[jimmyjolly]

Hi all, I am running a yang vmc with a fanuc om g controller and it wont tool change in mdi mode, it will however tool change if running a program automatically. I remember years ago having a similar problem and was to do with missing a program O9000 that was locked in the controller. I am relatively unfamiliar with fanuc controllers, does anyone have any idea of what I may be able to do to both program this and get it into the controller? Thanks in advance for any help, jimmy

[Al_The_Man]

If you want to gain access to the 9000 programs you need para 0010 bit #4 set to 1.
Be aware that while this bit is set, it is possible to erase them through the clear programs command.
Al.

[Namnp2007]

Hi jimmyjolly
Pls. sent me this O9000 program( when you can access it), I need it for my VMC machine . Thanks.

[crazycnc]

Hi Jimmy,
Are you sure that the 9000 program is missing?
We have a VMC with a O-Mate M control, and I couldn't figure out how to do the tool change in MDI mode either. But finally figured out you had to be in AUTO mode and run the appropriate 9000 program from there. Our machine has a tool change button that would index the changer one slot every time the button was pressed while in this program. Hope this helps.

Now maybe you can help me yet, if you ever get a hold of this toolchange macro. I accidently deleted mine, and my backup got lost, so I'm wondering if yours would be similar enough that I could make it work on my control. I know it wasn't a long program at all. I think maybe 5 lines long.

Thanks,
Lorne

[stevo1]

O9020(TOOL CHANGE PROGRAM)
#20=#4120--(sets #20 equal to modal T)
G40G80—(tool dia cancel & canned cycle cancel)
IF[#20EQ#xxxx]GOTO1--(skips tool change if calling tool in spindle)
G91G28Z0M9—(tool change position in Z & coolant off)
M19--(tool orientation)
G28Y0M5—(tool change position in Y & spindle stop)
M6—(tool call of modal T value)
N1—(address to jump to if calling current tool in the spindle)
G90G49Z#5043—(cancel tool offsets no tool movement)
#535=#20—(sets #535 equal to the tool that was called to the spindle)
M99

You must change the XXXX in the 3rd line to the variable that specifies your current tool in the spindle. Mine is #1033. Also if you don’t like the #20 in your program take it out. Remove the first line #20=#4120 then change your 3rd line to IF[#4120EQ#xxxx]GOTO1. #4120 is your modal T command. I use the #20 so I can set #535 at the end of the program equal to the tool in the spindle because some of my machine displays don’t show the T on the program check screen. So all the operator has to do is look at #535 to see what tool is in the spindle.

There is also a lot of other things that I have in my tool change macro like setting the H value so you don’t have to keep programming it at every tool change and the Z won’t move. I also set my S&F’s there. This is stripped down and basic so with a few adjustments this should work for you.

In your control you have to change macro parameter to call the tool change program with an M6. On the OM control they are as follows:
#230-#239 calls programs 9020-9029
#240-#242 calls programs 9001-9003

Just an FYI I would think jimmyjolly got it fixed since he has not posted here since this thread in September.

Good luck,
Stevo

[crazycnc]

Thanks Stevo,
You might regret replying to my question, I might need a lot of coaching! First problem, when I try creating my 9000 program by typing in O9000 [INSERT] on the operator panel I get this error: "074 P/S Alarm". According to the manual this means 'The program number is other than 1 to 9999'. And yes I did try this with a few other 9000 numbers, and yes it does work with a 'regular' program number such as '101'.

[Stebedeff]

________________________________________
:9020 (TOOL CHANGE MACRO)
IF[#1015 EQ1 ]GOTO50
IF[#20 EQ#0 ]GOTO60
#1100 =1
#106 =BIN[#1032 ]
IF[#106 EQ#20 ]GOTO40
#101 =#4001
#102 =#4002
#103 =#4003
G17 G91 G80 G0 M86
M19
M85
G30 Z0.
M82
M84
M07
G28 Z0.
T#20
M07
G30 Z0.
M83
M88
M81
N30 G#101 G#102 G#103
N40 M87
G90
#1100 =0
M99
N60 #3000 =1 (M06-NO-T-CODE)
G90
M99
N50 #3000 =2 (MACHINE/MST-LOCKED)
G90
M99

There may be some machine specific parameters that need to be changed as this is from a Yang Eagle machine.
Best of luck


* Don't know where I got this from but thought I'd post it anyway. This was copied from another post wich I pasted to word a while ago. Hope it could help. Good luck

[stevo1]

I don’t mind helping that’s what where all here for.

I am assuming you are using an Om control? Your 9000 programs are probably locked. You have to change parameter 10.4 to get access to them. You should then be able to create 9000-9999 programs. Just an FYI parameter 384.2 is the locking of the 8000-8999 programs.

What was your old tool change program number before you lost it? 9000? There is no way to have the M6 call a 9000. You can have the 9000 called with a T code if parameter 40.5 is set. If this is how your machine was set up in the past then you could do a tool change with just a T code no M6 needed in your main program.

