Manual tool changing method on a VMC

vmipacman · Aug 21, 2017

Is there a way to write a manual tool change into my program rather than an automatic one using the toolchanger? My '96 Supermax needs to have the toolchanger swing gearbox motor rebuilt so I have stopped using toolchanges until I get it done.
For the last couple parts I have just made each tool its own program but that's a PITA. I was thinking there might be a way to single step through a manual change. Like a Z-axis move, M01, tool release, pause, M01, tool insert, pause, M01, and back to program.
My main issue is I can't figure out how to tell the drawbar to release inside the program.
My toolchange program is O9000-something (ran across it but not looked closely). Would that have the commands for each step I need?
Thanks

Bobw · Aug 21, 2017

I'm not sure you would want the PROGRAM to spit the tool out, if your hand isn't there
you're going to have some busted tools...

Don't you have a Tool In/Out button?

Cancel tool height offset, bring the head up.. M0.

Pop tool out, Pop new tool in, call up a different height offset and get busy.
I had to do that for a few days on one of my Fadal's while waiting for a proximity
sensor.

Its going to be a pain in the ass if you can't release the tool while the program is active,
I wonder if that would be something that you could change with a parameter.

I'm going to take a guess that you won't find an M code that will simply release the tool.

DMF_TomB · Aug 21, 2017

vmipacman said:
Is there a way to write a manual tool change into my program rather than an automatic one using the toolchanger? My '96 Supermax needs to have the toolchanger swing gearbox motor rebuilt so I have stopped using toolchanges until I get it done.
For the last couple parts I have just made each tool its own program but that's a PITA. I was thinking there might be a way to single step through a manual change. Like a Z-axis move, M01, tool release, pause, M01, tool insert, pause, M01, and back to program.
My main issue is I can't figure out how to tell the drawbar to release inside the program.
My toolchange program is O9000-something (ran across it but not looked closely). Would that have the commands for each step I need?
Thanks

.
M0
take out of memory and put in manual mode like handle
you do tool change manually not in memory mode. operator near machine in memory mode is dangerous
,
when done put back in memory mode

vmipacman · Aug 21, 2017

Since I could not find anyone else asking this question, I figured this might be an oddball request. i.e. not the right thing to do.

As far as the program releasing the tool, I would put a M01 (with maybe a 3 sec pause too) in before the release so I could put hands on the tool when released.

I do have a tool in/out button, but I have to be in JOG, then jump back to the program, make sure its where I want to start, etc.

I will double check to see if I can leave the program active and use the tool in/out button, but I'm 99% sure it have to be in JOG mode for the button to work.

Booze Daily · Aug 21, 2017

It's like Bobw said. As long as you don't hit RESET you should be fine.

DMF_TomB · Aug 21, 2017

vmipacman said:
Since I could not find anyone else asking this question, I figured this might be an oddball request. i.e. not the right thing to do.

As far as the program releasing the tool, I would put a M01 (with maybe a 3 sec pause too) in before the release so I could put hands on the tool when released.

I do have a tool in/out button, but I have to be in JOG, then jump back to the program, make sure its where I want to start, etc.

I will double check to see if I can leave the program active and use the tool in/out button, but I'm 99% sure it have to be in JOG mode for the button to work.

most cnc will not do a manual tool change in memory mode as memory mode is dangerous for operator to be near reaching in etc when active. many cnc in memory mode will not respond to mcode to go into neutral and or release tool clamp. probably a parameter settings prevents this. all machines i have run tool unclamp switch for operator will not work in memory mode. usually it is to force operator to take out of memory mode
jog, handle, rapid are all manual modes and take it out of memory

Mud · Aug 21, 2017

All my machines have had a way to designate a tool as a manual tool change tool, for use with tools too heavy or too big to put in the changer. But none of them were Fanuc. Perhaps your operations or programming manual will have that information?

DMF_TomB · Aug 21, 2017

usually on long tool that will not go through tool changer door i add
edit program add block delete at programmed tool change
M0 (turn on block delete)
M0 (to warn load tool and tool offsets)
after tool op done then M0
turn off block delete
unload tool and tool offsets
.
picture of broken drill bit that was trying to go through tool changer door and broke and went flying through cnc monitor of machine next to it
.
important not to put too long a tool in tool changer magazine

706jim · Aug 21, 2017

We had a tool changer malfunction on a large machining center. Until it was repaired, we built a plywood tool holder rack and changed tools manually at the zero return position. As a program mod I would just insert M00 codes at the tool change program locations and edit them out later.

Vancbiker · Aug 21, 2017

Mud said:
All my machines have had a way to designate a tool as a manual tool change tool, for use with tools too heavy or too big to put in the changer. But none of them were Fanuc. Perhaps your operations or programming manual will have that information?

Including that capability is determined by the machine builder's ladder program, not Fanuc. The ladder logic is totally capable of switching toolchange behavior based on tool call information passed through the program or entered in the tool/pot data table.

@OP
Other than maintenance mode M-codes that some builders use, I've never seen a machine builder include a "standard" M-code to unclamp the spindle in their ladder program. I'd be very surprised to hear that the ability exists on your machine. As to needing to be in a manual mode to use the tool unclamp pushbutton, that is a common behavior chosen by machine builders for the exact reasons outlined by DMF_TomB.

