[baow]

Dear all
please help me, I use a Matsuura RA-II CNC M/C control fanuc OMB.
Macro program tool change O9000 is lost by human deleted.

I'd like to give a macro program tool change O9000.

Thank you & Best Regards.
Baow (Thailand)

[fanucman]

Dear all
please help me, I use a Matsuura RA-II CNC M/C control fanuc OMB.
Macro program tool change O9000 is lost by human deleted.

I'd like to give a macro program tool change O9000.

Thank you & Best Regards.
Baow (Thailand)

contact matsuura they should have it... also block out your 9000's so this doesnt happen again...

[baow]

contact matsuura they should have it... also block out your 9000's so this doesnt happen again...

I contact Matsuura on last month, they reply " We checked the machine RA-2 is not including the ATC macro program and just command Z-axis zero return command (G91 G28 Z0) before command M06(tool change command)."

Thank you for reply Mr. fanucman

Do you have a sub-program tool change macro (O9000)?

Best regards.

[stevo1]

Baow,
A lot of people including myself will write a macro for the tool change so it always does an M19 and Z0 before changing. I use this macro for many other things like tracking the current tool in the spindle, setting my G43H() code so I don’t have to put it in the program, setting speeds and feeds, and bypassing the M6 code if you program a tool change for a tool that is already in the spindle.

Ok we will do just a simple very basic program and we can add to it if you want to do any other features.

First thing is if you were using a macro before then your custom macro parameters were probably set up to call the macro by an M6. So let’s try and keep it the same. You may have lost the program but your parameters should still be the same. We need to find out which program the M6 was calling.

Go to your parameters and look at parameters 230-239 and 240-242 one of these should be set to a 6 for calling a custom M6 code. This will tell us what program number it was calling.

230-239 calls programs 9020-9029. Ex if #231 is set to 6 then program 9021 will be called with every M6
240-242 calls programs 9001-9003. Ex if #240 is set to 6 then program 9001 will be called with every M6.

Once we find which program then we will make that program and put the code in it. Let’s just use 9001 for example sake.

O9020(tool change program)
G40G80------------tool comp cancel and canned cycle cancel
G91G28Z0M9-------position tool to Z0 and turn off coolant
M19---------------orientate spindle
G28Y0M5---------i like to send Y home to clear any parts but it is not needed
M6---------------tool change
M99--------------sub program end

We may or may not have to cancel tool offsets but we can see it this works.

Now as Fanucman has stated but didn't give you the parameter numbers there is a way to set the parameters to protect the 9000-9999 programs so this cannot happen again by operator error. IIRC set parameter 10.4 to 1 so this protects the 9000’s, set to 0 if you need to edit. Keep in mind if you backup your machine programs with this bit set to protect it will NOT output the 9000 programs. There is also a parameter to protect the 8000 programs, it is parameter 389.2

Stevo

[fanucman]

Now as Fanucman has stated but didn't give you the parameter numbers there is a way to set the parameters to protect the 9000-9999 programs so this cannot happen again by operator error. IIRC set parameter 10.4 to 1 so this protects the 9000’s, set to 0 if you need to edit. Keep in mind if you backup your machine programs with this bit set to protect it will NOT output the 9000 programs. There is also a parameter to protect the 8000 programs, it is parameter 389.2

Stevo

yep 10.4 make it equal 1 and 9000 are protected.... forgot to add that info..

[John_B]

steveo1,

Could he have a machine with the Custom Macro Cassette? I bought an old Fanuc Tape Drill recently that doesn't use the macro 9000 series program, but I was told the toolchange macro was written in the cassette mounted to the backplane???? First time seeing this for me.

Also, I looked at your macro example:

O9020(tool change program)
G40G80------------tool comp cancel and canned cycle cancel
G91G28Z0M9-------position tool to Z0 and turn off coolant
M19---------------orientate spindle
G28Y0M5---------i like to send Y home to clear any parts but it is not needed
M6---------------tool change Won't this cause a loop?
M99--------------sub program end

I've always seen the place where you show the M6 to have the individual commands for the pot down/arm forward/drawbar release/arm down/arm forward/arm up/drawbar clamp/arm forward/pot up commands or the umbrella out/drawbar release/z retract/umbrella index/z return/drawbar clamp/umrella retract commands.

I could be wrong, as I've not really had to monkey with that macro alot, just add small details to make it work as I wanted in a special case.

Rgds,
John

Forgot to add,the machine I got lately has the 0m-c.

[baow]

Baow,
A lot of people including myself will write a macro for the tool change so it always does an M19 and Z0 before changing. I use this macro for many other things like tracking the current tool in the spindle, setting my G43H() code so I don’t have to put it in the program, setting speeds and feeds, and bypassing the M6 code if you program a tool change for a tool that is already in the spindle.

Ok we will do just a simple very basic program and we can add to it if you want to do any other features.

First thing is if you were using a macro before then your custom macro parameters were probably set up to call the macro by an M6. So let’s try and keep it the same. You may have lost the program but your parameters should still be the same. We need to find out which program the M6 was calling.

Go to your parameters and look at parameters 230-239 and 240-242 one of these should be set to a 6 for calling a custom M6 code. This will tell us what program number it was calling.

230-239 calls programs 9020-9029. Ex if #231 is set to 6 then program 9021 will be called with every M6
240-242 calls programs 9001-9003. Ex if #240 is set to 6 then program 9001 will be called with every M6.

Once we find which program then we will make that program and put the code in it. Let’s just use 9001 for example sake.

