Variable H read offset tool

[dcoupar]

Sure doesn't look like any Fanuc code I've ever seen... looks more like an Okuma.

[broby]

I agree with dcoupar, this code below, for example is DEFINITELY Okuma code specific!

-snip-
N0830 S324 M03 T1
N0840 G00 X-4.00 Y0.8750 G94
N0850 M327
N0860 VTMNO=2
N0870 G56 H=VATOL M08
N0880 G284 Z=0.4529 R2.0539 P0.5 F18.
N0890 M326
N0900 G00 Z7.00
N0910 X4.00 Y0.3750 G94
N0920 M327
N0930 VTMNO=2
N0940 G56 H=VATOL
N0950 G284 Z=0.717 R2.0539 P0.5 F18.
N0960 M326
N0970 G00 Z7.00
N0980 G80 M09
-snip-

With this in mind, and your previous indication that you were running a Fanuc controlled machine, I would guess you would be having lots of problems.
As far as your program goes there are lots of problems with the way you are calling up the tool length offset for each tool, but that statement is only true if you are using an Okuma control system.
I do not use any Mills with a Fanuc controller, but I am guessing that even on a Fanuc, your code would have problems running also.

You really need to tell up EXACTLY what controller you are trying to run this program on.
Regards
Brian.

[fdonosos]

I'm sorry is my mistake it is OKUMA.
Thanks

[broby]

Well I guess you have finally got one thing correct... BTW no way is the machine a Mori Seki, that would use a FANUC control system but I am guessing that you do actually have a Okuma MC50VA, but as for which control... OSP5000M, OSP5020M, OSP7000M OSPE100, P100, P200??? Can you actually figure out that the more accurate and informative your description of your problem the easier it is for us to help you?
But enough of that...


/GOTO N0010
CALL OFX20 Unable to know what is going on here, no listing
CALL OZOFZ XP1=16.85 YP1=05.57 ZP1=7.505 FON=1 ZPOS=0.500 same here...
$PRB=1 continuation of above line above...
CALL OZOFY YP1=04.64 XP1=16.500 ZP1=7.69 YP2=05.08 YP3=2.65 same here...
$ YP4=2.21 FON=1 YPOS=0 PRB=1continuation of above line above...
CALL OZOFX YP1=03.70 XP1=13.763 ZP1=7.69 XP2=13.323 XP3=19.44
$ XP4=19.8 FON=1 XPOS=0 PRB=0 continuation of above line above...
G30 P2 Positioning to P2
M01
N0010 G40 G90 G17 G15 H1 G15 H1= Select coordinate system 1
N0020 M06 T12 (2.00 DIA FACE MILL) Tool change To Tool#12
N0030 H1 M03 S900 T3 Pre Stage Tool 3
N0040 G00 X0.0 Y0.0 M08
N0050 G56 H1 Z3.5819 PROBLEM!! You are calling up Tool Length offset #1 but you have TOOL 12 in the spindle!! This should be G56 H12
N0060 G01 Z2.554 F10.7
N0070 Y1.9438
N0080 X-3.3973
N0090 G03 X-3.4973 Y1.8438 I0.0 J-0.10
N0100 G01 Y-1.9012
N0110 G03 X-3.3973 Y-2.0012 I0.10 J0.0
N0120 G01 X3.3927
N0130 G03 X3.4927 Y-1.9012 I0.0 J0.10
N0140 G01 Y1.8438
N0150 G03 X3.3927 Y1.9438 I-0.10 J0.0
N0160 G01 X-0.5
N0170 Y0.0
N0180 Z2.534
N0190 Y1.9438
N0200 X-3.3973
N0210 G03 X-3.4973 Y1.8438 I0.0 J-0.10
N0220 G01 Y-1.9012
N0230 G03 X-3.3973 Y-2.0012 I0.10 J0.0
N0240 G01 X3.3927
N0250 G03 X3.4927 Y-1.9012 I0.0 J0.10
N0260 G01 Y1.8438
N0270 G03 X3.3927 Y1.9438 I-0.10 J0.0
N0280 G01 X-0.5
N0290 Y0.0
N0300 Z2.514
N0310 Y1.9438
N0320 X-3.3973
N0330 G03 X-3.4973 Y1.8438 I0.0 J-0.10
N0340 G01 Y-1.9012
N0350 G03 X-3.3973 Y-2.0012 I0.10 J0.0
N0360 G01 X3.3927
N0370 G03 X3.4927 Y-1.9012 I0.0 J0.10
N0380 G01 Y1.8438
N0390 G03 X3.3927 Y1.9438 I-0.10 J0.0
N0400 G01 X-0.5
N0410 Y0.0
N0420 G00 Z20. M09
N0430 G30 P2
N0440 M01
N0450 M06 T3 (1.00 DIA END MILL) No need to specify T3 again, machine already has T3 ready to go.
N0460 H1 M03 S1000 T4 What is the H1 on this line for? NOT REQ, Pre-Stage tool #4
N0470 G00 X4.208 Y-3.022 M08
N0480 G56 H1 Z4.3934 Once again, you are calling up Tool length offset no1, Should now be G56 H3 as tool 3 is now in the spindle
N0490 Z2.7934
N0500 G01 X-4.456 F10.
N0510 G00 Z14.0
N0520 X4.208 Y3.095
N0530 G00 Z2.7934
N0540 G01 X-4.456 F10.
N0550 G00 Z20.0 M09
N0560 G30 P2
N0570 M01
N0580 M06 T4 (SPOT DRILL 0.500")
N0590 H1 S2500 M03 T2 ditto for last tool change
N0600 G00 X-4.00 Y0.8750 M08
N0610 G56 H1 Should be G56 H4
N0620 G81 Z3.363 R4.439 F28. P.2
N0630 G00 Z20.00
N0640 X4.000 Y0.375
N0650 G56 H1
N0660 G81 Z3.363 R4.439 F28. P.2
N0670 G00 Z20. M09
N0680 G30 P2
N0690 M01
N0700 M06 T2 (DRILL 0.265INCH OR F HOLE)
N0710 S800 M03 T11 H1
N0720 G00 X-4.00 Y0.8750 M08
N0730 G56 H1 Z3.76
N0740 G83 Z2.02 R3.26 Q0.5 F18. P0.2
N0750 G00 Z20.
N0760 X4.000 Y0.3750
N0770 G56 H1 Z3.76
N0780 G83 Z2.165 R3.26 Q0.5 F18. P0.2
N0790 G00 Z20. M09
N0800 M01
N0810 G30 P2
N0820 T11 M06 (5/16-18NC TAP)
N0830 S324 M03 T1
N0840 G00 X-4.00 Y0.8750 G94
N0850 M327 TAP TORQUE monitoring ON
N0860 VTMNO=2 Select level 2 for Monitor Level
N0870 G56 H=VATOL M08 Activate tool length offset for Active Tool
N0880 G284 Z=0.4529 R2.0539 P0.5 F18.
N0890 M326 TAP TORQUE MONITORING OFF
N0900 G00 Z7.00
N0910 X4.00 Y0.3750 G94
N0920 M327 MONITOR ON
N0930 VTMNO=2 LEVEL 2 MONITOR
N0940 G56 H=VATOL NO NEED TO REPEAT LENGTH OFFSET SELECTION, IT IS ALREADY SELECTED!!
N0950 G284 Z=0.717 R2.0539 P0.5 F18.
N0960 M326 MONITOR OFF
N0970 G00 Z7.00
N0980 G80 M09
N0990 M01
N1000 G30 P2
N1010 M30