Whysosharp · Aug 21, 2017

Yeah the best thing is to go manual then back to memory. We have 4 supermaxs from the 90's and that's just how you gotta do it. You can actuate certain parts of the knockout and clamp unclamp but I strongly advise against it

cwtoyota · Aug 21, 2017

I have a couple parts that I use a 6" wheel to cut a slot down the side.
Since it's possible to crash that large diameter tool in the magazine, I just do a manual tool-change.

Program starts with all the regular stuff ,work offset, etc and is at G43 offset H0 (no tool).

M0;
(MANUAL TOOL CHANGE T22);
(T22 - 6" DIA SLITTING, 30FL, HSS);
(CHECK OFFSET H22);
G43H22Z1.5S100M13;
.
.
.
M9
M5
G28H0Z0T16;
M0;
(MANUAL TOOL CHANGE REMOVE T22);
G0X5.Y5.M6;
G43H16Z1.S3600M13;

This code works well for my needs on my specific machine (Fanuc).

This is off topic: In my case, there is another solution to oversized tools.
The machine tool builder (Kuraki) did include a specific function M16 to always return the oversized tools to the same pot in the magazine. Using M16 with my example above, T22 is oversize and I could leave #21 and #23 pockets empty in the magazine. M16 would always replace T22 back to pocket #22 so that it would not crash into other tools.

Vancbiker · Aug 21, 2017

cwtoyota said:
.....This is off topic: In my case, there is another solution to oversized tools.
The machine tool builder (Kuraki) did include a specific function M16 to always return the oversized tools to the same pot in the magazine. Using M16 with my example above, T22 is oversize and I could leave #21 and #23 pockets empty in the magazine. M16 would always replace T22 back to pocket #22 so that it would not crash into other tools.

Better machine builders include features like that. Older Moris used 9000 series tool numbers (ie, T9010) to make sure they returned to the same pot. Additionally they had 8000 series tool numbers that designated an extra small diameter tool. Then one could specify 8000 series tools adjacent to a 9000 series and it would always place the 8000 series on either side of the 9000 series large tool. In that way one could still use their full number of magazine pockets.

mikiemus · Aug 25, 2017

vmipacman said:
Since I could not find anyone else asking this question, I figured this might be an oddball request. i.e. not the right thing to do.

As far as the program releasing the tool, I would put a M01 (with maybe a 3 sec pause too) in before the release so I could put hands on the tool when released.

I do have a tool in/out button, but I have to be in JOG, then jump back to the program, make sure its where I want to start, etc.

I will double check to see if I can leave the program active and use the tool in/out button, but I'm 99% sure it have to be in JOG mode for the button to work.

On a Fanuc control I would test to let the machine get off 'hogging' the Auto mode. Test if it is possible on yours.

M0;
;
;
;
M0;

What happens is machine stops at 1st M0,
Then you go 'single block' and press 3 times,
and stop at the last 'semi-colon' before the M0,
this because the readahead in memory should release.
(Some machines has up to 6 blocks ahead, this example is for 3)
Now press Tool-change button, the control should now be
on 'finish block execute mode', sorta 'program done'.
The last M0 is there only if you just pressed to many times...

I did this back late 1990's on a machine with similar problems
and had to juggle tools manually. Pain, but worked.

GL

angelw · Aug 25, 2017

mikiemus said:
On a Fanuc control I would test to let the machine get off 'hogging' the Auto mode. Test if it is possible on yours.

M0;
;
;
;
M0;

What happens is machine stops at 1st M0,
Then you go 'single block' and press 3 times,
and stop at the last 'semi-colon' before the M0,
this because the readahead in memory should release.
(Some machines has up to 6 blocks ahead, this example is for 3)
Now press Tool-change button, the control should now be
on 'finish block execute mode', sorta 'program done'.
The last M0 is there only if you just pressed to many times...

I did this back late 1990's on a machine with similar problems
and had to juggle tools manually. Pain, but worked.

GL

If I understand you, that you're saying that the Tool can be released in Auto Mode, this would only be the case if it were allowed in the MTBs Ladder Program. It would be most common for an Internal Ladder Relay for Auto Mode to be included in the Ladder Rung for Manual Release of the Spindle Tool to inhibit such an event when in Auto Mode.

Regards,

Bill

adama · Aug 25, 2017

One thing for certain, bet come about 4 hours your suddenly going to bump up that tool changer repair on the to do list, manual tool changeing sucks!

vmipacman · Aug 25, 2017

adama said:
One thing for certain, bet come about 4 hours your suddenly going to bump up that tool changer repair on the to do list, manual tool changeing sucks!

Thats right! Not my replacement motor today. Soon it should be worry free toolchanges again.

So I was going to DNC the toolchanger program to my laptop and post it but I have not had a chance yet. Looks like there might be a M code for actuating the drawbar? I see the safety aspect of backing out of the memory before sticking your hands in the machine. This is a Fanuc OM btw.

Search

Largest Manufacturing Technology Community on the Web

Search

Manual tool changing method on a VMC

vmipacman

Cast Iron

Bobw

Diamond

DMF_TomB

Diamond

vmipacman

Cast Iron

Booze Daily

Titanium

DMF_TomB

Diamond

Mud

Diamond

DMF_TomB

Diamond

Attachments

706jim

Titanium

Vancbiker

Diamond

Whysosharp

Cast Iron

cwtoyota

Cast Iron

Vancbiker

Diamond

mikiemus

Aluminum

angelw

Diamond

adama

Diamond

vmipacman

Cast Iron

Similar threads