Printable View
Hi All,
I have a Supermax max5 VMC and I would like to run multiple cycles without the tool being taken out after each M02 or each M30. I assume I need to use a subroutine to do this but do not understand how to do this? I got this machine used and did not get a user manual with it, help please !
regards, John S. Wracher
Accra machine shop, Inc.
what is your control? and what do you mean by "the tool being taken out after each M02 or each M30".
Do you want to keep spindle running between each cycle?
It depends a lot on your control as to the format for calling up and running a sub routine.
On a Fanuc control you would have your subprogram numbered like O2300, and your main program like O230.
In your main program when you want to run your sub routine you call up your sub by inserting an M98P02300, at the end of your sub you need the line M99 instead of the normal M02 or M30 so it knows to jump back into the main program where it left off. That's it in a nutshell. Very simple to impliment so long as you know the format required of your machining center.
What kind of cycles are you running? Trying to get a visual of what you want to do. You don't necessarily have to end a program with an m2 or m30 unless you want it to rewind. You could even use a 'GOTO' line at the bottom of your cycle with a line number reference if your machine supports this feature. I might have something like this:
N5000 M0; (I'd want an opportunity to pause the cycle before restarting it so M0 is used)
......
......
cycle;
.....
GOTO 5000; (you might include a block delete feature here if you want to stop the cycles)
It's a little sloppy, but it would allow you to bypass an end program/rewind statement and you could stop it all by hitting 'Reset' or turning 'Block Delete' on.
Thank you all for the quick responses, I can see I forgot to include some pertinant information so here goes. I am running a Fanuc control o-m control on a Supermax max5 VMC. What I meant by not takeing the tool out every time is let's say I have an air vise set on the table, I am going to drill 2 holes and then have the machine returne to a home position and stop while I put another piece in the vise and then hit the cycle start button again. The way this machine works it will not start another cycle with a tool in the spindle, so I am forced to remove the tool at the end of the program cycle. You can see what I wast of time and wear and tear on the machine if you were cycling many thousands of cycles. Thank you for your time, I will look for your reply.
regards, John S. Wracher
Accra Machine Shop, inc.
A simple way to do this is a M0 at the end of the program followed by GOTO 10 (beginning of the tool)
Be sure to check that you turn off coolant, and the spindle ect. as well as start/set everything back up correctly inside your loop.
On another note, the requirement to have the spindle empty to start seems a bit odd. Perhaps you can talk to the machine tool builder to find out how to change that. There is a pretty good chance the fix is small and relatively painless.
Best method is to have the progam operate as you would normally have it run
ie
1-> header
2-> select the tool
3-> body of the program
4-> return the tool
What you want is to continually cycle #3
Block skip ON = program runs thru to the end normallyCode:...
N19 T2M6
/N20 M0
N21 S-- M3
M8
....
N200 M9
N201 M5
N202 G91 G28 Z0
/N203 G0T0 N20
N204 T0 M6
N205 M30
%
Block skip OFF = prog. will load tool, stop on M0, run to GOTO command, jump back to M0 and stop. Turn the block skip ON when in the program body, it will then run thru to the end as normal.
If you have more than one tool in the program put the M0 and jump to spot before the first toolchange
Wouldn't it just be easier to replace the m30 or m02 with m99 and put an m00 on the line before it? Or have I missed something?
Quote:
Originally Posted by Jawbreaker38
That's exactly how you could do it on a lathe. Of course a lathe wouldn't be causing his problem. An M02 or M30 would work fine. Never programming for a mill, I haven't a clue. My only question about using the M99 would be "How would the machine react when it sees the T2M6 block." I don't know, but wouldn't mind knowing.
Maybe some others could clarify the point for me. Not that I will ever get the opportunity to put that knowledge to work. :(
I have a mill part I run for a customer with an 11 second cycle time. Code is essentially:
G0 G40 G90
M0
T1
S3500 M8
G0 Xx Yy M3
G0 G43 H1 Z.025
....
