G71 Fanuc cycle poll/argue

[mystiks]

Ok, i want your opinion on this argument we seem to have on other thread.

Control is fanuc, and we're talking about cycle G71, and both (Type I/Type II) options installed on machine.

See attachment for profile (Only doing the white profile, ignore the two red lines)

And the profile starts from higher diameter ofc.

My claim was that if you dont give Z-movement on first line after the cycle, it would do the profile with 1 cut. And i'd even remember fanuc's own 2D simulation(Under the graph button) simulating this with 1 cut.

Just write what you think the machine would do in this instance. Thanks

[sinha_nsit]

Angelw does not agree with me, and I have not yet done further experimentation to verify what I believe, but this is what I think will happen:
It depends on the start X. If it is, say, X40, and the depth of cut in G71 is 0.25, then there would be two straight roughing cuts, the first at X39.5 and the second at X39. Thereafter, the step-removal pass of G71 would start, and the defined profile would be traced by the tool (assuming zero finishing allowances). If the depth of cut is, say, 1.0, then there would be no roughing pass, and the entire material would be removed in one pass. But, as I said, Angelw does not agree with me. So, I have to check.

If you have both types available, there is no reason to use type I at all. Type II has an additional advantage that it does not create steps in roughing. So, finish is likely to be better than type I. Therefore, even for monotonic increase/decrease in diameter, type II should be used.

Sinha

[mystiks]

Yep, but the Z is missing for reason =), and i'll be doing some experiments too on tuesday when i get back to work.

Hmms, and you are prolly right on those first two straight cuts, if the cut depth would be so small, remembering some old scene that almost happened =).

[angelw]

Originally Posted by sinha_nsit Angelw does not agree with me, and I have not yet done further experimentation to verify what I believe, but this is what I think will happen: It depends on the start X. If it is, say, X40, and the depth of cut in G71 is 0.25, then there would be two straight roughing cuts, the first at X39.5 and the second at X39. Thereafter, the step-removal pass of G71 would start, and the defined profile would be traced by the tool (assuming zero finishing allowances). If the depth of cut is, say, 1.0, then there would be no roughing pass, and the entire material would be removed in one pass. But, as I said, Angelw does not agree with me. So, I have to check. If you have both types available, there is no reason to use type I at all. Type II has an additional advantage that it does not create steps in roughing. So, finish is likely to be better than type I. Therefore, even for monotonic increase/decrease in diameter, type II should be used. Sinha

The attached pictures of a sample part similar to the program posted earlier, only using diameters that suited the material being used in the machine.

The first picture shows the part cut using G71 Type II.
The second picture shows the start of the first cut using G71 Type I. The same program was used with the Z move on the P line deleted.
The third picture show the part after the G71 Type I cycle had finished.

[sinha_nsit]

Angelw,
I believe, G71 is exactly same on all control versions of Fanuc.
Still, which version have you experimented with?
Sinha

[angelw]

Originally Posted by sinha_nsit Angelw, I believe, G71 is exactly same on all control versions of Fanuc. Still, which version have you experimented with? Sinha

I became aware of how G71 Type I reacts with a part program containing pockets when 6TB controls were current. I believe that this was the first Fanuc control that had Type II and therefore, capable of machining pockets.

The sample was machined on a Takasawa TS20 with an 11T control. Controls from "O" series on use two G71 blocks to define the cycle, in the same way that the screw cutting G76 does to pass its parameters. However, I don't think that the basic architecture or the cycle is different. The G71 cycle on the 10,11 and 12T controls have additional parameters compared to the two block version on later controls in that there is an I and K value to specify a rough-finish margin in addition to the finish allowance U and W.

I recall you asking in a different post whether cutter radius compensation is available in a G71 cycle. It is with 10,11 and 12T controls with some caution applied to the start and finish block of the part shape description. An override of the cutting depth in 1% units is also available by parameter set is also available with these controls. It allows the depth of cut to be varied without rewriting the value of D of the cycle. I'm not sure if this applies to current controls.

Regards,

Bill

[sinha_nsit]

I verified on 0i Mate TC.
This control does not have G71 type II cycle.
Type I runs exactly as I described. It does not spoil the part. Material in the valley is removed in one pass (the step-removal pass of G71). Dimensionally correct part is made, at least theoretically (because practically it is not possible to remove the entire material in the valley in one pass).

