[Caprirs]

I am a newbie on an MA-400HA hmc with the wine rack ATC. Is there a way to prevent the tool changer from returning a tool from the ready station back to the wine rack/magazine? Specifically, running a program that only uses 2 tools. As soon as the M6 completes the swap between ready station and spindle, the ATC2 takes over and returns the tool that just came out of the spindle even if there is a precall/preselect for that exact tool immediately following the M6.

Example:

T1
M6
T2
...
blah
blah
blah
...
T2
M6
T1 <--- tried adding this to keep T1 in ready station
...
blah
blah
blah
...
M2

At the start of the program, the machine waits for T1 to be fetched from the matrix magazine and placed in the ready station. Then, the first tool runs while T2 is brought to the ready station. After T2 is loaded into the spindle, the program runs and T1 is put away into the magazine.

The next time the program runs, the machine has to get T1 from the magazine again. It just had it! Why does it have to put it away?

I tried adding a T1 precall/preselect after the T2 tool change so that T1 would be in the ready station at the end of the program (and thus the beginning of the next cycle). Although this makes the start of the next cycle quicker, it then adds a delay after T2 is loaded because the ATC2 insists on putting T1 away in the magazine first so it can then retrieve it again and bring it back to the ready station. With the T1 precall after the T2 -> M6, the machine will not start moving until it has finished putting T1 away. Basically, ATC2 delays the start of T2's cutting code because it cannot fetch T1 until it finishes putting T1 away.

Any way to get the machine to just leave the 2 tools in the spindle and ready station?

Thanks.

[MCR-B II]

Second T2 command gives an alarm. Is it correct

[shawnc74361]

The T1 buy its self is just a pre call. It should be programed as fallows.

T1 M6 (tool command and tool change on the same line)
S10000 M3
T2 (pre call to stage the next tool)

if it programed like
T1 (calls T1 if called up already will fold it in and then back out)
M6 (changes tools)
T2 (call next tool)

My first example is correct way to handle the tool change.

[Caprirs]

Thanks for the replies.

No alarms with the code in my post above. Putting the T1 M6 as one block does cause an alarm, something about T command error. I'll try it again and see what the specific alarm is.

The machine runs error free with the code above. However, after running the arm to transfer tools between the ready station and the spindle, the machine waits until the outgoing tool is placed back in the wine racks before resuming the program. What I would like to do is get the machine to keep the outgoing tool in the ready station instead of putting it away in the wine rack.

[Superman]

No alarms with the code in my post above. Putting the T1 M6 as one block does cause an alarm, something about T command error. I'll try it again and see what the specific alarm is.

I assume it is a 5000 control
it may not like the T stated as a prep tool & then defined again on the M6 line. Your example in the #1 post is probably close to correct for that control

Is the tool return ( to the wine rack) part of the M6 cycle ?
- tool preselection may not be the actual problem
- your op manual should show the sequence of the toolchange cycle

[Caprirs]

I'm sorry, should have mentioned it is a OSP-P200M control.

Tool return to the wine rack seems to be part of the M6 command. If I run a program in single block, the M6 line will run the arm to swap tools, and return the outgoing tool to the wine rack.

I've read through the books but have yet to find the trick to keep that outgoing tool in the ready station instead of sending it back to the wine rack/magazine. I would think there is a code or parameter which I can use to prevent this.

I've also tried using M63 but the machine still insists on putting the outgoing tool away and leaving the ready station empty.

[OkumaWiz]

I've used it on a bit older machine and do not believe that you can prevent this from happening even on the newer machines. The Matrix is a bit of a stand alone device that takes over once the tool has reached the ready position. Thus it delivers what is asked of it and puts away what it's given. That's all.

I've run into the same problem where you can drill a small hole on all 4 sides/stations and be done with the tool before the matrix can deliver the next one.

The only way i've found to help is to place the tool in the rack as close as possible to the ready station so that the distance to go get it and put it back is reduced.

I guess it's the price you pay for having larger tool capacity. ;-)

Keep asking Okuma, they sometimes listen and add new features if enough people complain. (technically this should be an easy IF statement)

Best regards,

[Caprirs]

Thanks for the reply.

Can the tool change macro on this control be edited? I would like to add some IF blocks to get the macro to be a bit smarter. A few lines of code would make the machine much friendlier to use with regards to tools already in the spindle and ready station.

In some instances, I have added such IF statements to programs to make it easier for the other guys who run this at night. The fewer alarms they deal with, the more they can focus on making parts.

[OkumaWiz]

You can't edit the Okuma macro, but you can make it substantially smarter by defining your own G-code macro which uses the IF statements to eliminate the alarms. We use G111 on all of our machines and then set up the following program as a Library program so it is always available.

Then our program uses G111 T5 Q6 to make active tool 5 and prep tool 6. Even if they are already in the spindle or prepped.


$TOOLCHECK.LIB%
OTCHK
( SET GCODE PARAM. G111 TO OTCHK )
( AT TOOL CHANGE KEY IN G111 T= TOOL NO. Q = NEXT TOOL EX: G111 T1 Q2)
IF [ VTLCN EQ PT ]NST1 (ACTIVE TOOL)
IF [ VTLNN EQ PT ]NRT1 (NEXT TOOL)
IF [ VTLNN EQ 0 ]NOT1 (NEXT TOOL)
M64
NOT1 T=PT
NRT1 M06
NST1
IF [ PQ EQ EMPTY ]NEND (IF READY TOOL EMPTY/JUMP )
IF [ VTLNN EQ PQ ]NEND (IF PREP TOOL IS AT NEXT TOOL POS./JUMP)
IF [ VTLNN EQ 0 ]NTT1 (IF NEXT TOOL HAS NO VALUE)
M64 (NEXT TOOL POT RETURN)
NTT1
T=PQ
M356 (NEXT POT ADVANCE)
NEND G56 H=VTLCN
D=VTLCN
RTS
PQ DEF: WHEN P IS ATTACHED TO A LETTER IT BECOMES READABLE
%


Works great unless you already have 1000 programs with the old method. We've asked Okuma for this to be built into their macro, but so far no success. (heck if we can do it why can't they?)

Best regards,

[mqu02]

OkumaWiz: We have been using a macro very similar to what you posted for several years, however our does not incorporate the M356. Could you please tell me what exactly you are accomplishing (toolchange wise) with that function, or why it is in the macro?

[OkumaWiz]

On some of your machines such as the MC-V4020 the POT can be advanced to the Vertical position so as to make your tool change faster using the M356. When it is not used the POT stays in the Horizontal position and has to "fold down" once the M6 is issued.

Probably saves about 1.5 seconds per tool change. 10 changes = 15 seconds of reduced cycle.

Not all Okumas can use this...or need to depending on machine design.

Best regards,

[Caprirs]

Okumawiz,

I put your above macro into our machine but have yet to try it as the machine has been busy making parts.

Can you confirm that I have done everything correctly? I am still learning this control.

I created the macro except using G113 because G111 and G112 are already in use and I commented out G356 because this is a Matrix Magazine ATC.

• Macro is called FOOLSTOOLCHANGE.LIB.
• First line of the file is OG113.
• In Parameters -> G M Code, G113 is set to OG113.

[OkumaWiz]

Looks like you've got it correct. On older controls you had to "register" the .LIB program but you should be OK with the P200 I believe it automatically registers them if I remember right.

Best regards,