Need Help!- Need help w/ Fanuc 18ti live tooling problem...

[bdyenter]

I have a problem. I am not able to move my C-axis in 90 degree increments in
the following program below. The drilling cycle will work but it seems I am missing something here. It does however index to C-O degrees but will not index to 90, 180, and 270. Can someone explain?

I am trying to drill and tap 4 M10 x 1.5 holes 1.250 deep.

(DRILLING CYCLE
T0909
M35
G28H0
G0X250.Z250.C0.
G98G97S2300M33
Z5.0
Z.1X5.0M8
G83Z-1.25R0.Q1000F5.M89
C90Q3000
C180Q3000
C270Q3000
G0Z2.
G80
G0X30.M9
Z20.
G80

[dcoupar]

Does it appear to tap the same hole 4 times?

Maybe you need a decimal point; C90. C180. and C270. Your control may be interpeting those as C0.090, C0.180, and C0.270... just a thought.

[cnc-king]

Originally Posted by dcoupar Does it appear to tap the same hole 4 times? Maybe you need a decimal point; C90. C180. and C270. Your control may be interpeting those as C0.090, C0.180, and C0.270... just a thought.

you are correct. fanucs will read his numbers that way if there is no decimal point because the control will add a decimal point after 4 places if none is defined

[dcoupar]

I believe that parameter 3401 bit 0 (DPI) affects how commands without decimal points are treated. But I never heard back from 'bdyenter' if that in fact WAS the problem.

[GERASIMOS]

Try this...(an example 4 M10 threads in 20mm depth at a diameter 100)
------
GOX300Z100C0
G97S1280M33
G0Z8
X100M8
G83Z-20R-5Q1000F0.1H90K4M89.
G0Z15
X300Z100M9
G80
It works perfect in a puma 600LM .
Be carefull the first hole is in 90 deg.(NOT IN 0 DEG)and the last in 360 deg.
and for rigid taping
try this

-------
G97S318M33
GOX100Z10C0
M29S318(This enables the rigid mode)
G84Z-17R-3F1.5H90K4M89
GOZ15
X300Z100
G80
Try it with a generous 0FFZ correction first time.Dont need any special tapping collet.A good R-8 is ok.Try in single block mode once.The machine go to x100z10c0 and the tap rotates.then the tap stops.after that the machine moves - 3mm in z axe.At this point the tap starts rotate and move to point z-17 in controled condition.then the tap stops rotating motion and moving together.After that the tap rotates anticlockwise and moves
back to the point z7and stops again.(note that the first thread is in 90 deg and the last in 360 deg.) you can not break any tap!!!

[dcoupar]

HEY BDYENTER! You kick the bucket or something? How about a little feedback? Feels like I'm talking to my wife or a wall or something...

[bdyenter]

Sorry fella's. I was on vacation. I appreciate your help. It was a mix of two different problems.

1) First... yes you were indeed correct that C90 needed to be C90. with a decimal point. That did infact fix the problem with rotating to the correct degree point.

2) My other problem that I found was that I did not use an M90 to unclamp before the chuck would index 90 degrees. After I changed these two items, It worked perfectly.

Thanks for all your help guys. Sorry I did not reply right away. Wont happen again.

Bdyenter

[manoharan]

You are right some machine should unclamp before rotating table to any degree. Before turn table unclamp block need.

[dcoupar]

bdyenter,

I believe if you put the M89 in the G83 block, it should unclamp automatically when it reads a new axis command (C90., for example). Check parameter #5110. It should be 89, IIRC.

Dave

[dcoupar]

Does your machine have a sub-spindle? If so, you should have these macros in the control to set prm #5100 to 89 for main spindle and 189 for the sub-spindle.

O9001(M289 5110=89)
#3003=1
G10L50
N5110R89
G11
#3003=0
M99

O9002(M389 5110=189)
#3003=1
G10L50
N5110R189
G11
#3003=0
M99

[cncjcl]

G83 Z-2.0 R-.5Q1000F0.1H90.K4M89
H= deg to next hole
K= number of holes
That should work for z axis drilling

G87 if you wanted todrill in the x axis