Blueprint Programming fanuc 18T

[adamant]

I get a lot of 041 alarms in my programs when using tool comp........G41.....G42.....

Drives me crazy some times trying to figure out why the darned thing won't just run what I tell it too.

Here is my latest stab at a simple G71 canned cycle..........

I'm wondering if the ,R.054 will run in a block all by itself the way I have written it.

I'm at home and don't have a good simulator for fanuc 18T turning.

T0101 G96 S1000 M14
G0X.55Z.1
G71U.02R.01
G71P21Q22U10W10F.003
N21G1 X0 F.001
,R.054
X.169 Z-.370 ,R.370
Z-1.4
X.55
N22 G0 Z.1
M98P1
M1
N3 (FINNISH)
M98P1
T0202 G96 S1000 M13
G70 P21 Q22
M98P1
M1

[hatchmar]

I am at home too but i think when i get an 041 alarm happens when you try to restart a cycle while the machine is still in cutter comp mode. if you stop in the middle of a cycle and it doesnt get a chance to execute the G40 C/C Cancel it gets confused. im not positive but thats what happens on my Miyano with OT control.

As for the G71: does this work? im not familliar with the commas

T0101 G96 S1000 M14
G0X.55Z.1
G71U.02R.01
G71P21Q22U10W10F.003
N21 G0 X.55
G1 X0 R-.054 F.001
X.169 Z-.370 ,R.370
Z-1.4
X.55
N22 G0 Z.1
M98P1
M1


Also, If you plan on using this tool to get your finish dim. you should have
G70P21Q22 after your N22. this tells it to take the final finish profile pass.

[hatchmar]

oops- i didnt see the last part of your proggie- forget the G70 thing i said

[Gunner]

I'm not super familiar with the 18T control but I had some thoughts on this. Using cutter comp is the way to go. You don't have to fudge numbers to get what you want. What is the radius of the insert you are using? Do you have the radius plugged into the R value on your tool offset page? Do you have the correct T value for the quadrant your cutting in? I don't see where you are calling the cutter comp in your program. Normally we use G41 for ID work and G42 for OD when working on the main spindle. This looks like your contouring an OD. I'd use a G42. As an example, if I were using a DNMG 432 insert to turn the OD I'd have .031 plugged into the T value on the offset page for tool 1 and T3 for the quadrant. I'd also call up my cutter comp after the face cut during the positioning of the tool prior to calling up the canned cycle. Remember to cancel the cutter comp before you call up your next tool.

[adamant]

Hey Gunner, hatchmar

You are correct. I don't see the cutter comp there either.

I'm getting used to the machine and control. Things are going a lot smoother. A lot of learning CNC is just putting in the hours.

Thanks for your replies.

adamant

[geach73]

If you are using the roughing tool for your finish pass you need to call cutter comp before the G71 P100 Q200;

lIKE THIS
STOCK DIA= 1.250

GOO X1.200 Z.125 ;
G01 G42 X1.250 Z.100 F.010;
G99;
G71 U.150 P.025;
G71 P100 Q200 U.010 W.005 F.008;
N100 GOO (MACHINE THE WORK PEICE)
;
;
;
;
;
N200 X 1.250;
G00 Z.100;
G70 P100 Q200;
G30 U0.0 W0.0 T0
G97 G40 (G40 CANCELS CUTTER COMP AND G97 CANCELS SFM);
M01;


IF USING ANOTHER TOOL FOR FINISHING CALL THE CUTTER COMP BEFORE YA CALL THE G70 P100 Q200;

[extrem89]

N1(ROUGH TURN)
G97 S1200 M14
M98 P1
T0101
G50 S5500
G96 S1000
G0 X.550 Z.100
G71 U.020 R.010
G71 P21 Q22 U.010 W.010 F.008
N21 G0 X0
G1 G99 Z0 F.OO8
X.169 Z-.370 R-.370 F.003 (I dont think fanuc control uses coma's)
Z-1.400 F.005
X.550
N22 G0 Z.100
M98P1
M1
N2 (FINISH TURN)
G97 S2500 M13
M98 P1
T0202
G50 S5500
G96 S1000
X.560 Z.300
G1 G42 X.550 Z.100 F100. (Depending on your nose radius , how much you move)
G99
G70 P21 Q22
M98P1
M1
M30

[positiverake]

The comas are for blue print programing,a bit strange but it does work nice,why not let the machine do the math,it will figure out a radius into a angle and things like that,real nice with the cutter comp