Help with new program

[gbowne1]

First of all on the G92 thread.. my book on G parameters says G92 is:

G92: Preset Absolute Registers. This enables the zero datum position to be changed as part of the program, during the running of the program.

Anyhow, here's my problem. This is my program.

N1 G21
N2 G95
N3 G00 X54. Z20. T00
N4 G00 X100.8 Z25.9 T00
N5 T01
N6 G97 S100
N7 X0 Z4.5 M03
N8 G01 Z0.8 F1.
N9 G00 X100.8 Z25.9 T00
N10 T02
N11 G97 S800
N12 X52. Z0
N13 G01 X-2 F0.2 M08
N14 G00 X100.8 Z25.9 T00
N15 T03
N16 G97
N17 X50.
N18 Z1.
N19 G01 X53.2 Z2.6 F0.2
N20 X47.2
N21 Z-65.
N22 X50.
N23 Z-67.
N24 X53.2
N25 G00 Z2.6

M00

This is a FANUC 6 program in Word Addressed format for a part called a "Pin" I'm using Mastercam and may change to BobCAD/CAM.

Is there a better way to do this program?

[Ozemale6t9]

Hi,

As most people here will agree, you would be much more likely to get help with this problem if you included a detail drawing of the part. It is hard to understand what you are trying to achieve from your program.

regards, Oz

[gbowne1]

Ok :-) That's noted.. I'm still working with AutoCAD 2005 and goin to come up with a much more detailed drawing of the part that I have.

My machine has a BTR and I'm doing some basic programming with this.

I still have to program in the Magic 3 method. I tried this program with several different speeds with a G97 spindle speed selection.

My machine has both the linear and circular interpolation modes. I'm also able to turn on G71 metric. It's a Boxford machine converted to Fanuc from the Audit control. It's held in a collet chuck with no parting operation.

The first example was 50mm dia 500mm long. I had to reduce the size per a customer request, but the part still has the same details. The front end of the part has a M10x1.5 thread and behind that a 2mmx1.5mm undercut. From there it's got a 60deg taper to 20mm for a lenght of 25mm. Then it goes straight and level for 45mm, to a 10mm radii, out to 40mm, and then straight for 65mm to a shoulder on the 50mm dia.

The second example part that goes with this pin, a different pin. Mild Steel round bar, 30mm dia x 100mm long. Similar program.

My problem occurs when going for the taper and the 10mm radii. It doesn't do exactly what the program calls for.

Greg

[tobyaxis]

Looks like your Lathe Program needs a little spit and polish. When you call a tool in a lathe T01 is correct, but you forgot the offset T0101 will call T01 and offset 01. Depending on how old you control is you may have to set a G50 X and Z for all your tools. Here is an example of a Fanuc 6T from a 1984 Ikegai FX25N. Do not forget to set the Tool Tip Designation. Without it you can't use G41/G42. For quick reference a standard right hand turning tool CNMG 432 will use Tip "3" . A right hand boring bar will use Tip "2" . There should be a list in your manual for Tool Nose Radius Compensation.

%
O1154
(IKEGAI FANUC 6T)
(DRWNG=ABPLC1.CAD)
(MATERIAL=SAE 1018)
(5.0D 1.075L)
(OP1)
(DATE 1/15/04 PGMR TJD)
(DATE REV 1/15/04)
(LAST RUN)
(T1=CNMG432 VALENITE SV330 T3)
(T2=DRILL 1.0D INDEX)
(T3=DNMG431 SECO FF1 CM T3)
(T4=B-BAR .5D CCMT21.51-F2 TP1000 T2)
(T5=B-BAR 1.0 D .0312R T2)
(JAWS=400 PRESS=18)
(CYCLE TIME= MS)

G0 G40 G97 G99 M5
G28 U0 W0 M9
G50 S2000 M39 >>>>>>>>>>>>>>>(This G50 sets Max Spindle speed SFM)
M1

N1(R-FACE/TURN)
G28 U0 W0
T0100
G50 X(RP) Z(RP) M8 >>>>>>>>(The RP stands for Relative Position)
G96 S900 M3
G0 X5.2 Z.2 T0101
G72 P10 Q11 W.005 D400 F.008
N10 G0 G41 Z0
N15 G1 X0 F.004

