Okuma 5020 won't repeat cycle---Help?

[jakent]

I have an odd problem. I have written and run a program on my Okuma LNC-8 successfully hundreds of times. Trying to assign a "GOTO" command at the end results in the program repeating up to the first G01 line. X and Z motion stops. The spindle does not stop. In the program below it stops at line N0008. Thanks in advance

 

$B4C.NC%

N0000 (B4C.NC)

N0001 (MON. 11/18/2013 03:30PM)

V9=V9+1

N0003 G00 X10. Z.5

N0004 G50 S1000

N0005 G96 S500 M41 M03 M08

N0006 G00 X.6222 Z.1 T080808

N0007 G00 Z-.06

N0008 G01 X-.06 F.015

N0009 G01 X.02 Z-.05

N0016 G00 X.822 Z-.05

N0017 G00 X.242

N0018 G01 Z-.071 F.015

N0019 G03 X.2627 Z-.0917 I-.0549 K-.0404

N0020 G03 X.2662 Z-.1154 I-.0938 K-.019

N0021 G01 X.2664 Z-.2987

N0022 G01 X.4048 Z-.2989

N0023 G03 X.4445 Z-.3087 I-.0018 K-.0285

N0024 G03 X.4545 Z-.3205 I-.0196 K-.0152

N0025 G03 X.456 Z-.3627 I-.3361 K-.0272

N0026 G01 X.5398 Z-.3633

N0027 G01 X.5639 Z-.3657

N0028 G01 X.5926 Z-.3725

N0029 G03 X.642 Z-.4105 I-.0347 K-.0496

N0030 G00 Z-.05

N0031 G00 X.1585

N0032 G03 X.242 Z-.071 I-.003 K-.0578

N0039 G00 X.822 Z-.06

N0040 G00 X.1573

N0041 G03 X.2314 Z-.0813 I-.0023 K-.047 F.015

N0042 G03 X.2461 Z-.1086 I-.0397 K-.0253

N0043 G01 X.2464 Z-.3087

N0044 G01 X.4045 Z-.3092

N0045 G03 X.4304 Z-.3158 I-.0001 K-.0162

N0046 G01 X.4352 Z-.3222

N0047 G01 X.436 Z-.3727

N0048 G01 X.5278 Z-.3729

N0049 G01 X.551 Z-.3743

N0050 G01 X.5707 Z-.3779

N0051 G03 X.622 Z-.4124 I-.0218 K-.043

N0052 G00 X10.

N0053 G00 Z0.

N0054 T0800

N0055 G96 S500 M09

N0056

N0057 G96 S500 M41 M03 M08

N0058 G00 X.6535 Z-.5057 T101010

N0059 G01 X.5424 F.007

N0060 G00 X.6535

N0061 G00 X11.

N0062 G00 Z.5

N0063 T1000

N0064 G96 S500 M09

N0065

N0066 G96 S500 M41 M03 M08

N0067 G00 X.822 Z-.685 T121212

N0068 G01 X0. F.007

N0072 G96 S500 M09

N0073 M01

N0074 M05

G94 Z-.5 F200.

G00 X-2.55

M84

G04 P1

G94 Z.135 F100

M83

N0075 G00 X10.

N0076 G00 Z1.

N0077 T1200

N0078 GOTO N0001

N0091 M02

[gcode]

I think you need a G95 before N0008 to turn ipr feedrates back on.

You're calling G94 F100. (IPM) at the bottom of the file.. and I don't think the machine is stopping at N0008 , its just feeding very very slow (.015 IPM)

[gcode]

G94 Z.135 F100

 

and you might need to change F100 to F100.

[RaiderX]

will an m99 at end work? been a while since I worked Okuma but works with fanuc.

[crazy^millman]

I think you need a G95 before N0008 to turn ipr feedrates back on.

You're calling G94 F100. (IPM) at the bottom of the file.. and I don't think the machine is stopping at N0008 , its just feeding very very slow (.015 IPM)

 

We have a winner. That is what I suspect as well.

[jakent]

I have to add to this:

It actually IS repeating, but the feedrate is so slow it is imperceptable other than watching the position readout slowly tick down! What changed my feedrate?

[jakent]

G95 wins!!!!!

 

MUCH appreciation guys!

[gcode]

[chrisdavala]

gcode-The OSP doesn't need to see an F100. like a Fanuc would. It reads F100 as the same thing. No decimal point = whole number, not smallest increment. Out of habit, however, I still usually command F100.

 

Another note to add to the G94 situation. Depending on the software rev, it is possible you will need to command an M808 (Feedrate interlock release) to get the axis to move in IPM. Typically only when no spindle rotation, but nice to know if you run into this.