[Zoner]

I was very kindly sent the following macros by Kryle for our 0M control on a VMC700, having lost our own toolchange macro 9001 and other stuff.

They have been very kind and as they are extremely busy I don't want to barrage them with questions that users should already know the answers for.

Can anyone please translate them for me so we can understand what they will do? They are not specifically for our machine but for another close-serial one. Ideally one of them will operate the carousel!

We have a 20-slot tool carousel on the VMC.

O9001(ISOMACRO)
M22
G65H81P30Q#1000R1
G65H01P#149Q#4003
M19G91G80
G65H81P10Q#1001R1
M23G28Z0
M21
M26
G30Z0
N10G65H81P20Q#1002R1
M26G30Z0
M24
M21
G28Z0
N20M25
M22
G28Z0
G#149
N30M99



O9003(CAPMACRO)
G65H1P#149Q10170
T#9149
M22
G65H81P30Q#1000R1
G65H01P#149Q#4003
M19G91G80
G65H81P10Q#1001R1
M23G28Z0
M21
M26
G30Z0
N10G65H81P20Q#1002R1
M26G30Z0
M24
M21
G28Z0
N20M25
M22
G28Z0
G#149
N30M99
%

[beege]

Aha! Finally some examples of macro A. Surely someone has an old manual...

[JimBoyce]

This machine had the parameters erased. It has not been determined (by reading other posts by Zoner) that the basic parameters that have to be entered in hexadecimal are OK, or other parameters for that matter. Looking at the Macro, there is nothing special there, in other words run the macro lines in MDI and see if anything happens.
In fact try some basic code in MDI, (S500 M3 or M8) and post what happens.

[Zoner]

Yes the machine was erased (partially anyway), its toolchanger and MPG don't work, but the state of our machine won't have any bearing on these macros.

What I was looking for here was just a translation of what these 2 macros will do, step by step? I want to understand them.

One other thing - one macro is at 9001 and I guess that will call when we do an M6? We do have a 6 in the memory attached to calling 9001.

So how about the one at 9003, how do we get to call that one? I've seen a C.A.P. softkey on one of the screens but don't know what it is or how to use it?

[The Engine Guy]

Yes the machine was erased (partially anyway), its toolchanger and MPG don't work, but the state of our machine won't have any bearing on these macros.

What I was looking for here was just a translation of what these 2 macros will do, step by step? I want to understand them.

One other thing - one macro is at 9001 and I guess that will call when we do an M6? We do have a 6 in the memory attached to calling 9001.

So how about the one at 9003, how do we get to call that one? I've seen a C.A.P. softkey on one of the screens but don't know what it is or how to use it?

The 9001 Macro is for operating the toolchanger when you are in ISO mode, that is when you are using NC code ("G" code).
The 9003 Macro is for operating the toolchanger when in the C.A.P Mode, this stands for Fanucs "Converstaional Automatic Programming", if your control can be used in either mode then you will need both Macros installed in the Program Library.
Pressing the C.A.P. softkey should take you to the screens where you just input data and the control does the rest, it should also have simulation "wire frame" type graphics where you can run the program you have just written on the screen and watch the tool path as if the machine is cutting the part.

Hope that helps.
Regards
Rob

[dcoupar]

As far as I can tell... (I don't have a machine manual for M-codes and/or I/O signals)

G65Hnn calls a function, i.e.: =, <>, etc. P, Q, & R are the variables.

