[cruizer67]

Hello
Does anyone here have a Doosan Puma VTR (vertical lathe) with Live tooling. We are purchasing a VTR1216M and I am trying to prep Programs for it in advanced so that we can hit the floor running one it gets here. We use Mastercam for programming so the general turning part of a program is not a problem. What i need help with is understanding how the tool call out is it's a little bit different because of the quad tool holders

I have a sample program that was sent from the manufacturer.
I know most of these codes but can't figure out the

there is a bit of a learning curve for me so i am trying to get a jump start on my own so i know where i will need to focus my attention.

As always i appreciate any and all information you can supply.

thanks



*M481* ??

N10(OD R-TURN D432.)
G0G18G40G80G99
G55(Z=1057.3)
G28U0W0.
M481(0-INDEX)
(M6T3)
M34
M6T0800(X335.440 Z0 R1.6 T3)
M43
T0807
G50S100
G97S15M3P11

or here, how the q setter gets called out should be a M77(I thought) although the M37 could be the code for that (M76 puts the arm away)
also M483 what is it doing? it is rotating the quad holder

N15(Q-SETTER)
M483(180-INDEX)
M6T1000
G0X2660.0
T1004
G40
G0X2639.5
G0Z-105.0
G37Z-137.8
G4U1.0
G98G01W5.0F1000.0
M76
G28U0
G28W0
M1

[Dale123]

Each turning tool has 4 index positions.
M481 – Index position 1
M482 – Index position 2
M483 – Index position 3
M484 – Index position 4

So for Example if the quad tool is in station 1 then M6T0100 will call it into the spindle . Then M481 for position 1 etc .
If you want to then set the offset command T0101 for offset 1 and then set the tool off the Q Setter. You will need 4 different offsets per quad tool.

M77 is Tool Setting Arm out but it is missing from your example . One other thing is when setting the tool and the button is depressed , the X Axis must be over reference as the ATC door automatically opens to allow clearance on the tools when using the Q Setter

G37 is a Skip move in Z so when it hits the sensor it will stop and set the value .

G36 is the corresponding move in X

M35 engages C Axis
M34 turning Mode .

Spindles are designated P11 for turning spindle and P12 for Milling spindle .

[cruizer67]

Thank you very much that explains alot