O9020(tool change program)
G40G80------------tool comp cancel and canned cycle cancel
G91G28Z0M9-------position tool to Z0 and turn off coolant
M19---------------orientate spindle
G28Y0M5---------i like to send Y home to clear any parts but it is not needed
M6---------------tool change
M99--------------sub program end

We may or may not have to cancel tool offsets but we can see it this works.

Now as Fanucman has stated but didn't give you the parameter numbers there is a way to set the parameters to protect the 9000-9999 programs so this cannot happen again by operator error. IIRC set parameter 10.4 to 1 so this protects the 9000’s, set to 0 if you need to edit. Keep in mind if you backup your machine programs with this bit set to protect it will NOT output the 9000 programs. There is also a parameter to protect the 8000 programs, it is parameter 389.2

Stevo

Thank you very much, sir

I can't call program O9001,but I can calling program O9000
I set parameter 240 --> 6
241 --> 6
242 --> 6
machine alarm 071 P/S ALARM, Can not edit programe in O9001

Mr.Stevo In case I delete program in O9000, Do you have a methode to recall program O9000?

Best Regards
Baow

[stevo1]

John,
I have never seen or used the macro cassette. The only thing I have seen is on one of my old 10t controls that had a yellow cassette that looks like an old 8track tape mounted on the backplane. This is the ladder logic. As you said it was the first time you have seen it and it’s the first time I have heard of it. I would be curious to hear more on this as I did not know that hardware was required for any macro programming on any of the controls.

Some tool change programs will have all the data in it as you were referring to, arm up, arm down tool release etc. Most mt that I have seen have all of this written into the ladder and the only thing the machine really needs is to be at Z0. Obviously this is not always the case. The M6 will not cause a loop. When a program or MDI sees a T()M6 then the custom program will be called based on the M6, the T() value will be modal. Once the M6 is read alone then it will call the modal T value via tool change.

Baow,
Ok it was an oversight on my behalf. If you were using program 9000 in the past then this was done by setting of parameter 40.5. When this is set to 1 then program 9000 is called when a T() is specified. This is done the same as a custom code that I explained before. Set parameters 240,241,242 back to the original value. I am not sure if you were trying to set all 3 of them to 6 but that is not the way. As an example if 240=6 then program 9001 will be called with every M6. If 241=7 then program 9002 will be called with every M7, if 242=150 then program 9003 will be called with every M150.

What you need to do is create program 9000 and put the code that I have posted into program 9000.

The reason you are getting the 071 alarm is because you have your parameters setup to call a subprogram but you do not have that program in memory. It would be no different than say doing a M98P1234 but there is no program in memory that is O1234. You need to create program 9000 in memory. I am not 100% on the Om control on the exact steps for doing so.

If you cannot edit your 9000 programs then it is because they are locked with the parameters that I had listed above. Once you delete the program there is no way of calling it back. What you should do is a backup of your control via RS232 port. Then if you every delete or lose the memory in your machine you can just simply re-download the data.

Stevo

[ahmet677]

Fanuc OM


&HE:%
:9001
G80G40
G65H81P25Q#1013R1
G65H81P25Q#1008R1
G65H01P#132Q#4014
G65H01P#131Q#4003
G65H01P#130Q#4006
M66G91G30Z0
G65H12P#1132Q#1132R4096
G65H11P#1132Q#1132R1024
G04P100
G65H12P#148Q#1032R255
G04P100
G65H12P#1132Q#1132R4096
G65H11P#1132Q#1132R2048
G04P100
G65H12P#531Q#1032R255
G04P100
G65H12P#1132Q#1132R4096
G65H01P#1115Q1
G04P100
G65H12P#149Q#1032R255
G65H81P20Q#531R#149
G65H81P1Q#148R#149
G04P100
M42
N1G65H81P5Q#1011R1
G65H80P1
N5G65H86P10Q#531R18
G#132
G#131
G#130
G65H99P1
N10G65H83P15Q#531R0
G#131
G#130
G65H99P2
N15G65H01P#1112Q1
G65H11P#1132R256
G04P100
G65H01P#1113Q1
G91G30Z0M19
M52
M12
G04P500
G28Z0
G65H01P#1114Q1
M41
G30Z0
M11
M53
G65H01P#1109Q1
G04P100
G65H12P#1132Q#1132R4096
N20G65H01P#530Q#531
G#132
G#131
G#130
N25M67
M99
%

[John_B]

John,
I have never seen or used the macro cassette. The only thing I have seen is on one of my old 10t controls that had a yellow cassette that looks like an old 8track tape mounted on the backplane. This is the ladder logic. As you said it was the first time you have seen it and it’s the first time I have heard of it. I would be curious to hear more on this as I did not know that hardware was required for any macro programming on any of the controls.

Yeah, new to me. I was told that is held the toolchange macro by another shop owner like myself so that is not gospel - probably quite the contrary. This Tape Drill machine is pretty odd, it has the C series control, but the alarm list you have to use is for the 0-Mate. I did see in the options list for this machine that there is an ATC option can be set. I had the notion that the ladder on the 0m-C was on the memory board in the chips mounted there.

The M6 will not cause a loop. When a program or MDI sees a T()M6 then the custom program will be called based on the M6, the T() value will be modal. Once the M6 is read alone then it will call the modal T value via tool change.Stevo

Ok, thanks for the insight.

[sinha_nsit]

In a macro/subprogram called by G-code (other than G65/G66), M-code or a T-code, all G, M and T-codes are treated as standard codes, with their pre-defined meanings. So, in a macro called by, say, M06 (with or without arguments), no macro can be called by any G (other than G65/G66), M and T-codes. Therefore, M06 will have its usual tool change function in a macro called by M06.