 S320 M3 (spindle on)
(SP/intermediate) G54 G00 Z0.100 M8 (coolant on)
(SP/intermediate) X2.500
G96 S200 (SFM)
G71 P11 Q22 D0.050 U0.025 W0.025 F0.005 (rough pass)
N11 G42 G00 X0.000 F0.010 (profile start)
(ORIGIN) G01 Z0
(A) G01 X0.630
(B) X0.750 Z-0.060
(C) Z-0.625
(D) X1.250 Z-0.875
(E) Z-1.875
(F) X1.550
(G) G3 X1.750 Z-2.075 R0.200
(H) G1 Z-2.875
(I) X2.250
N22 Z-4.725 (profile end)
G40 G00 X2.500
Z0.100
G96 S250
G70 P10 Q21 (finish pass)
G40 G00 X2.500
Z0.100
M9 (coolant off)
G28 U0
G28 W0
M01
M02
%

N22 Z-4.725 (profile end)
G40 G00 X2.500
Z0.100
G96 S250
G70 P10 Q21 (finish pass) (Try Changing the Q21 to Q22)

And p10 to p11
U don't have there rows signed n10 and n21. Parameters p and q are row numbers signed in code. U need to sign row number anywhere U need to call specific row(with some exceptions)

Oh i read it once again... give row numbers to all Your geometry rows alarm will then say which row is the problem.
Now it's a row without n word, so haas doesn't tell U where it is.

Toneloc, check haastipoftheday videos. There is a video that will help you get past your alarm.

As steryd mentioned, the P and Q for both G71 and G70 should be the same, for it to run the same profile to finish it. That will not cause your problem though. There are only a couple of things I see that are weird, to me.

1) It is customary to incorporate your G40 into the last line of your tool path. In this case, you would just move the N22 to the line with the G40. That way, you do not need the redundant code following the G70. Again, this should not cause your problem.

2) Since you are getting a non-monotonous arc alarm, and there is only 1 line with an arc on it, I would look hard at that line. The thing that strikes me as odd here, is the arc itself. Either the arc is not tangent to the face and OD, or your math is not accurate. I see a -0.200 Z travel and a 0.200 radius...great! That would mean 0.400 X travel. Your X value should be at 1.950 for the arc to be tangent to both the face and the OD. This is based on a convex arc, which, in this case should be a G2, not G3. If the arc is to be concave, the G3 is correct, but then the start and end of it would not be perpendicular to the face and OD given your current dimensions.

I think the path is giving you the alarm because of the "Type" of turning operation selected, combined with the current concave radius. In using G71, there are two different styles of turning: Type I and Type II.

You are using Type I, which means prior to the G71, you called a G0 X and a G0 Z, both on separate lines. This means that the tool path must always move in the same direction as what you start. So if the first move in Z is negative, it must always move negative through the G71. If the first move for X is positive, it must always move positive through the G71. In this case, because you have a concave radius that is not perpendicular to the face of the part, and the radius is small enough, it is causing the tool path to move in an X negative direction to make the radius. Since you are using Type I, it is non-monotonous because the X direction will change from positive to negative.

If you use Type II, you would have to combine your G0 X and Z values to the same line. That will tell the control that it is OK to change directions in either X or Z. In this case, try combining yours to G00 X2.5 Z0.100, prior to the G71. I think you will see that it WILL run, but you may not like the way the radius looks compared to what you may be trying to do.

Good luck to you! We need more CNC machinists and programmers in this country, so stick with it!

Mike

you guys have been great! thank you all for the advice. I'm going back over all my math right now and I'm 98% certain that gizmo_454 is right on the money my 604 non monotonous arc problem. Thanks guys! Feels good knowing I have an entire clan of experts here to help me further trouble shoot any problems I may have further down the road in my career as a machinist! Hope yaw'll have a good weekend!

https://youtu.be/0_GiMspK0pc

In the first line of the G71 "N11 add a Z value, can be current position.


Sent from my iPhone using Tapatalk