I however always set mine up to use the M6 call which means you have to use programs 9001-9003 or 9020-9029. So as I stated in my last post if you set parameter 203=6 now every time an M6 is programmed it will call program 9020. If you set parameter 204=6 it will call 9021 with an M6 ect.

Let me know if you get hung up or you want to add anything else like setting the H value or S&F's ect.

Stevo

[crazycnc]

OK, now I can create my 9001 program, and I can see the main program is calling up the 9001 program, but now I need to study up on my macro programming as the code is not working yet. I'll also have to figure out yet what variable references my current tool. See if I can find it in the manual.

'You must change the XXXX in the 3rd line to the variable that specifies your current tool in the spindle. Mine is #1033.'

Is this 1033 actually parameter 1033?

[stevo1]

What part of the program is not working? The main reason the #1033 and #4120 are in there is so that if you are calling a tool that is already in the spindle then it will bypass the M6 command. So to try out the code you can remove these and do a tool call. Just make sure every time you call a tool it is not the same one that is in the spindle. This will help you at least prove out the positioning and M6 ect. until we find the parameter for the tool in the spindle

Yes that is parameter 1033. These are the input signals. I cannot write to #1033 this gets set every time the tool changes. So I can read from it. This is not going to be in your Fanuc manual this will be in your MTB manual. I am pretty sure that these are the same input/output numbers on the OM control so we should be able to find the one that tracks your tool(there should be one, I hope). So there are a few things that you can do to try and find the parameter that is tracking the tool.

The input/output parameters are as follows:
#1000-#1035 input
#1100-#1135 output

So if you run this program
#1=0
#2=0
WHILE[#1LT35]DO1
#[100+#2]=#[1000+#2]
#[136+#2]=#[1100+#2]
#1=#1+1
#2=#2+1
END1
M30

Now your common variables #100-#135 are set to #1000-#1035 in sequential order. #136-#171 are set to #1100-#1135. Look at the variables and see if any one of them are set to the current tool in the spindle. If so then do a tool change to a different tool number and run the program again. If it is the same variable that changed to the tool in the spindle you have found your tool tracking parameter.

Stevo

[Carter]

O9020(TOOL CHANGE PROGRAM)
#20=#4120--(sets #20 equal to modal T)
G40G80—(tool dia cancel & canned cycle cancel)
IF[#20EQ#xxxx]GOTO1--(skips tool change if calling tool in spindle)
G91G28Z0M9—(tool change position in Z & coolant off)
M19--(tool orientation)
G28Y0M5—(tool change position in Y & spindle stop)
M6—(tool call of modal T value)
N1—(address to jump to if calling current tool in the spindle)
G90G49Z#5043—(cancel tool offsets no tool movement)
#535=#20—(sets #535 equal to the tool that was called to the spindle)
M99

You must change the XXXX in the 3rd line to the variable that specifies your current tool in the spindle. Mine is #1033. Also if you don’t like the #20 in your program take it out. Remove the first line #20=#4120 then change your 3rd line to IF[#4120EQ#xxxx]GOTO1. #4120 is your modal T command. I use the #20 so I can set #535 at the end of the program equal to the tool in the spindle because some of my machine displays don’t show the T on the program check screen. So all the operator has to do is look at #535 to see what tool is in the spindle.

There is also a lot of other things that I have in my tool change macro like setting the H value so you don’t have to keep programming it at every tool change and the Z won’t move. I also set my S&F’s there. This is stripped down and basic so with a few adjustments this should work for you.

In your control you have to change macro parameter to call the tool change program with an M6. On the OM control they are as follows:
#230-#239 calls programs 9020-9029
#240-#242 calls programs 9001-9003

Just an FYI I would think jimmyjolly got it fixed since he has not posted here since this thread in September.

Good luck,
Stevo

I am not in front of my machine atm, but, will this macro work for 16M or does there need to be edits made?

thank you,
carter

[marsheng]

I have a FANUC OMD and after the battery power was lost. Had to reenter the parameters, PMC and macros.

I cant however enter the macros 9020 and 9021. Have set parameter 0010 # 4 to a 1 but still cannot upload the files. Get 074 File name error.

Trying to rename an existing program also gives Error 074.

Something else is stopping access to 9000+ files.

Any suggestions ?

[SantiiA1]

I have a FANUC OMD and after the battery power was lost. Had to reenter the parameters, PMC and macros.

I cant however enter the macros 9020 and 9021. Have set parameter 0010 # 4 to a 1 but still cannot upload the files. Get 074 File name error.

Trying to rename an existing program also gives Error 074.

Something else is stopping access to 9000+ files.

Any suggestions ?

I have the same problem and i don't now What is the parameter 0010

[Al_The_Man]

Parameter 10 allows the access to the macro programs.
You need a copy of the macro in order to re-enter it.