live tooling gand m codes

[LIVVY111]

can any one tell me wheir to find a list of codes and their uses for a puma 400 live tooling only .........please

[dcoupar]

What control does it have?

[Jaguar]

Should be an 18 or 21 unless it is a new one.

Did you get a manual or training with the machine?

J

[dcoupar]

Should be an 18 or 21 unless it is a new one.

Did you get a manual or training with the machine?

J

I know what it SHOULD be, I asked what it IS. The codes are different if it's a new machine with a 0iT-D.

[LIVVY111]

What control does it have?

will find out exact control tomorrow but quite sure it is an 18itb

[LIVVY111]

Should be an 18 or 21 unless it is a new one.

Did you get a manual or training with the machine?

J

not got a manual , most programmes are their for me but some codes i dont understand

[dcoupar]

Maybe this will help. If you have specific questions, ask away.

[LIVVY111]

Maybe this will help. If you have specific questions, ask away.

thanks for that no doubt i will quiz youre knowledge in the near future!

[LIVVY111]

Maybe this will help. If you have specific questions, ask away.

it would help me if you could write a programme to drill and tap 6 equi spaced holes of nominal depth and pitch with explanations beside each code so i can grasp exactly what the machine is doing using the z axis

[mroy0404]

Maybe this will help. If you have specific questions, ask away.

Hello dcoupar

I have been doing some face drilling on the sub spindle of a 2006 Doosan 2000sy with Fanuc 18iTB control. Here is a sample of the code.
(TOOL - 9 OFFSET - 9)
(15/32" DRILL)
G55
T0909
G17G99
M135
M7
M190
G0A0.
G0X3.5Z-.25
G97S2500M33
G83Z.965R.15F.008M189
X4.5A-12.
X3.5A-24.
X3.6285A-43.66
X4.5A-60.
X3.5A-72.
X4.5A-84.
X3.5A-96.
X4.5A-108.
X3.5A-120.
A-144.
X4.5A-156.
X3.5A-168.
X4.5A-180.
X3.5A-192.
X4.5A-204.
X3.5A-216.
X4.5A-228.
X3.5A-240.
X4.5A-252.
X3.5A-264.
X4.5A-276.
X3.5A-288.
X4.5A-300.
X3.5A-312.
X4.5A-324.
X3.5A-336.
X4.5A-348.
G80
G0Z-.3
M9
M35
G28U0.
G28W0.
T0900
M30

The problem I have had is the spindle is only clamped with M189 for the first hole. If I add a M189 on the end on each block, the spindle gets clamped before the machine has moved fully to the commanded location and alarms out.
Is there a way to make the M189 wait until the machine has arrived at the programed location before it clamps?

[Jaguar]

You might want to try an M190 between moves as it is not advisable to do a rapid move with the sub spindle clamped.

J.

[dcoupar]

Hello dcoupar

I have been doing some face drilling on the sub spindle of a 2006 Doosan 2000sy with Fanuc 18iTB control. Here is a sample of the code.
(TOOL - 9 OFFSET - 9)
(15/32" DRILL)
G55
T0909
G17G99
M135
M7
M190
G0A0.
G0X3.5Z-.25M389 <----- add this command to set 5110 to 189
G97S2500M33
G83Z.965R.15F.008M189
X4.5A-12.M189 <----- add M189 to each block
X3.5A-24.M189
X3.6285A-43.66M189
X4.5A-60.
X3.5A-72.
X4.5A-84.
X3.5A-96.
X4.5A-108.
X3.5A-120.
A-144.
X4.5A-156.
X3.5A-168.
X4.5A-180.
X3.5A-192.
X4.5A-204.
X3.5A-216.
X4.5A-228.
X3.5A-240.
X4.5A-252.
X3.5A-264.
X4.5A-276.
X3.5A-288.
X4.5A-300.
X3.5A-312.
X4.5A-324.
X3.5A-336.
X4.5A-348.
G80
G0Z-.3
M289 <----- Add this to set 5110 back to 89
M9
M35
G28U0.
G28W0.
T0900
M30

The problem I have had is the spindle is only clamped with M189 for the first hole. If I add a M189 on the end on each block, the spindle gets clamped before the machine has moved fully to the commanded location and alarms out.
Is there a way to make the M189 wait until the machine has arrived at the programed location before it clamps?

If you check parameter 5110 I'll bet it's 89. When drilling on the sub-spindle with M189, parameter 5110 needs to be 189 for the sub-spindle to index properly between holes.

M289 runs macro O9001 which sets parameter 5110 to 89, and M389 runs macro O9002 which sets it to 189. So, before drilling on sub-spindle, command M389, and before drilling on main spindle, command M289.