[acrodave]

I'm a complete newbee in terms of a Mitsubishi control, having run a Haas for a dozen or so years, as well as a Hurco, and an Ajax/Centronics control....

The history ..... I bought a Mighty Comet with a Mitsubishi 520AM control, and have it up and ready to run, after some work, but when I loaded in my first program, and tried to run it, the tool changer crashed, immediately!

Tool changer works fine in MDI, and works fine in the only "left over" program in the machine, so it must be something in the program .....

I surmised that the program which runs ok, cancels all offsets, before commanding a tool change, and then re-calls them up after ..... it also retracts the Z to home before doing a tool change, so I assume this is what is needed, but it sure seems odd, as I never had to do that with the HAAS... all I did there was tell the thing to change a tool, and it did it...

Is there something I'm missing, or is is "normal" to have to cancel the offsets, with a G49, and retract the Z with a G28 before doing a tool change on this control???

Any help would be appreciated ..... the Mits manuals are so convoluted that it is hard to get the information needed ...... I'm sure it is in there somewhere, but it's well hidden.

Dave

[Caprirs]

It would help to understand what you mean by "crashed". What ran into what?

You should just be able to run a tool change by putting "T_ M06" on a line by itself. No special codes required other than the M06. This would be for a machine with the umbrella type ATC. On a swing arm ATC, the T_ and M06 would be on a separate lines.

[acrodave]

Umbrella type tool changer, and the tool changer went in as the head went down, so the bottom edge of the head (not the spindle, but the head itself) caught the edge of the tool changer and stripped a bolt holding the tool pocket ring onto the rotator, as well as bent that ring. I've fixed that, and have the machine running with a G28 Z0. and a G49 before each tool change, as well as putting the tool selection, and change command on a separate line from everything else, and then a G43 Hxx Dxx, on a separate line.

As to whether the head hit the tool changer, or the tool changer hit the head, it's a chicken and egg situation, and it happens pretty quickly, so it's difficult to see which moves first.

I suspect it is the G49 which cures the problem, but I haven't tried eliminating the G28 Z0. yet ...... the question is why either would be necessary????

The comment "on a line by itself" might be important, as I have always used a line like "N50 T5 H5 D5 M6" with the HAAS, where the G43 is modal, and included in a line at the beginning of the program. and it was this format which created the problem.

Thanks

Dave

It would help to understand what you mean by "crashed". What ran into what?

You should just be able to run a tool change by putting "T_ M06" on a line by itself. No special codes required other than the M06. This would be for a machine with the umbrella type ATC. On a swing arm ATC, the T_ and M06 would be on a separate lines.

[Caprirs]

All offsets should be canceled/ignored by the tool change macro. Did this just start occuring for no apparent reason? It sounds like the control has the wrong macro possibly?

Definitley leave the "H" and "D" out of the tool change block. Only the T_ M06 with nothing else in that block of code.

[acrodave]

Can't say it was suddenly, or for no apparent reason, as this is the first time I have tried to run the machine with one of my own programs ..... I've spent the last couple of months getting the RS232 to download the programs, (It had some bad components on the input board) as well as getting the rest of the machine all working properly. (as an example, the previous owner had disabled the shifting mechanism, and left it in low range all of the time .... turned out the problem was a nicked o-ring in the pneumatic cylinder .... it works fine now, also was getting spindle errors, and that turned out to be a FILTHY motor pickup)

I thought it was strange that the tool offsets would effect the tool change function ...... I'll try removing the G28 Z0., and the G49 I have inserted before each tool change, but leave the T_ M06 on it's own line to see if that was the problem ..... I was so used to putting the tool offsets on the same line as the tool selection, and tool change, (for the HAAS) that I never gave it a thought ..... old habits will die hard!

I suspect the Macro is fine, and this is an operator problem!!!

Thanks for your help

Dave

All offsets should be canceled/ignored by the tool change macro. Did this just start occuring for no apparent reason? It sounds like the control has the wrong macro possibly?

Definitley leave the "H" and "D" out of the tool change block. Only the T_ M06 with nothing else in that block of code.

[jetblackaircraf]

Dave,

can i get a copy of your tool changer program just for grins? I've been fighting an issue on my Dynamechtronics with Meldas 520 control for a while. Just curious to see the similarities.

Caprirs,

I remember getting help from you a long time ago with my tool changer. You directed me to Kevin S at mitsubishi. He and I have gotten the machine a lot closer to perfect than it was, but we are still stumped by the tool changer. It will change tools perfectly in MDI mode, but not in memory mode while running a program. The control gives a Z axis overtravel before the spindle should raise to clear the tool. Any ideas? Thanks!

Mike Black
[email protected]

[CNC Viking]

Hi,

Here is my Tool Change Program from my Mitsubishi Meldas 520 AMR in my 1996 Feeler FV-800 VMC. Ask someone experienced to analyse it so it works with your control. Note, this PLC's G30 is using the second Ref. Point. My manual says that if there is no Px designation after a G30 command, then the second Ref Point (P2) is selected anyway. Let us know if this works or not.

%
O9001()
N1#1=#4003
N2#2=#4001
N3#3=#1033
N4#4=#4120
N5IF[#4LE0]GOTO20
N6IF[#4GT18]GOTO20
N7IF[#3EQ#4]GOTO20
N8G40G80G63
N9M60
N10G91G30Z0M19
N11M40
N12G04P500
N13M12
N14G04P500
N15G91G28Z0
N16M41
N17G30Z0
N18M11
N19M42
N20G#1G#2
N21G64
N22M99

%

[CNC Viking]

Info, if you want to check or alter your Reference Points:

Procedure to set, or modify, the 2:nd, 3:rd and4:th Reference Points (G30P2, P3, P4)

1. Press DIAGN IN/OUT button.
2. Press Menu key under the screen until you can see the option PLC I/F.
3. Press PLC I/F key under the screen.
4. Make settings: DEVICE (1001) DATA ( ) MODE ( M ).
5. Press green INPUT CALC button. You will see no change, but leave it at that.
6. Press TOOL PARAM button.This brings you to the MACHINE PARAMETERS menu which is now open.
7. Press MENU until the ZP-RTN option is visible.
8. Press ZP-RTN key under the screen.
9. Edit P2,P3,P4 settings for X, Y, Z and 4:th axis. The 4:th axis page is not visible unless "4:TH REMOVE" is switched off in the PLC-switch area.
10. Press DIAGN IN/OUT button.
11. Press Menu key under the screen until you can see the option PLC I/F.
12. Press PLC I/F key under the screen.
13. Make settings: DEVICE (1001) DATA ( ) MODE ( U )
14. Press green INPUT CALC button. You will see no change, but leave it at that. This brings you back to normal "USER PARAMETER" status.

As for using the G30 command in programs: My manual says that if there is no Px designation after a G30 command, then the 2:nd Ref Point (P2) is selected anyway.