DMG Mori Celos - implications of disabling tool management?

Machine is an NTX2500 2nd generation.

I am finding the tool management system to be overly heavy, it creates a not insignificant time overhead when you do a lot of changeovers like we do.

We do everything in CAM and I am used to entering the absolute minimum of tool data at the control. I don't like the amount of data duplication that we're doing here.

I read in the manual that it can be disabled, and it explains how to do so, but doesn't say much of anything about what gets disabled and what is left. Just says "Call DMG Mori Service", which I can of course do, but I am curious if anyone has done it to theirs and has some experience of using their machine with it disabled.

Things like, I don't need redundant tools, so the serial number is just a pointless number that has to be entered. And I want to be able to load a tool manually that isn't assigned to a pot in the magazine. Etc.

Alternatively, the control has functionality to programmatically define tools, and I could add that to my post without much difficulty, but then I need a foolproof method to synchronise between machine and CAM which tools are already registered in the machine, and which need to be defined...

I don't think you are going to be happy disabling the tool management on an NTX. It handles all of the fun kinematics and tool length adjustments, etc... FANUC has some of that built in, but it's way more primitive.

I setup a program once to load all the tools straight from CAM on a MAPPSIV NTX. I really like working that way, and it's what I do in my shop. At the time though, I'm not sure the guys running the machine really liked it.

*edit* Another thought. Is it possible that you could benefit from some more training? A lot of folks even at DMG MORI don't really understand the tool management that well. They are used to setting up half a dozen tools for a demo/training, then walking away. I've seen a lot of machinists that were trained to feed the machine way more data than it actually needs. Part of what's nice about the CELOS tool management is that you can ignore half of it if you want.

boosted said:

I don't think you are going to be happy disabling the tool management on an NTX. It handles all of the fun kinematics and tool length adjustments, etc... FANUC has some of that built in, but it's way more primitive.

I setup a program once to load all the tools straight from CAM on a MAPPSIV NTX. I really like working that way, and it's what I do in my shop. At the time though, I'm not sure the guys running the machine really liked it.

*edit* Another thought. Is it possible that you could benefit from some more training? A lot of folks even at DMG MORI don't really understand the tool management that well. They are used to setting up half a dozen tools for a demo/training, then walking away. I've seen a lot of machinists that were trained to feed the machine way more data than it actually needs. Part of what's nice about the CELOS tool management is that you can ignore half of it if you want.

Click to expand...

Thanks for the reply, you've pretty much answered the first part of my question.

I think we're pretty good on training tbh, the guy that was here was good and I've been using it long enough to have a pretty good handle on what can be omitted at the control. I'd just be happier with something a little more... lightweight I suppose. Loading the tool data from CAM would negate that altogether, if I can figure out how to keep it all in sync.

While I have your attention, if I let it be as is, are you aware of any way to call a tool that isn't registered in the magazine to load manually? I fairly frequently am working with tools that are too long or too delicate to go in the magazine (gundrills, long silent bars etc) and the only solution they were able to give me was to assign a space in the magazine and call the tool normally but load it by hand and remove it by hand before the next tool change. I'd really like to have a better solution for this but I'm drawing a blank.

I'm not familiar enough with the MAPPS V NTX's to say with certainty how you can handle large tool changes That said; the fact that your DMG MORI team hasn't given you a large tool solution your happy with is a huge red flag from a training standpoint. It might be worth hounding them. If nothing else maybe push for future changes. On Siemens controlled machines it's just a check box on the tool data.

With some parametric programming you could probably set up a user macro so that every time you do a regular tool change to a certain range of tool numbers it just automatically treats it as a hand load/unload.

boosted said:

I'm not familiar enough with the MAPPS V NTX's to say with certainty how you can handle large tool changes That said; the fact that your DMG MORI team hasn't given you a large tool solution your happy with is a huge red flag from a training standpoint. It might be worth hounding them. If nothing else maybe push for future changes. On Siemens controlled machines it's just a check box on the tool data.

With some parametric programming you could probably set up a user macro so that every time you do a regular tool change to a certain range of tool numbers it just automatically treats it as a hand load/unload.

Click to expand...

I hear you on the training, but I have scoured the manual cover to cover, and it genuinely seems like the method they gave me is the only way to do it with the tool management system as is. I don't feel that there's much to gain by hounding them further, and from what you've told me it sounds like I don't want to disable the tool management!

There is just no way to simply call a tool offset, only a physical tool, and physical tool changes only work for tools that are registered in the magazine, otherwise alarm. At the root of it is the absence of a real global tool offset table; there is only a per tool offset table that is loaded by the tool management system when you do a tool change.

Re. parametric programming, each tool can have multiple offsets, so in theory it would probably be possible to have one tool registered in the magazine that was the "manual tool" and write a macro to enclose the toolchange to handle that. Still a bit of overhead to manage that.

gregormarwick said:

so the serial number is just a pointless number that has to be entered.

Click to expand...

The serial number is optional on all mills with CELOS. Is this not the case on the NTX?

For example, I can use T10001 M6 (Serial 1, Group/Tool# 1), or simply use T1 M6 like every other machine. Both will work by default.

The main thing that TLM changes is your H and D offsets. You can still have multiple offsets per tool (needs to be enabled), but your H and D numbers are going to 1, 2, 3, etc. So tool 123 might look something like:

T123 M6;
G43 H2;
G41 D2;

And I want to be able to load a tool manually that isn't assigned to a pot in the magazine. Etc.

Click to expand...

I create a dummy tool number in the TLM, e.g. T999.

If you're loading some sort of indicator that will be removed before the next operation, you can also start with a T0 M6.

Orange Vise said:

The serial number is optional on all mills with CELOS. Is this not the case on the NTX?

For example, I can use T10001 M6 (Serial 1, Group/Tool# 1), or simply use T1 M6 like every other machine. Both will work by default.

The main thing that TLM changes is your H and D offsets. You can still have multiple offsets per tool (needs to be enabled), but your H and D numbers are going to 1, 2, 3, etc. So tool 123 might look something like:

T123 M6;
G43 H2;
G41 D2;

Click to expand...

When I said "the serial number is just a pointless number that has to be entered" I meant when entering the tool data, not when calling it.

I don't have any other Celos machines, so I don't know how the ntx differs, but I can tell you how it works.

Tools are not called with a Txxxx like on a lathe, or with an M6 like on a mill.

Basic tool change on the NTX is:

T1
G361 B-90. D0
T2
G43 H1

Where T is the group number. Which serial number is selected is determined by the tool life management, probably it can also be explicitly specified as per your example but I've not tried. G361 performs the physical tool change and has a few variants that affect the motion during/after the toolchange. D determines the tool orientation/use, D0 = milling tool, D1/D2 are oriented turning tools. Second T prestages the next tool.

There doesn't appear to be any way to call a tool without using one of the G36x variants, and all them alarm out if the tool is not registered in the magazine. There are no programs in the 9000 range that are mapped to the G36x codes, so I don't know how or where those are defined in the control and can't look at them to see how they work internally.

Unfortunately the tool management is totally different on an NTX. It's why I can't say for sure how it should work on that machine. In the early days the FANUC CELOS was a super buggy POS, and we weren't selling any. We sold a ton of MITSUBISHI CELOS machines though, and even those were really poorly understood. I promise you though that half of the applications staff at DMG MORI still doesn't know how it can or should be tweaked. Hooking up with the right individual who has factory support and a willingness to dig into it will solve your problems.

The G36X codes aren't going to be user-editable, but you should be able to build a user macro that piggy backs on it. Sort of like building an M6 macro that calls M6 at the end.