[ginner]

Hey guys,

Running my VMC15xt mostly thanks to the advises from you guys. It runs ok, finished few jobs and things seem ok.

Got a question - after the tool change, the tool goes to z=0, and later it goes to xyz that I programmed. If the tool change occures, for example, above the fixture setup, it might crash my cutter or worse. Something like that happens when I execute the program via DNC - only, if the tool number in g code is the same as the tool no. in the spindle - then the tool goes to tool exchange height, does nothing (because it's the same tool no.), then goes to z0, and then to programmed z coordinate.

What am I missing? Some first lines or some commands after the tool change in my g code, some parameter setup?

Thanks a lot!!!

[rodney247]

Are you running in Format 1 or Format 2 ...... Format 1 is the "FADAL" format = very safe and simple operation with the machine.... everytime a program stops it will return to defaults nothing stays Modal. Format 2 is the "FANUC" format.... acts more like a Fanuc machine retains things Modal if it is called up in a program it continues to run even after you exit the program like a G54 fixt 1 will stay active.... or G90.... or G0 etc... Anyways long story in Format 1 the machine will be safer in a sense...Nothing wrong with Format 2 but your post has to be correct or crashes will be common....... the Formats are in the SETP first page.

simple program is

N87T3M6
N88* OPERATION 4: HOLES
N89* DXF LAYER 'CK_LEVEL_1'
N90* TOOL 3: .25 DRILL
G90G0G17G80*safe line
N91S1400M3
N92G17G90G0X-4.0532Y-.0872E1
N93Z.1H3M7
N94G83G98X-4.0532Y-.0872Z-.75R0.1Q.3125F4.
N95G0G80Z.1
N96G0G90M5M9
N97G53Z0
N98M1
N99T4M6

[ginner]

Are you running in Format 1 or Format 2 ...... Format 1 is the "FADAL" format = very safe and simple operation with the machine.... everytime a program stops it will return to defaults nothing stays Modal. Format 2 is the "FANUC" format.... acts more like a Fanuc machine retains things Modal if it is called up in a program it continues to run even after you exit the program like a G54 fixt 1 will stay active.... or G90.... or G0 etc... Anyways long story in Format 1 the machine will be safer in a sense...Nothing wrong with Format 2 but your post has to be correct or crashes will be common....... the Formats are in the SETP first page.

simple program is

N87T3M6
N88* OPERATION 4: HOLES
N89* DXF LAYER 'CK_LEVEL_1'
N90* TOOL 3: .25 DRILL
G90G0G17G80*safe line
N91S1400M3
N92G17G90G0X-4.0532Y-.0872E1
N93Z.1H3M7
N94G83G98X-4.0532Y-.0872Z-.75R0.1Q.3125F4.
N95G0G80Z.1
N96G0G90M5M9
N97G53Z0
N98M1
N99T4M6

It runs in format 2. I assumed that was one of the possibilities - I recently bought it and started working on it. I guess that's why in a drilling cycle it goes hole to hole to hole in G1 with drilling feed instead of G0.

Previous owner (some school) must have set things like that and the modal commands remained. I will try with the format 1.

Thank you very much!

[Beltdrive]

I like using format 2
For tall parts or long tooling a typical program might go like this

With Z fixture =0
Tool 0s= surface to be drilled

G0G90G80X-5.Y0E1 (Safe location to change tools)
T1M6 (.25 DRILL)
H1Z3. E1 (G43 isn't needed)
S1200M3
G0G90X1.Y1.M8
G73G98R0+.1Z-1.5Q.1P.02F4.
X2.
X3.
X4.
Y2.
X3.
G80M9
G0G90X-5.
M6
M30

An M6 with out a tool number will:

Shut off spindle M5
Shut off coolant. M9
Take Z to tool change. G53 Z0
Orient spindle. M19

[ginner]

I like using format 2
For tall parts or long tooling a typical program might go like this

With Z fixture =0
Tool 0s= surface to be drilled

G0G90G80X-5.Y0E1 (Safe location to change tools)
T1M6 (.25 DRILL)
H1Z3. E1 (G43 isn't needed)
S1200M3
G0G90X1.Y1.M8
G73G98R0+.1Z-1.5Q.1P.02F4.
X2.
X3.
X4.
Y2.
X3.
G80M9
G0G90X-5.
M6
M30

An M6 with out a tool number will:

Shut off spindle M5
Shut off coolant. M9
Take Z to tool change. G53 Z0
Orient spindle. M19

Thanks, a lot! I am not by the machine, cant wait to try again!