G0 G40 X5.2 Z.1
G71 P20 Q25 U.02 W.005 D1000 F.01
N20 G0 G42 X4.765
G1 X4.985 Z-.01 F.0025
Z-.75 F.004
N25 X5.2 F.0035

G0 G40 Z.1 M9
G0 X(RP) Z(RP) T0100
G28 U0 W0
G97
M1


N2(DRILL)
G28 U0 W0
T0200
G50 X(RP) Z(RP) M8
G97 S2400 M3
G0 X0 Z.2 T0202
G1 Z-1.125 F.0025
Z.05 F.2

G0 G40 Z.1 M9
G50 X(RP) Z(RP) T0200
G28 U0 W0
G97
M1

N3(F-FACE/TURN)
G28 U0 W0
T0300
G50 X(RP) Z(RP) M8
G96 S1000 M3
G0 X5.2 Z.2 T0303
G70 P10 Q15

G0 G40 X5.2 Z.1
G70 P20 Q25

G0 G40 Z.1 M9
G0 X(RP)Z(RP) T0300
G28 U0 W0
G97
M1

N4(R-BORE)
G28 U0 W0
T0400
G50 X(RP) Z(RP) M8
G96 S400 M3
G0 X1.0 Z.1 T0404
G71 P40 Q45 U-.02 W.02 D320 F.0075
N40 G0 G41 X4.6628
G3 X1.975 Z-.3 R2.5 F.0035
G1 X1.875 Z-.35 F.0025
Z-.43 F.004
X1.518 F.0035
X1.483 Z-.455 F.0025
Z-.9 F.004
N45 X1.0 F.0035

G0 G40 Z.1 M9
G0 X(RP) Z(RP) T0400
G28 U0 W0
G97
M1

N5(F-BORE)
G28 U0 W0
T0500
G50 X(RP)Z(RP) M8
G96 S550 M3
G0 X1.0 Z.1 T0505
G70 P40 Q45

G0 G40 Z.1 M9
G0 X(RP)Z(RP) T0500
G28 U0 W0
G97

M30
%

This one is a Dainichi BX45 Slant Fanuc10T

%
O1154;
(ANTI-BALLOONING PLATE);
(DRWNG=ABPLC1.CAD);
(MATERIAL=SAE 1018);
(5.0D 1.075L)
(OP1);
(DATE 1/15/04 PGMR TJD);
(DATE REV 1/1504);
(LAST RUN);
(T1=CNMG432 HORE. T3);
(T3=DNMG431 HORE. T3);
(T5=DRILL 1.0 INDEX T0);
(T7=B-BAR .5 D METAL .0156R T2);
(T9=B-BAR 1.0 D .0312R T2);
(JAWS=400 PRESS=18);
(CYCLE TIME=M S);
;
G0 G40 G97 G99 T0 M5;
G28 U0 W0 M9;
G50 S2000 M41;
M1;
;
N1(R-FACE/TURN);
G28 U0 W0 T0;
T101 M8;
G96 S475 M4;
G0 X5.2 Z.2;
G72 P10 Q11 W.003 D350 F.008;
N10 G0 G41 Z0;
N11 G1 X0 F.004;
;
G0 G40 X5.2 Z.1;
G71 P20 Q30 U.02 W.005 D600 F.01;
N20 G0 G42 X4.765;
G1 X4.985 Z-.01 F.002;
Z-.75 F.004;
N30 X5.2 F.003;
;
G0 G40 Z.25 M9;
G28 U0 W0;
G97;
T0;
M1;
;
N2(F-FACE/TURN);
G28 U0 W0 T0;
T303 M8;
G96 S650 M4;
G0 X5.2 Z.2;
G70 P10 Q11;
;
G0 G40 X5.2 Z.1;
G70 P20 Q30;
;
G0 G40 Z.2 M9;
G28 U0 W0 M5;
T0;
M1;
;
N3(DRILL);
G28 U0 W0 T0;
T505 M8;
G97 S2400 M3;
G0 X0 Z.25;
G1 Z-1.25 F.0025
Z.25 F.2;
;
G0 Z1.0 M9;
G28 U0 W0 M5;
G97;
T0;
M1;

