FANUC OMD feed hold only works right after startup

[sorenbj]

the machine it a yang eagle 1000 from 1998
it runs great, the only thing is the feed hold and feed override, they only work right after i have started the machine, if i run an other program it will not feed hold, but if i turn off the mill and start it up again i works,
then switch to an other program the problem is back

have someone had this problem, or any good tips that i should tjek,
i have all manuals and parameterlist and have read thru all i have, i am lost

best regards
Søren

Similar Threads:

• FANUC-OMD program problem
• Need Help!- Fanuc omd dripfeed issue
• Help With DNC on FANUC OMD
• Line numbers Fanuc OMD

[Superman]

Has an M-code been executed to override feed control ?

Ie ... the same codes that turn those features OFF when threading/tapping.
You may need to chase those codes up that control the feedrates then see if they are being applied.

[sorenbj]

no the only m codes in the program is M3 M5 M8 M9 and M30
it works right after startup, but not if i run an other program

Do you think that a tool change an M6 code could activate somthing
i will try later, to run some programs with no tool changes and see what thad do

Thanks for the Reply

[Superman]

no the only m codes in the program is M3 M5 M8 M9 and M30
it works right after startup, but not if i run an other program

Do you think that a tool change an M6 code could activate somthing
i will try later, to run some programs with no tool changes and see what thad do

Thanks for the Reply

It is a big possibility as the M6 actually calls up a macro and may disable the feedrate/feedhold buttons, and maybe also the single step, so it can't have any slowdown or stopping in the toolchange sequence.
To view the program, you would need to enable editing of the 8000/9000 protected program area....

NOTE...
Remember to backup them ALL before changing anything...
Even take a photo

[servtech]

Has an M-code been executed to override feed control ?

Ie ... the same codes that turn those features OFF when threading/tapping.
You may need to chase those codes up that control the feedrates then see if they are being applied.

I agree superman.
There are m codes to prevent operators feed holding or overriding during program.
The thinking behind it is for programmers to control the process, feedhold and override can ruin tools and workpieces.
Usually only set for G1, G2 and G3 because these are cutting feeds.
It's probable a previous user modified the tool change macro.
Perhaps there is a clean version stored.

[Superman]

I agree superman.
There are m codes to prevent operators feed holding or overriding during program.
The thinking behind it is for programmers to control the process, feedhold and override can ruin tools and workpieces.
Usually only set for G1, G2 and G3 because these are cutting feeds.
It's probable a previous user modified the tool change macro.
Perhaps there is a clean version stored.

Stop guessing... it is not helping at the moment
You don't know what has happened. So stop blaming a "previous user".

The OP has to go back to his machine to check codes in his M6 macro, that some features that are changed, are restored to their original status when leaving the macro.

Until then..... we wait
Usless there is an alternative solution

[sorenbj]

Thanks for the feedback,
i have the 9020 tool change macro in the book that came with the machine, i can see that it is using some valuabels like #4001 #4002 #1032 and and some M codes to bring the toolmag in and out and other things i do not know about

i will see if i can get in to the machine and compare the macro from the book to the one in the machine

Thanks

[servtech]

Stop guessing... it is not helping at the moment
You don't know what has happened. So stop blaming a "previous user".

The OP has to go back to his machine to check codes in his M6 macro, that some features that are changed, are restored to their original status when leaving the macro.

Until then..... we wait
Usless there is an alternative solution

Not guessing.

As a CNC service engineer and programmer on Fanuc and Siemens, I'm well past guesses.

I'm telling you, no blame attached to anyone, locking out feed and spindle override during program is an option well known in the CNC industry. I worked for German and Swiss machine tool builders not some back street job shop.

M48 used to lock the override and M49 enable on earlier Fanuc controls. M49 could be included at the beginning and end of the program.

