Assistance with an MSC 520 control please

This control is attached to a Mori Seiki MV40E. Absolutely new to me, I have been running a Fanuc "O" since I cant remember. At any rate can someone please explain how the tool change thing works. This is a rotary magazine machine, I am used to an umbrella type. It seems to me that the first Txx puts the magazine in position, then an M6 Txx actually does the tool change. I am just a litle confused about how I should go about setting this whole thing up. There is a screen where it shows what tool number is in what pot number, it seems to me that they should match but they don't. I see a real pain in the butt trying to keep track of where your tools are so any help you can give will be greatly appreciated.
Thanks
FredT

All the tool changers with an arm use a kind of internal counter.
It knows where the tool is, even if you do not.
To set it up, go to MDI and call for T1, it will put it in position to be changed.
Take it out, put your tool in it and stick it back into the same pocket, whatever the number.
From now on, that tool is #1 regardless where it sits in the tool changer.
When you program later:
T1 M6*, it will find it.
It sounds confusing, but try it.
The old and really slow toolchanger always put the tool back in the same pocket, on this, you can usually pre-select by programming T2 somewhere in the program and it puts the tool into position to be changed while you are doing something else, like actually making chips.
Maybe someone else has a clearer explanation, remember, my first language is german.
Heinz.
www.doccnc.com

Your tool change format will either be TXX M6; or Txx; M6; Either way you should be able to prestage. As Heinz was saying. Call tool one to the spindle and load it, so on so forth.

Anyone know how to change the parameters (fanuc 18i) so the machine will interperet a single line tool change format instead of having to two line them?


Husker

The T-code must be in a block ahead of the M06. They are different functions. The T will index the magazine to bring the next tool to the "waiting" position (Mori terminology). The M06 will cause the ATC to exchange the spindle and waiting tools. You can then program the next T to index the magazine so it will be waiting whenever the next M06 is read. Don't program T___ M06 together. There are machines that use this format, but Mori doesn't.

The ATC described above is known as a random-address. The spindle tool and waiting tool are simply exchanged, so the tools are constantly ending up in different pots (pockets). The software tracks this, so that is why you have the screen that shows the tool numbers assigned to certain pots. Toolchangers where the tool always ends up back in the same pots are called fixed-address. They are generally slower.

huskermcdoogle said:

Anyone know how to change the parameters (fanuc 18i) so the machine will interperet a single line tool change format instead of having to two line them?

Click to expand...

This is NOT a Fanuc function, and it is NOT a parameter. There is a great amount of misunderstanding about the PMC (ladder) software on a Fanuc-controlled machine (and many other brands, too). The toolchanger programming and operation are a function of how the MTB (machine-tool builder) wrote the software. That is why some machines have a T___ M06 format and some have it as T___ on one block, then an M06 on a following block.

Metaltech
I though it was something like that....It is confusing as hell when I have been using the other kind of tool changer for ........... well a long time. So I need to pay attention to the wcreen that keeps track of my tools and the pots that they are in. So after I run a program for a while it is going to be real difficult to know what pot your tools are in. However as long as the machine is running a program it is going to remember which tool is in which pot and when I call tool 1 from pot 5 and my syntax will be: T05; M06 T01; two seperate lines? Then the next time the program calls for tool 1 the program will be putting pot 5 on deck but tool 1 may not be in it, So how the hell do ya keep it straight?
Thanks
Fred

WE have 7 moris. Two have T#M6 Format and 5 have the T#; M6; format. Two of the machines are basically the same SH-500s but use different formats. It could be a Keep Relay or K parameter that would control this function. You can change a lot of things with the machine using these, if you have the MTB documentation. But many of them are not described.


Husker

Fred T said:

So after I run a program for a while it is going to be real difficult to know what pot your tools are in.

Click to expand...

Nope. You don't have to remember. That's what the tool-table screen is for. Just call it up and refer to it as necessary. This is typical for a random-access ATC.

Fred T said:

However as long as the machine is running a program it is going to remember which tool is in which pot and when I call tool 1 from pot 5 and my syntax will be: T05; M06 T01; two seperate lines? Then the next time the program calls for tool 1 the program will be putting pot 5 on deck but tool 1 may not be in it, So how the hell do ya keep it straight?

Click to expand...

Relax, it's easier than you think. At some point in the program, before the toolchange executes, command the T-code to index the mag to the next tool needed. When the current running tool finishes, move Z to ATC position (maybe zero return, or a second-reference point), then command M06. After the fresh tool starts cutting, you can now command the next T-code to have it ready at the next M06. The T-codes and M06 codes are on different blocks (lines).

Only command the TOOL number. Ignore the pot number, it's not your problem. The PMC will track the pairings between tool and pot, and will manage it for you.

One last thing: there will be a pot known as the empty pot, which should be shown on the tool table. Of all the pots in the magazine, plus the spindle, one of them must remain empty. The PMC will track it, you don't need to. Don't ever load a tool into it. However, the machine might do that, but then it will be emptying another pot while changing. The empty pot can be called to waiting-position by commanding T0. This will index the mag to the empty pot (unless the spindle happens to be the empty pot). The empty pot is used when assigning tools of large diameter that won't fit next to an adjacent tool. The ATC will go half-way through its cycle, swing the pot up, index the mag to the empty pot, then swing it down. The tool that left the spindle will be loaded into the empty pot. The empty pot will then no longer be considered the empty pot (duh, just stating the obvious here). When the next tool is called, and the large tool in the spindle is finished, the ATC will again go through the this Type B cycle. The pot will drop, the arm will grab both tools, then stop halfway through the 180° rotation. The pot will swing up, and the mag will index around back to the pot that the large tool originally came out of. The pot swings down and the arm finishes it cycle. This has put the large tool back into the pot it was originally in, where it would fit without interference from adjacent tools. In this case, the large tool has a fixed-address, always living in the same pot, while the rest of the tooling gets mixed around in the other pots.