As you can hopefully see, you are not correctly referencing the current tool offset.
Another more idiot proof way to program tool length offsets is to use G56 HA.
The HA command tells the machine to access the first tool offset group for the tool that is active in the spindle.

The G15 Hx command tells the machine to select coordinate system designated by the Hx value, were "x" is the number of the coordinate system you desire.

Hope this helps a little...
Regards
Brian.

[dcoupar]

I'm sorry is my mistake it is OKUMA.
Thanks

So, 14 replies later, we learn that we've all been chasing our tails trying to help you. I would suggest that next time you have a problem, get your facts straight BEFORE you post a question.

This is a great place to get help, but if you won't take the time to even look at the machine and control to see what they are, I'm sure a lot of the folks here will tire of trying to pry information out of you.

Also, I might suggest that if you have an Okuma problem, the Okuma forum would be a more appropriate place to post.

Good luck.

[broby]

So, 14 replies later, we learn that we've all been chasing our tails trying to help you. I would suggest that next time you have a problem, get your facts straight BEFORE you post a question.

This is a great place to get help, but if you won't take the time to even look at the machine and control to see what they are, I'm sure a lot of the folks here will tire of trying to pry information out of you.

Also, I might suggest that if you have an Okuma problem, the Okuma forum would be a more appropriate place to post.

Good luck.

Hear Hear!!

[fdonosos]

Thank you very much for the help, I did change and it worked very well and I'm sorry for not giving all the incorrect information, I know the answer would have been faster and easier to understand the problem.
It's my first visit to CNCZONE and truth do not know where the post
Thanks Dcoupar and Broby
Sergio

[fdonosos]

My Company got new Machine Okuma Millac 761V Serie 31i Model A5 with Facnuc Control I writing program now but I have some issue to get in the program amchine home position, this what I have so far:
G80 ;
M09 ;
G91 G30 Z10 M19 ;
G90 ;
M01 ;
M30 ;

This does'n work, somebody can help me and tell me what is the worng with it
Thanks

[txcncman]

My Company got new Machine Okuma Millac 761V Serie 31i Model A5 with Facnuc Control I writing program now but I have some issue to get in the program amchine home position, this what I have so far:
G80 ;
M09 ;
G91 G30 Z10 M19 ;
G90 ;
M01 ;
M30 ;

This does'n work, somebody can help me and tell me what is the worng with it
Thanks

New machine, eh? Did you look in the accompanying manuals? Sure you need G30 and not G28?

[fdonosos]

I will check it out.
Thanks

[fordav11]

try......

G80 ;
M09 ;
G91 G28 Z0 M19 ;
G90 ;
M01 ;
M30 ;

[fdonosos]

Already try and work.
Thanks for you help