[sorenbj]

I have tryed som programs in the machine and it is working with feed hold, but as soon as i do a tool change the feed hold dont work any more,
so i tryed to check the tool change macro, but i cant see it, og load it to the screen
any idears about how i gain acces to O9020
sorry about my spelling

[servtech]

I have tryed som programs in the machine and it is working with feed hold, but as soon as i do a tool change the feed hold dont work any more,
so i tryed to check the tool change macro, but i cant see it, og load it to the screen
any idears about how i gain acces to O9020
sorry about my spelling

There could be an OEM bit select for this, speed and feedhold locks are quite common in automotive and aerospace, to prevent operators damaging tooling and expensive workpieces. Check your operator manual for M codes and bit selects. ie M48/49 or other.

[sorenbj]

so i maneged to get in to the O9020 Tool Change Macro, and compare it to the one in my Fanuc P.C.B book and they are the same, i will post it here so you can see it,
i will try with the m48 m49 if that helps,

%
:9020
IF[#1015EQ1]GOTO50 (check machine lock/mst lock z axis lock)
IF[#20EQ0]GOTO40 (no t code)
#1100=1 (check m86 command from o9020 signal)
M86 (enter atc mode)
#106=BIN[#1032] (spindel tool number read)
IF[#106EQ#20]GOTO40 ((if spindel tool no equit mag no)
#101=#4001 (memory g code)
#102=#4002 (memory g code)
G17G91G80G0G49G63
G28X0Y0M19
M85 (search pocket for spindel number)
G30Z0
M82 (mag out)
M84 (spindel tool unclamp)
M07 (air blow)
G28Z0
T#20
M07
G30Z0
M83 (spindel tool clamp)
M88 (change tool number)
M81 (mag home)
N30G#101G#102 (set g code)
N40M87 (finish tool change)
#1100=0 (cansel m86 command from o9020 signal)
M99
#3000=1 (m06-no-t-code)
M99
N50#3000=2 (machine/M.S.T-locked)
M99
%

[Superman]

so i maneged to get in to the O9020 Tool Change Macro, and compare it to the one in my Fanuc P.C.B book and they are the same, i will post it here so you can see it,
i will try with the m48 m49 if that helps,

%
:9020
IF[#1015EQ1]GOTO50 (check machine lock/mst lock z axis lock)
IF[#20EQ0]GOTO40 (no t code)
#1100=1 (check m86 command from o9020 signal)
M86 (enter atc mode)
#106=BIN[#1032] (spindel tool number read)
IF[#106EQ#20]GOTO40 ((if spindel tool no equit mag no)
#101=#4001 (memory g code)
#102=#4002 (memory g code)
G17G91G80G0G49G63
G28X0Y0M19
M85 (search pocket for spindel number)
G30Z0
M82 (mag out)
M84 (spindel tool unclamp)
M07 (air blow)
G28Z0
T#20
M07
G30Z0
M83 (spindel tool clamp)
M88 (change tool number)
M81 (mag home)
N30G#101G#102 (set g code)
N40M87 (finish tool change)
#1100=0 (cansel m86 command from o9020 signal)
M99
#3000=1 (m06-no-t-code)
M99
N50#3000=2 (machine/M.S.T-locked)
M99
%

Biggest error is that it changes to incremental mode(G91) and doesn't change back to absolute (G90) before leaving the macro. Unless it is held in #4001 or #4002.
... not sure of what G63 is for, the others on the safety line are pretty well standard
... return to machine position X0Y0 at every toolchange BEFORE any raising of Z-axis might appear dangerous. MHO is that a toolchange should only change tools, not move the the part around, unless it needs to move to that position for TC.
... the M99 codes, why is there 2 before the N50 line, the #3000=1 (m06 no T code) line will never be read. 1st M99 may need to be omitted, to allow #3000 to be set.

[Superman]

Googling G63 gives back that it may be "tapping mode".
If it is, then it may be what is creating your issues.