Hah! That's prolly more than you wanted to know...

Metaltech
NO That is not more than I want to know, in fact I think I am on the right track so please bear with me once more. So to call a tool, lets say Tool 5 for the sake of this discussion the program would look like this:
T05;(puts tool 5 in the on deck or ready position, regardless of the pot number)
M06 T05;(actually performs the tool change)
I think I got it now please tell I am correct in my thinking. I hope I am not tol old to get thisLOL

Thanks
FredT

Close! The M06 stands by itself with no T-code, so it's like:

T05
M06
T06
M06
T07
M06...

You can call the T-code in the line immediately before the M06, or hundreds before. The idea is the T-code puts the tool on deck (as a baseball geek, I like your analogy), so when it comes time to use it, the magazine doesn't have to search for it. The M06 is strictly a command to run the ATC, so whatever tool is on deck, it will end up in the spindle. That means near the end of the program, you can call the first tool to have it on deck. You can choose to change tools so that T1 ends up in the spindle at the end of the program, ready for the next part, or you can do the toolchange at the beginning of the program. At the end means a little less cycle time. But, it also means no toolchange in the beginning of the program, instead assuming that T1 is in the spindle when the program starts. Some of the older Moris would give an alarm if the tool called was in the spindle (because the T-code runs the magazine and the tool wasn't in the mag). Later ones would expressly ignore a T-code followed by an M06 if that was the command for the tool already in the spindle. This way, you can call T1 into the spindle at the end of the program, then call it again at the top, just to ensure that T1 is actually in the spindle before starting cutting. Your machine should be new enough to ignore a redundant toolchange command like that.

As an aside, some machines won't let you call a T-code after another T-code. Once stating a T-code, you must command M06 before the next T-code, or you will get an alarm. Toyoda is like this. Very annoying if you're just trying to repair or adjust the magazine and want to index it a lot by one T-code after another.

By the way, in the example above, the T-code isn't the only thing that can be in that block. Same for the M06. For instance, my first two lines of a new tool would look like this:

N120 M06 (T15 .75 4-FLUTE EM)
N125 G00 G54 G90 X12.3456 Y-4.321 S1300 T0016 M03

Thank you so much to the tool change help, now for the next question; When I communicate with the machine via rs232, going from the machine to the computer all I get is jibberish on the screen, going the other way I get a buffer overflow error on the machine control. What gives here, Baud is 4800, even, 7,1. The software is ONECNC, The cable is from one of the other two fanuc controlled machines we have. The are both O-M's tho. I am "pretty sure" the data matches on both ends. I know if they dont I cant communicate. Since I am getting errors at the machine and jibberish at the computer I am once again confused...........
Thanks again for your time
Fred T

Jeesh, too many variables here. CNC--->PC: junk received is usually a baudrate mismatch. Make sure that the PUNCH CODE is ISO, not EIA on the mill. It would be fairly quick and easy to just change the baud on the PC and do a download, trying a range of settings to see if the 4800 you have set isn't what the machine is actually set to.

The buffer overflow is because the Fanuc told the PC to stop sending (while the buffer empties), but the Fanuc continued to receive characters. Make sure the handshaking method matches on both ends and matches the actual cable. Software handshaking XON/XOFF on the PC is known as "control-codes used DC-1 through DC-4" on the Fanuc. If the control codes aren't used, this implies hardware handshaking.

When I'm asked to either do a hook-up or troubelshooting of RS-232, the first thing I do is try it with my own laptop/software/cable to qualify that the machine works, before trying it with the shop PC. Perhaps you have access to another PC setup that is already operational.

Metaltech
Thank you for the time you took to respond to my questions. We are running at near light speed and communicating with no problems, thanks to you . I owe ya a beer, a real one, ont one of those that you can see daylight through either. Thanks again
Fred T

That's good to hear, really good. I often give advice, but many times there is no feedback to say "it worked", or "you're an idiot". I like to know either way, so I can also learn.

I'd love to take you up on that beer! How'd you know I like the real stuff? I truly would rather drink water than some of the horsepee that is popular in this country. The good thing is there are more great beers being made all the time.

Metaltech;
LOL I always say if ya can see daylight through it,it aint beer! So as I move forward with this frickin control I find I cannot make it do things that the other ones do. For instance, Once I pick up a part and define my G54 location and establish the tool lengths I can on a Fanuc O control, select manual, enter, G00 G43 H03 Z1.0 and tool 3 is one inch above the part asuming that tool 3 is in the spindle. Well with the new control I put tool 3 in the spindle, put in the above code and nothing happens. IMagine my frustration!!!!!!!!!!!!! Can ya shed some light on what is going on here?
Thanks
FredT

Well, maybe you stumped me this time. You said manual. Did you mean MDI? Also, is G90 or G91 in effect?

Hey Fred T,
where in OHIO are you?

Metaltech
Yes I mean MDI, sorry. I can command either G91 or G90, but assume, maybe foolishly that the control defaults to G90. I have tried several syntaxes and none of 'em seem to work. We have a Fanuc O on a different vmc and it is the same way. It is absolutely infuriating when you are trying to machine a fixture or a set of jaws.
Thanks
Fred T

MOri4200 I am in Tallmadge

Hey Fred,
I don't know when I will be down there again (Hermitage,PA).
I would like to help you but its a little too far from here.

Try to call HEINZ, he will help you!