Okuma Mill variables

[jeff]

OSP700M control,

Does anyone know if it's possible to have a variable expression to check the current spindle tool # and if it's not the right one,change tools?

 

Something like this:

IF [sPINDLE TOOL] >1 THEN [T1M6]

 

I'm looking to dummy-proof our programs a little bit more.

Thanks

[35K chipper]

Jeff,

This is what we use. You must have user task 2 option. Vatol is the tool in the spindle. If it is

it will jump the tool change. If it's not it will

make the tool change. You need this at the start of every tool.

Hope this helps

35k chipper

 

(NEXT TOOL NOT ACTIVE)

(PGM Z MAX Z.1)

(PGM Z MIN Z-.227)

G0G90G80G40G17G94

N10

IF [VATOL EQ 10] N121

T10M6

N121

(.03125 DIA. 15 DEG. 2 FLT. TAPER)

[jeff]

Thanks 35K Chipper,

thats exactly what I was looking for.

[jeff]

Thanks for the help!

This is what I ended up doing:

$PROGNAME.MIN%

IF[VATOL EQ 1]GOTO N1

IF[VATOL GT 1]GOTO N2

N1G00Z20.

X-20.

T1M6

N2

N100(FINISH FLOWLINE)

BLAH BLAH BLAH

M30

%

[Lathe-Mill]

jeff, my post was custom to work that way, pre-stage tooling..do you have the 30 tool carrussel and quick tool change arm?

 

( 22943-03 REV.B - OP.#4 )

(PROGRAMMED BY JUAN C. GARCIA - FEB -16 -05 -11:34 )

N1 G90 G80 G40 G0 G17

IF [VATOL EQ 19] NT19

N2 T19 M6

( OKUMA - 1/4 FLAT ENDMILL )

( SPOTFACE 1 PLC. )

NT19 G0 G90 G15 H10 X-.25 Y0. A-180. S1500 M3

N3 G56 H19 Z4.8 T1 M8

N4 G71 Z4.8

N5 G81 Z3.75 R4. F3. M53

N6 G00 Z4.8

N7 M9

N8 G0 Z40.

IF [VATOL EQ 1] NT1

N9 T1 M6

N10 M1

( OKUMA- 1/4 SPOT DRILL )

( SPOT 1 PLC. )

NT1 G0 G90 G15 H10 X-.25 Y0. A-180. S3500 M3

N11 G56 H1 Z4.8 T28 M8

N12 G71 Z4.8

N13 G81 Z3.7 R4.05 F10. M53

N14 G00 Z4.8

N15 M9

N16 G0 Z40.

IF [VATOL EQ 28] NT28

N17 T28 M6

N18 M1

( OKUMA - 1/8 DRILL )

( DRILL 1 PLC. )

[jeff]

Lathe-Mill,

Our machiine is the MX55VB with 32 tools and an arm.

I'm curious though,why do you have it before every toolchange?Is that so you can start anywhere in the program and it will call up the correct tool?

After taking a closer look at your program,how can that not alarm on you?

It seems like it's checking to see if T19 is in the spindle and if it is,NT19????

My control would give me an alarm saying "Wrong T command".

Also do you know the M code to clear out the staged tool?Say you have T2 next in line,and if I call out another T,I get an alarm unless I go into manual and reset the ATC cycle.

[Lathe-Mill]

I'm curious though,why do you have it before every toolchange?Is that so you can start anywhere in the program and it will call up the correct tool?>>>>>>this is correct

tool 19 is in the spindle and as you see, tool 1 is next on line. pre-stage tool

[35K chipper]

Jeff,

This one is for a machine with tool pre-stage.

The block skip will save time when you cc the part

to size.

 

35K Chipper

 

(MAKES 1 PART WITHOUT SUBS)

(NEXT TOOL ACTIVE WITH / OFF)

(PGM Z MAX Z.1)

(PGM Z MIN Z-.635)

G0G90G80G40G17G94

N1

IF [VATOL EQ 1] N1510

M121

T1M6

M9

N1510

(4.00 6FL DMND SHELL MILL)

(FACE FRONT)

G131J2I0

(MAX Z.1)

(MIN Z0.)

/T15 (IS THE NEXT TOOL)

G0G90G15H1X-7.6264Y-2.0186S10472M3

G56H1Z.1M8

Z.05

G1Z0.F100.

G42D1X-5.1267Y-1.975

G2X-5.125I.0017J-.1

G1X5.125

G2X5.1267I0.J-.1

G40G1X7.6264Y-2.0186

G0Z.1

(FACE BACK)

G131J2I0

X-7.6264Y2.0186

Z.05

G1Z0.F100.

G41D1X-5.1267Y1.975

G3X-5.125I.0017J.1

G1X5.125

G3X5.1267I0.J.1

G40G1X7.6264Y2.0186

G0Z.1

M9

G0G30P1M5

G130

M1

 

N15

IF [VATOL EQ 15] N15131

M121

T15M6

M9

N15131

(.375 STUB CBD S POINT)

(DRL .375)

G131J2I0

(MAX Z.1)

(MIN Z-.5477)

/T13 (IS THE NEXT TOOL)

G0G90G15H1X-2.3601Y-.1907S10800M3

G56H15Z.1M8

G71Z.1

G81X-2.3601Y-.1907Z-.5477R.05F80.M53

Y.1907

X-2.0298Y0.

X0.

X2.1399Y-.1907

Y.1907

X2.4703Y0.

G80M3

M9

G0G30P1M5

G130

M1

[jeff]

Thanks 35K Chipper,

It's always interesting to see how other ppl do stuff.

[connormac]

This is what is in my post,

 

if next_tool<>t,n,*next_tool,e

 

hth

[connormac]

You can always add block delete to that also.

[jeff]

connormac,

If I read that right,that won't work for what I wanted to accomplish.

 

I added this in my post so the button pushers can change tooling and start a new part no matter what tool is in the spindle.

And it also moves up and away just to make sure it doesn't crash.

 

$PROGNAME.MIN%

IF[VATOL EQ 1]GOTO N2

IF[VATOL GT 1]GOTO N1

N1G00Z20.

X-20.

T1M6

N2

N100(FINISH FLOWLINE)

 

If my starting tool is NOT T1 then I would just change it to something like this:

$PROGNAME.MIN%

IF[VATOL LT 17]GOTO N1

IF[VATOL GT 17]GOTO N1

IF[VATOL EQ 17]GOTO N2

N1G00Z20.

X-20.

T17M6

N2

N100(FINISH FLOWLINE)

 

Does anyone know the M code to cancel or "un-stage" the next tool?

Is it M121 like in 35K CHIPPERS' post above?