G65H01 is variable assignment (P=Q)
G65H81 is simple (IF Q=R GOTO P)

So your ISO macro:

O9001(ISOMACRO)
M22 (unsure of function of M22)
G65H81P30Q#1000R1 (if #1000=1, goto N30 - #1000 is an I/O signal)
G65H01P#149Q#4003 ( #149=#4003 - store value of group 03 g-code - G90/G91)
M19G91G80 (orient spindle, set incremental mode, canned cycle cancel)
G65H81P10Q#1001R1 (if #1001=1, goto N10 - #1001 is an I/O signal)
M23G28Z0 (unsure of M23, return Z to home)
M21 (unsure)
M26 (unsure)
G30Z0 (return Z to 2nd zero)
N10G65H81P20Q#1002R1 (if #1002=1, goto N20 - #1002 is an I/O signal)
M26G30Z0 (unsure of M26, return Z to 2nd zero)
M24 (unsure)
M21 (unsure)
G28Z0 (return Z to home)
N20M25 (unsure)
M22 (unsure)
G28Z0 (return Z to home)
G#149 (set G90/G91 to original state)
N30M99

[stevo1]

Aha! Finally some examples of macro A. Surely someone has an old manual...

I agree. The cobwebs are going to have to be dusted off that manual. Well done Dave….as much as I hate macroA it is always nice to see an example of it.

Jim…I PM’d you back your parameters and labeled them. I would suggest using macroB for your tool change programs. I saw the programs in the PM and they are much easier to understand and tweek what you want to. MacroA is outdated IMO. You can see as Dcoupar has put in () the definition of each line and the definition he wrote (for arguments sake) is in a macroB format. A lot easier to follow.

To call up program 9001 with the M6 code you have to set parameter 240=6 and if you want to call program 9003 with the M6 then set parameter 242=6.

FYI on the Oseries controls
Parameters 240-242 calls programs 9001-9003 using M-codes
Parameters 230-239 calls programs 9020-9029 using M-codes
Parameters 220-229 calls programs 9010-9019 using G-codes

That’s my .02cents.

Stevo

[gbowne1]

I've been wondering about the 0M macros myself as the system 0M I have planned has a 266kB Macro Cassette.

I guess I will have to study the 0M-C macro manual more.

Greg

[stevo1]

I've been wondering about the 0M macros myself as the system 0M I have planned has a 266kB Macro Cassette.

I guess I will have to study the 0M-C macro manual more.

Greg

The nice thing is macro’s are macro’s and don’t just pertain to the Om control. The only things that will typically change across the different series fanuc controls would be the system variables. So once you learn them you will have a good understanding across the fanucs. I would suggest that if you are going to study up on them then study macroB. MacroA is outdated.

Once you start learning and using them you won’t stop. You will start to look for ways to incorporate them into everything you are doing, even if it’s overkill.

The fanuc manuals are going to be very hard to learn from.

Stevo

[Zoner]

Many thanks guys.

[gbowne1]

The Macro Cassette I have on hand is a A02B-0091-C115 and is a 256KB macro cassette for the FANUC 0 control. It's listed as a "Macro Cassette C" on the label.

This is much like the PC cassette on the 11 controls.

It's found affixed to one of the small slots on the mainboard.

I guess that it needs to be written to by a special device.

Greg

[stevo1]

Greg,
I have never used the macro cassette on the O controls. I would ass u me that you would need to write to it somehow. The cassette pertaining to the 11 series is the ladder logic.

Stevo

[gbowne1]

Well, for the 0 Controls.. the Macro Cassettes are descrived in the manual:

GFZ-61393E-1/02

This is a manual labeled Series 0/00/0-Mate Macro Compiler/Macro Executor.

The cassette(s) are also listed in the board listing of the Maintenance manual.

If you have the Graphics Conversion option, there are two other cassettes.

But there are some basic casettes used with the compiler addressed in this manual.

The are all A06B-0035-J542#0A80 and A06B-003-J542/#0A80 basic part numbers. These are if you use the English or Japanense Language text.

Read the section of the manual called "Series 0 Macro Compiler/Macro Conversion with Graphics Conversion".. and it is on Page A4-2.

There are also A06B-0035-J543 and A06B-0036-J543 cassettes. I also saw the numbers A02B-0098-J560 and A02B-0099-J560 on pg. A4-11.

There is a System F-G or P-G for the macro units shown on page 4 and 5 of the manual.

Greg