M9
G0 Z5.
G28 Y0.
M99
M30
The first part requires pressing the Cycle Start button twice, but then each subsequent part only requires one Cycle Start. Spindle remains spinning while running through all the parts in the job. By eliminating the spindle start/stop, the cycle is much quicker.
This is on a VMC with a Mitsubishi M3 control.
Quote:
Originally Posted by Caprirs
I gather from your example that if the OP takes out the M6 then he should have no problem either.
Let me try to explain this better. The program cycle will not run if there is a tool in the spindle before it is started. So after the program ends the tool needs to be taken out befor the program will run again. Thank you all who have responded.
regards, John S. Wracher
My machines do not require using the M6. Calling the Tt runs the tool changer as this has an umbrella type, not swing arm ATC. M6 is redundant if the machine cannot pre-load from the magazine.
By having the M99, the program never ends. As far as the control knows, it is forever running the program and you only entered an M0 to change clamps or clear chips.
A modified version using a GOTO can eliminate the control seeing the tool call line more than the first time.
G0 G40 G90
T1
N1000
M0
S3500 M8
G0 Xx Yy M3
G0 G43 H1 Z.025
....
M9
G0 Z5.
G28 Y0.
GOTO1000
M30
Again, my machines are Mitsubishi control so format may be different. This leaves the spindle running which may or may not be safe for your application. Likely not OSHA approved method. :D
I am confused why your machine will not cycle with the tool already in the spindle. That is something I've never encountered before. Have you contacted the builder to see if there is a parameter that is set incorrectly or you have the wrong tool change macro?
Yes I am going to contact the machine builder to see if I can maybe change a parameter that would leave the tool in and recycle. Also I tried the G0T0 trick today but apparently my control does not like it. It gave me an error. Thanks for your reply.
regards, John S. Wracher
Without attempting to be insulting, are you using "GOTO" or "G0T0"? All letters, no number zeros.
Quote:
Originally Posted by Caprirs
I tried this in a different application today on a lathe, but it wouldn't post it as mentioned. It tried to enter it as an invalid tool number. I run numerous parts in the same family and would like to use this feature as described, I get tired of adding the block skips on each line. I really want to use this, any advice?
No I must confess I used zeroes instead of letter o. I will try this again, Thank you for the sugestion.
regards, John S. Wracher
Using an actual sub-program may be the best bet if 'GOTO' is giving trouble.
For this one, you say that you want to drill a cpl holes in multiple parts without changing the tool. I would set it up like this :
O11111 (MAIN PROGRAM)
T1 M6;
G00 G54 G90 X0. Y0. S1000 M3;
G43 H1 Z.25 M8;
/M0;
/M98 P2222 L99 (PICK ANY NUMBER LARGE ENOUGH TO COVER ALL PARTS);
G49 Z0. M9;
G28;
M30;
O2222 (SUB-ROUTINE)
M0;
G81 ......... (WHATEVER DRILL ROUTINE);
G80;
M99;
This uses the 'Block Skip' feature to allow you to recycle the sub-routine indefinitely. Just turn block skip on when you want it to stop.
Hi All,
I realy appreciate all the help with the sub-routine programming, but now I am having an even bigger problem trying to understand the tool changer on this machine. The machine is a Supermax max5 VMC with a Fanuc O-M control and the tool changer is the belt style. I was told to load tools into the changer and to initialize them to the control you have to first, push T#,input,cycle start then m6,input,cycle start then load that tool manually into the spindle and then perform the same opperation again for the next tool. The first tool is then loaded into the magazine with each successive load. The machine does not seem to remember the proper tool numbers with this routine. And yes I did try starting with an M19 as somebody recomended earlier. Any help would be a real blessing.
regards, John S. Wracher
M19 is spindle orientate, this rotates the spindle and locks it aligning the drive keys to suit the toolchange arm and carousel ( chain or umbrella styles). It is a hidden command inside a M6 ( toolchange cycle )Quote:
Originally Posted by accramachine
Txx is to pre-select or pre-stage the tool ready for toolchanging
M6 is the actual toolchange cycle, if no tool is pre-staged most machines will error.
