Okuma Multus M323 question

So having ran a Multus for awhile now I have always hated that if you have a tool pre-called that is different than the tool you want to call next it will alarm out instead of sending that tool back to the magazine and calling up the tool you now want. Or alternately if you have a tool precalled and you need to Re-run the tool you currently have in the spindle it will alarm out when it tries to pre-call the tool that is already pre-called. So I thought to myself I will just create a macro to send a tool back to the magazine if the waiting tool is not correct. The biggest issue I have found so far is it seems that the M323 is written to somewhere I cannot find. The actual tool change is commanded with M321 which I can find and change but the TD tool call which will populate all the variables I need uses the M323 to get into M321. And unless I can find out where to edit the M323 and add a couple lines of code to it I dont think what I am attempting to do is possible. I know I could just add a whole macro section before every tool change that would have to be edited on every tool change on every program, but I am trying to avoid that by adding some IF statements into the M323 command. Ive done this on a Okuma horizontal mill with using a G111 for a tool change where it will send the waiting tool back if its not the correct tool called up which was easy to do. I dont know why Okuma decided it wanted to make the Multus so much more difficult. Does anyone have any input?

Quote:

---

So having ran a Multus for awhile now I have always hated that if you have a tool pre-called that is different than the tool you want to call next it will alarm out instead of sending that tool back to the magazine and calling up the tool you now want.

---

hy :) a good tool change macro should handle the case of "another" prestaged tool

Quote:

---

Or alternately if you have a tool precalled and you need to Re-run the tool you currently have in the spindle it will alarm out when it tries to pre-call the tool that is already pre-called.

---

it should detect if the tool that you are calling is allready in the spindle

a good code covers shop floor events, not only theoretical ones; i have solved this for mb machines a few years ago, after i saw that shared codes don't cover particular cases; besides what you described, there may be other cases

unfortunately, i don't have experience with multus; you will need patience to fix it / kindly :)

Quote:

---

Originally Posted by deadlykitten

hy :) a good tool change macro should handle the case of "another" prestaged tool

it should detect if the tool that you are calling is allready in the spindle

a good code covers shop floor events, not only theoretical ones; i have solved this for mb machines a few years ago, after i saw that shared codes don't cover particular cases; besides what you described, there may be other cases

unfortunately, i don't have experience with multus; you will need patience to fix it / kindly :)

---

The issue with a Multus and how the tool change works is you have to have a TD=XXXXXX M323. That gives the machine the tool position and number then starts the toolchange. If you dont have a M323 in the TD line it will alarm out, and if you have the wrong precalled tool it alarms out immediately 3 lines into the M323 subroutine. I need to find if I can edit and where that subroutine is located in the control. It is not in with the rest of the Okuma SSB files.

And as far as it knowing what tool is in the spindle upon restarting the tool path, it does. That is not the issue. The issue is when the next tool Pre-call happens that is already in the ready station it alarms out.

hy malachi :) i am not a multus guy, but here is what i would do :

if your control is runing on windows, use an infile search for M323; once you find the file, copy it and inspect the copy, save it for later use, etc ... if you open the file on the machine, it's possible to mess it up ( text may get wraped differently, lines may get splited, etc ), depending on text editor settings; in such a situation, if file was opened, then don't save it :) consider back up first

if machine is not windows based, then i have no clue how to acces it's inner files or those from setup disks; thus it should be possible, only that so far i have no such experience

another method, is to try the edit function while machine is runnig, maybe it will open the file containing M323; i am not sure if it will work, but give it a try :)

if that doesn't work, then run the machine in condition that all will work, like next tool is ok, thus be sure that M323 performs error free, and visualize the code on screen, maybe in step-by-step; if needed, consider changing page layout, so to find a view that shows more lines of text

if all above fails, then is needed to inspect manuals and on machine help menus

final goal is to find system variables of interest, hoping they exist :) once those are found, you may proceed in 2 methods :
... change the file that contains M323, thus implement logic inside M323 procedure
...... or
... logic outside, thus before M323 procedure

there may be hidden effects, a few things to be aware with each method, but now is not the case; let's see if those variables can be found

---

another approach : is it possible to always cancel prestaged tool ? is it possible to prestage a tool, cancel then prestage other, and so on ? if you consider, look also into this; is needed a system variable for next tool, and a code to cancel active prestaged tool; its possible that those exist; if you will share the manuals, i will take a look / kindly :)

on a mill, you can read next tool with VTLNN, and cancel prestage with M64 ; maybe those work also on multus :)

Quote:

---

Originally Posted by deadlykitten

on a mill, you can read next tool with VTLNN, and cancel prestage with M64 ; maybe those work also on multus :)

---

Sadly I wish the Mills and a Multus were the same in their Variable calls. Im an Applications Engineer for an Okuma Distributor and have been trying to find a way around this issue for weeks to no avail. Every other machine style Okuma makes I can get around it. Just not the Multus which is why I came here to see if anyone had ever tried to figure out the issue from my original post before. Was kind of a shot in the dark.

hy malachi :) i also looked for TD inside manuals, and it seems that it works only with M323 : i guess atc position, ofset and arm swing, all are comanded in 1 block, while on a mill, there are 3 different blocks for each one ( T M6 G56 )

my 1st impresion was that such a multus mix may lead to problems, or more precise, to more downtime required to fix a situation, comparable to a mill

i don't have access to multus, i can't do much ... but if you wish, share the multus manuals, i will take a look / kindly :)

This thread is a few months old but here you go. Note; the macro uses G20 hP=4 for safe home position move, edit as needed. If your machine doesn't have G20 HP=4 set up don't run without editing, you will may crash.

OATC1
(TOOL CHANGE MACRO)
(COMMAND IS G206 PT=??)
()
()
()
TOOL=PT*100+1
M331
IF[VTTLN[1] EQ PT] NEND
M331
IF[VMTTL EQ PT] NCH
M331
IF[VMTTL NE PT] NCLR

NCH
G136
G0 X100.
G20 HP=4
MT=TOOL
M321
GOTO NEND

NCLR
M228
G136
G0 X100.
G20 HP=4
MT=TOOL
M321

NEND
RTS

Quote:

---

Originally Posted by YoDoug

This thread is a few months old but here you go. Note; the macro uses G20 hP=4 for safe home position move, edit as needed. If your machine doesn't have G20 HP=4 set up don't run without editing, you will may crash.

OATC1
(TOOL CHANGE MACRO)
(COMMAND IS G206 PT=??)
()
()
()
TOOL=PT*100+1
M331
IF[VTTLN[1] EQ PT] NEND
M331
IF[VMTTL EQ PT] NCH
M331
IF[VMTTL NE PT] NCLR

NCH
G136
G0 X100.
G20 HP=4
MT=TOOL
M321
GOTO NEND

NCLR
M228
G136
G0 X100.
G20 HP=4
MT=TOOL
M321

NEND
RTS

---

How do I go about editing macros on a multus? Where are they even located?