N4(R-BORE);
G28 U0 W0 T0;
T707 M8;
G96 S300 M4;
G0 X1.0 Z.1;
G71 P40 Q50 U-.02 W.02 D300 F.007;
N40 G0 G41 X4.6628;
G3 X1.975 Z-.3 R2.5 F.003;
G1 X1.875 Z-.35 F.002;
Z-.43 F.004;
X1.518 F.003;
X1.483 Z-.455 F.002;
Z-.9 F.004;
N50 X1.0 F.003;
;
G0 G40 Z.2 M9;
G28 U0 W0;
G97;
T0;
;
N5(F-BORE);
G28 U0 W0 T0;
T909 M8;
G96 S400 M4;
G0 X1.0 Z.1;
G70 P40 Q50;
;
G0 G40 Z.1 M9;
G28 U0 W0;
G97;
T0;
;
M30;
%

The differences are on how the tools are set. The Ikegai uses the old method of G50 X and Z Reference Positions. The Dainichi uses a newer method in a Tool Geometry Page setting all tools to one Zero point of T3 (finish tool).
You will have to excuse all of the EOB's.

[tobyaxis]

First of all on the G92 thread.. my book on G parameters says G92 is:

G92: Preset Absolute Registers. This enables the zero datum position to be changed as part of the program, during the running of the program.

Anyhow, here's my problem. This is my program.

N1 G21
N2 G95
N3 G00 X54. Z20. T00
N4 G00 X100.8 Z25.9 T00
N5 T01
N6 G97 S100
N7 X0 Z4.5 M03
N8 G01 Z0.8 F1.
N9 G00 X100.8 Z25.9 T00
N10 T02
N11 G97 S800
N12 X52. Z0
N13 G01 X-2 F0.2 M08
N14 G00 X100.8 Z25.9 T00
N15 T03
N16 G97
N17 X50.
N18 Z1.
N19 G01 X53.2 Z2.6 F0.2
N20 X47.2
N21 Z-65.
N22 X50.
N23 Z-67.
N24 X53.2
N25 G00 Z2.6

M00

This is a FANUC 6 program in Word Addressed format for a part called a "Pin" I'm using Mastercam and may change to BobCAD/CAM.

Is there a better way to do this program?

Does your machine control have G76? You may be better off using G76 in place of your G92. As a note both suport Tapered Threads with "I" designation in radius form.

[gbowne1]

I saw that G45 thru G52 are available for Tool comp / offset. I don't have anything with a real large nose radii. I always try to use 7deg positve rake inserts.

I normally use G92.. but.. I didn't see the others.. like G72 through G78 are not referenced in my manual.

I was more inclined to include the G81 rapid cycle. Possibly a G87 chip breaking cycle and a G33 for the thread/screwcutting, and at last probably G43 positive offset.

I added a .txt file of the output of the program done the other way around, which might be better. I thought there might be changes because of the TTRC preset in lines N0135-N0145 and then adding lines from N0165 to N0172.

There's also a puzzle in here because there cuold have been a:

N03 G02 X+/-042Z+/-042 I042 K042 F04 S4 T03 M02* (done in tape format)

in this program.

I also thought of a G04 Dwell.

The actual 2nd operation should be adjusting to a stop

X= centerline Z=end face. My tool material is cemented carbide.

Greg

[tobyaxis]

I saw that G45 thru G52 are available for Tool comp / offset. I don't have anything with a real large nose radii. I always try to use 7deg positve rake inserts.

I normally use G92.. but.. I didn't see the others.. like G72 through G78 are not referenced in my manual.

I was more inclined to include the G81 rapid cycle. Possibly a G87 chip breaking cycle and a G33 for the thread/screwcutting, and at last probably G43 positive offset.

I added a .txt file of the output of the program done the other way around, which might be better. I thought there might be changes because of the TTRC preset in lines N0135-N0145 and then adding lines from N0165 to N0172.

There's also a puzzle in here because there cuold have been a:

N03 G02 X+/-042Z+/-042 I042 K042 F04 S4 T03 M02* (done in tape format)

in this program.

I also thought of a G04 Dwell.

The actual 2nd operation should be adjusting to a stop

X= centerline Z=end face. My tool material is cemented carbide.

Greg

G43 is for setting Height offset (G43Z1.0H01) in Mills. As for the program it looks like an old Ikegai format that I'm not acustom too.

[gbowne1]

This is the program format I learned when I started working with the machine. It could be that Ikegai wrote their standards for this machine and control. There were already similar programs stored in the machines memory.

Any other ideas?

Greg

[tobyaxis]

No idea. I'd have to see the Machine, Control and Manual. Sorry

[gbowne1]

Thanks for tryin'!

I'm goin' to keep pluggin along.

Greg