This can be shortened to Txx M6, then cycle start
The routine that you are instructed to use is a safe method of loading the tools into the machine, the machine will remember what "pot" it has placed that tool.
There is nothing worse than calling up a drill cycle and expecting a drill when there is a face mill in the spindle
With the side mount swing arm type tool changers, the tools do not stay in assigned "pots" on the belt/magazine the way they do on the umbrella types. With umbrella type machines, Tool 1 is always stored in position 1 on the carousel.
On swing arm machines. the purpose of loading the tools through the spindle is to give each tool to the machine via the spindle and let the machine assign it a "pot" on the belt/magazine. However, once a program has been cycled and the tools have been sequenced, the tools will not necessarily be in their original "pots". For example, suppose the machine starts with T1 in the spindle, pot1 on the belt/magazine is sitting empty, and T2-Tx are in pot2-potx on the belt/magazine. When running a part program, T2 is called. The belt/magazine places T2/pot2 at the ready postion. When M6 is commanded, the swing arm puts T2 into the spindle and puts outgoing T1 into pot2. Pot1 remains empty. The tool number will no longer match the pot number. Gets very confusing if the program skips around with tools, like going from T1 to T14 to T23. In that instance, T1 winds up in T14's pot, then T14 goes to T23's pot.
I think there are some machines which have an intermediate pot between the belt/magazine and the swing arm. This permits the tools to stay in assigned pots on the belt/magazine. I think this style is only found on really big horizontal machines.
As a useless tangent, this is why machine tool builders will sometimes claim tool capacity on swing arm machines to be xx + 1 as the belt/magazine can be full and one tool in the spindle and the tool changer will still work properly. All pots can be occupied and a tool in the spindle. Umbrella types must always have an open spot in the carousel to accept the tool currently in the spindle.
All twin arm changing machines I have seen have a tool table page on the control which will tell you which tool is in which pot number. Everything works fine until something happens and the table no longer matches the hardware.
It gets even more fun if you have an oversize tool where the adjacent pots need to remain empty.
What is the best way to initialy get the tools loaded into the system so that the control knows where they are. I am currently having dificulty getting the machine to remember where they are.Thank you.
regardss, JohnS. Wracher
The “best way” is probably a bit too subjective for something like this. :)
However when all else fails you can.
1: Pull all the tools out of the machine.
2: Reset the tool table, some machines will have a command to do this, others you need to do manually (pot 1 = tool 1, etc.) the procedure would be in the machine manuals.
I have seen a machine that would get messed up to the point it would show tool 4 in pot 6 and also in pot 11 etc. and tool 7 may not exist anyplace.
3: Load the tools back in thru the spindle.
If you want to keep the tools from moving around you can if you are willing to do extra tool changes. This just simulates the way an umbrella type of changer works and wastes a lot of time.
Code:O0001
(TOOL N IS SOME UNUSED TOOL NUMBER)
(THIS CAN GET MESSED UP IF TOOL)
(CHANGES ARE DONE USING MDI WITHOUT)
(THE TN M6 CHANGE BEING DONE)
…
TN M6
T01 M6
…
(machine with tool 1)
…
TN M6
T02 M6
…
(machine with tool 2)
…
TN M6
T03 M6
…
(machine with tool 3)
…
TN M6
(ETC.)
G30
accramachine,
First, before you started did you clear or reset the tool magazine data? Either by editing a table of data, or a M-code or similar? Check your manuals for how. You will want to reset the data so pocket 1 = tool 1 ect. initially to make sure that isn't a cause of problems.
When you say it forgets where the tools are, how are you determining this is the case?