So, I guess, i-series controls behave differently from older controls.

Sinha

[angelw]

Originally Posted by sinha_nsit I verified on 0i Mate TC. This control does not have G71 type II cycle. Type I runs exactly as I described. It does not spoil the part. Material in the valley is removed in one pass (the step-removal pass of G71). Dimensionally correct part is made, at least theoretically (because practically it is not possible to remove the entire material in the valley in one pass). So, I guess, i-series controls behave differently from older controls. Sinha

In the case of the 11T the part is ruined, but the machine and tooling remains undamaged. In the scenario you describe there's the distinct potential for at least the tool, if not the machine to be damaged, and the part may be ruined in the process. It surprises me that a control designer would take what seems to be a backward step.

[sinha_nsit]

I agree with you.
The control should either ignore the valley or alarm out, if type I is being used.
We are not machining butter!
But, spoiling the part is not a good idea. G71 should correctly do as much as it can.

[amir65esf]

Originally Posted by angelw The attached pictures of a sample part similar to the program posted earlier, only using diameters that suited the material being used in the machine. The first picture shows the part cut using G71 Type II. The second picture shows the start of the first cut using G71 Type I. The same program was used with the Z move on the P line deleted. The third picture show the part after the G71 Type I cycle had finished. Attachment 120809 Attachment 120810 Attachment 120811

i have problem with g71 and type II. when i execute the program it returns "PS0329" would you please mail me the program that you execute successfully on fanuc oi d .
amir65esf@gmail.com

[amir65esf]

i have problem with g71 and type II.when i execute the program it returns "PS0329" . would you please mail me the program that you execute successfully on fanuc oi mate td .
amir65esf@gmail.com

[angelw]

Originally Posted by amir65esf i have problem with g71 and type II.when i execute the program it returns "PS0329" . would you please mail me the program that you execute successfully on fanuc oi mate td . amir65esf@gmail.com

PS0329 THE FINISHING IS NOT A MONOTONOUS CHANGE

The alarm indicates that concave forms (pockets) are contained in a profile being machined with G71 Type I. The selection of Type I or Type II is determined by the addresses programmed in the block referenced by the P address in the second G71 block.
1. If only X(U) is programmed, Type I will be initiated and change in the direction of X moves in the profile description is not allowed
2. If both X(U) and Z(W) are programmed, Type II will be initiated and up to 10 concave forms (pockets) can be programmed in the profile description.

Following is the program listing for the part shown in the attached picture.

Regards,

Bill



%
O1000
(55 DEG. 0.8RAD RH TURNING TOOL)
(ROUGH PROFILE AND FACE)
N1 G21 G40
G28 U0.0 W0.0
G50 T0101 S3500
G96 S250 M03
G00 X192.400 Z2.200 M08
G71 U3.000 R0.500
G71 P111 Q112 U0.500 W0.100 F0.25
N111 G00 X88.400 Z2.200 (OR W0.0)
G01 Z0.000 F0.20
G03 X100.000 Z-5.800 I0.000 K-5.800
G01 Z-30.666
G03 X99.652 Z-31.316 I-1.300 K0.000
G01 X80.000 Z-48.335
G01 Z-80.469
G01 X149.238 Z-115.088
G03 X150.000 Z-116.007 I-0.919 K-0.919
G01 Z-165.666
G03 X149.652 Z-166.316 I-1.300 K0.000
G01 X120.000 Z-191.995
G01 Z-215.000
G01 X186.400
G03 X190.000 Z-216.800 I0.000 K-1.800
N112 G01 X192.400
G00 Z2.200
G00 X92.000
G01 Z0.000 F0.25
G01 X-1.600
G00 Z2.200
G28 U0.0 W0.0 M09
M01
(55 DEG. 0.8RAD RH TURNING TOOL)
(FINISH PROFILE AND FACE)
N2 G28 U0.0 W0.0
G50 T0202 S3500
G96 S250 M03
G00 X92.000 Z2.200 M08
G01 Z0.000 F0.50
G01 X-1.600 F0.20
G00 Z2.200
G00 X192.400
G70 P111 Q112
M09
G28 U0 W0 M05
M30
%