Okuma Spindle Tool Fix

[Greg Williams]

Hi All,

 

For those with Okuma mills, Below is the fix for the spindle tool commanded in program error. This fix will work for U100 E100 and P200 machines. It may also work on older ones but O have not tried them.

 

 

Ok, Save the following text as tool.lib

 

 

OTCK (GET NOMINATED TOOL)

IF [PT EQ EMPTY] NERR

IF [PT EQ VTLCN] NEND

IF [PT EQ VNTOL] NM6

IF [VNTOL EQ 0] NCT

M64

NCT T=PT

NM6 M6

NEND G56 H=PT D=PT

GOTO NRTS

NERR M63

M6

NRTS RTS

 

ONOT1(M201)

M63

M329

M06

RTS

 

ONOT2(M202)

M64

M63

M329

M06

RTS

 

 

Copy this tool.lib file to MD1 directory of the machine.

 

If the buffer has been set large enough all will be sweet, If not you will need to initalize the buffer and reset it to a binary number (say 4800)

If in doubt miss this step

 

Turn off all power

 

Restart Machine - Note if there are any lib registration errors, If there are none all is good if there are *lib errors see previous step

 

Go to Parameters G and M codes

 

Next to G116 set OTCK

 

Save, Yes very important

 

On a new P200 control you will need to register the *.lib file. From Run mode, press extend then Register lib files

 

 

OK now G code needs to look like this

 

Blah Blah

G116 T4

G00 X0 Y0 Blah Blah

 

So if T4 is in the spindle the program will continue with no errors if not the machine will go and get T4 then continue. This will also work thru DNC-DT

 

Hope this helps someone

[chris m]

I don't think I'll use it right now, but thanks for the info!

 

C

[jeff]

Thank you Greg!

[beej]

thanks, Greg!

[Greg Williams]

Glad to help,

 

If this works on an OSP7000 or older please let us know

[YoDoug®]

Hi All,

 

For those with Okuma mills, Below is the fix for the spindle tool commanded in program error. This fix will work for U100 E100 and P200 machines. It may also work on older ones but O have not tried them.

 

 

Ok, Save the following text as tool.lib

 

 

OTCK (GET NOMINATED TOOL)

IF [PT EQ EMPTY] NERR

IF [PT EQ VTLCN] NEND

IF [PT EQ VNTOL] NM6

IF [VNTOL EQ 0] NCT

M64

NCT T=PT

NM6 M6

NEND G56 H=PT D=PT

GOTO NRTS

NERR M63

M6

NRTS RTS

 

ONOT1(M201)

M63

M329

M06

RTS

 

ONOT2(M202)

M64

M63

M329

M06

RTS

 

 

Copy this tool.lib file to MD1 directory of the machine.

 

If the buffer has been set large enough all will be sweet, If not you will need to initalize the buffer and reset it to a binary number (say 4800)

If in doubt miss this step

 

Turn off all power

 

Restart Machine - Note if there are any lib registration errors, If there are none all is good if there are *lib errors see previous step

 

Go to Parameters G and M codes

 

Next to G116 set OTCK

 

Save, Yes very important

 

On a new P200 control you will need to register the *.lib file. From Run mode, press extend then Register lib files

 

 

OK now G code needs to look like this

 

Blah Blah

G116 T4

G00 X0 Y0 Blah Blah

 

So if T4 is in the spindle the program will continue with no errors if not the machine will go and get T4 then continue. This will also work thru DNC-DT

 

Hope this helps someone graemlins/cheers.gif

 

For P300 machines change the VNTOL to VTLCN. It will eliminate alarms if the tool is designated as heavy or large tool. It also will address alarms with tool numbers greater than 999.

[The Cathedral]

Nice update man, thanks!

[mig]

Is it works for  the older controls   with  Ethernet   connection ?

 Or  if code loaded in "md1: " drive only