If you do T1 M6 (insert and cycle start) load a tool, then repeat for T2, then T1 M6 again will the first tool be called back to the spindle? If so, this is all that matters (provided it is true for all the tool numbers).
Another possible method if you can insert the tools into the magazine by hand. Set tool numbers to = pocket numbers like above, then manually put in the tools. This ONLY work if you have set the pockets to equal the tools, and have not done any tool changes yet. AKA setup use only!
I didn't get a manual with this machine, so I am not sure how to clear the tool data. What I meant by the machine not remembering is, when in MDI I load tools and then go back and call them up, they do not come up . ie; I call for T1 and get T2 and so on .
Well lacking the actual manual your in a bit of a mess.
One thought, I have seen where having T# M6 on the same line would not work right. Try placing them on separate lines
T#
M6
Another thing to try is just command T#'s and check the tool it calls up to the ready pocket without the M6 getting involved. So T1, note the tool called, T2 note that one... Then come back and recheck T1 T2 ect. If you do not do a M6 will it be consistent?
With you lacking any other source of information, I'll offer some possibly dangerous for the machine advice. Observe the machine carefully before you even consider changing anything! On my machine the tool to pocket location table is in the diagnostics screen. Number 600 is the tool in the spindle, 601-624 are the tools in pockets 1-24 I have NO IDEA if this is the same for your machine! You can look at it and see if the changes in those numbers match what the machine is doing, and consider resetting them to the pocket numbers for a fresh start.
Thank you for the suggestions, I will look into it. Thanks again.
regards, John S. Wracher
For everyone who helped me with suggestions on how to re-run a cycle without taking a tool out of the spindle, I finaly found out how to do it. I simply leave a tool change number out of the program and then the machine will allow me to start the cycle with the tool in the spindle. Thanks again to all who helped me with this.
regard, John S. Wracher
Sounds too easy. :) We like secret parameters that need changing.
John,Quote:
Originally Posted by accramachine
Most of the time this is done in the tool change program. If you don’t want to have to edit your program and take out the tool change all the time then you can still use the M6 and call a macro with it and bypass the M6 in the macro if the current tool in the spindle matches the tool you are calling.
What you have to do is see if there is a parameter that tracks the current tool in the spindle on your control. If there is not one you can set one up. If your machine does not call a macro with the M6 which I ass u me it is not then you have to set the parameter to do so.
On your control #240-#242 willl call program 9001-9003 so if you want program 9001 to be your tool change program set parameter #240=6. Now when you command an M6 it will call program 9001. Now pick a variable that you want to use to track the tool in the spindle. Make sure you use variables #500 and above because they don’t reset or clear at power down. Lets just say #500. Manually set #500= to the current tool in the spindle. Now you can write your tool change program.
O9001(TOOL CHANGE PROGRAM)
G40G80—(tool dia cancel & canned cycle cancel)
IF[#4120EQ#500]GOTO1--(jumps to N1 and skips tool change if calling tool in spindle)
G91G28Z0M9—(tool change position in Z & coolant off)
M19--(tool orientation)
G28Y0M5—(tool change position in Y & spindle stop)
M6—(tool call of modal T value)
N1—(address to jump to if calling current tool in the spindle)
#535=#4120—(sets #535 equal to the tool that was called to the spindle)
M99
(*note #4120 is your modal “T” so when you program a T5M6 #4120 will be set to 5)
There is much more you can add to this if you want to. I have all of my speeds and feeds set in this program along with the G43H(). This way I don’t have to worry about hard coding it or fatfinger in the main program. It always sets everything to the tool I am calling.
There is an exception to doing the above. If your ladder is written to stall the program if you are calling the current tool in the spindle then I have another fix for you. I came across this when setting up a machine that had the ladder alarm when calling the current tool in the spindle. What MTB would ever do this is beyond me :mad:. I have never seen anything like it before. The ladder was burned into Eeprom so I did not bother going through the hassle of changing it.
Stevo