It may need to be "cutting mode" which is G64

[servtech]

so i maneged to get in to the O9020 Tool Change Macro, and compare it to the one in my Fanuc P.C.B book and they are the same, i will post it here so you can see it,
i will try with the m48 m49 if that helps,

%
:9020
IF[#1015EQ1]GOTO50 (check machine lock/mst lock z axis lock)
IF[#20EQ0]GOTO40 (no t code)
#1100=1 (check m86 command from o9020 signal)
M86 (enter atc mode)
#106=BIN[#1032] (spindel tool number read)
IF[#106EQ#20]GOTO40 ((if spindel tool no equit mag no)
#101=#4001 (memory g code)
#102=#4002 (memory g code)
G17G91G80G0G49G63
G28X0Y0M19
M85 (search pocket for spindel number)
G30Z0
M82 (mag out)
M84 (spindel tool unclamp)
M07 (air blow)
G28Z0
T#20
M07
G30Z0
M83 (spindel tool clamp)
M88 (change tool number)
M81 (mag home)
N30G#101G#102 (set g code)
N40M87 (finish tool change)
#1100=0 (cansel m86 command from o9020 signal)
M99
#3000=1 (m06-no-t-code)
M99
N50#3000=2 (machine/M.S.T-locked)
M99
%

Did you write the comments in brackets or were they in the macro when you opened it. The reason for my question is I can't believe the macro can be this complex and not work correctly, when compared to another copy of the same macro.
It makes no sense.

[sorenbj]

yes i put the comments in to help, i just took the comments from the book,

Did you write the comments in brackets or were they in the macro when you opened it. The reason for my question is I can't believe the macro can be this complex and not work correctly, when compared to another copy of the same macro.
It makes no sense.

[sorenbj]

i will try to post the macro from the book, mabye that will help, so you can see what is written on the line where the G63 it...is says (DEM G STATION)

Biggest error is that it changes to incremental mode(G91) and doesn't change back to absolute (G90) before leaving the macro. Unless it is held in #4001 or #4002.
... not sure of what G63 is for, the others on the safety line are pretty well standard
... return to machine position X0Y0 at every toolchange BEFORE any raising of Z-axis might appear dangerous. MHO is that a toolchange should only change tools, not move the the part around, unless it needs to move to that position for TC.
... the M99 codes, why is there 2 before the N50 line, the #3000=1 (m06 no T code) line will never be read. 1st M99 may need to be omitted, to allow #3000 to be set.

[sorenbj]

[sorenbj]

the problem was as you say superman G63,
just tested it gave the machine a G64 after the tool change and all works fine, Thank you so much all of you who helpe,
so great to have that sorted, Thanks Again

Googling G63 gives back that it may be "tapping mode".
If it is, then it may be what is creating your issues.

It may need to be "cutting mode" which is G64

[Superman]

the problem was as you say superman G63,
just tested it gave the machine a G64 after the tool change and all works fine, Thank you so much all of you who helpe,
so great to have that sorted, Thanks Again

Glad to have helped...

There are the other concerns that were highlighted that should be tested
1.... have an imaginary tool inside an imaginary bore (or surounded by clamps), and change tools.... if you have an X0Y0 move before any Z lift... you can crash....your macro should have the G28X0Y0 omitted.
2.... put your machine in G90 or G91 mode, do a toolchange...it should return to the mode you had before the macro.

[sorenbj]

i see your point, every time i run a program and do a tool change i have a subprog (M98 P4) that i do before the tool change, that move z axis home and oriend the spindel... i have learned today about G63 and G64, so if i could get the G64 command in my tool change macro and also have it go home in z i would not need my sub prog M98 P4

Glad to have helped...

There are the other concerns that were highlighted that should be tested
1.... have an imaginary tool inside an imaginary bore (or surounded by clamps), and change tools.... if you have an X0Y0 move before any Z lift... you can crash....your macro should have the G28X0Y0 omitted.
2.... put your machine in G90 or G91 mode, do a toolchange...it should return to the mode you had before the macro.