Mori Seiki NH4000 T com

[pieface]

We have just bought 2 new NH4000's to add to our existing range of Hitachi Seiki machines. An issue has arisen where the Mori does not seem to acknowledge a T command on the same line as the M6. eg. T1M6;
It will load whatever tool is in waiting pot regardless of the T value on the same line as the M6. Does anyone know of a way around this other than having to keep the M6 on a seperate line. We do not have any problem with this on any other machine control (Mainly Fanuc and Seicos) so I'm reluctant to have to change our recognised program format (T1M6; NOT T1;M6
Thanks

[pieface]

Foe interest to anyone else who hits this. we nailed the issue to simply the T code having to FOLLOW the M6 command. Our Hitachi's are similar except they will generate an alarm if T?M6 is not in correct sequence, the MOri will quite cheerfully carry on trying to machine with the wrong tool. I've since added a macro line into the tool change sub program to alarm if there is no T value following the M6 command. Problem solved.

[the thrill]

I always use T*;M6 because of the fact that mori's do not like T*M6 on the same line for some reason. Funny part is I don't know why and I work for Mori LoL! Make sure you change your tools to light tools in the tool register screen on the NH4000 because it will make tool changes lightning fast. Plus, if you prestage the tool and command your zero return for x and y and the M6 on the same line the shutter will start to open a little sooner than if you put the M6 on a separate line (I.E. T1;M6;T2;(program);G91G30P2X0Y0M6). Is this an MSG501 or MSX501 control?

[pieface]

Cheers for the info. It's an MSX501. I'll have a look at working around the M6 on the same line as X and Y moves, but we use a lot of unskilled labour who occasionally dabble, so I'm inclined to stay with the safety I've put in, which guarantees that unless the tool call is in the correct sequence with the M6, the machine will alarm (Even in MDI). Before I added the macro line into the M6 sub, I had notified Mori UK, through their applications guys, of the issue. They seemed to be concerned, and quite rightly. I was surprised that they didn't seem to be aware of the issue and they have notified Japan (Apparently). It is dangerous, as when the code is incorrectly sequenced (T*M6), then the machine WILL load whatever happens to be in the preselect pot and carry on machining with it as if the correct tool were loaded, hence potential costly disaster.
Regarding the light/heavy tool set up, I haven't really looked hard at it yet (1st Mori for me), do you know if the machine defaults to heavy tool? I haven't specified anything for any of them as yet. The machines are running well on a mass production job, and I'm on other projects right now, but I do need to re-visit in the new year to set up tool life monitoring, so that is something I could do simultaneously. Thanks again for the reply.

[the thrill]

the machine default is heavy tool so you have to go into the tool register screen (under offset) to select light tool which will make the tool changer about 15-20% faster in most cases. Just be sure not to use this setting with any tools that are very long due to the moment of the tool putting a torque load on the fingers or overly heavy tools. The MSX is a great control, very user friendly. I prefer it over our previous control (MSG) because of its increased functionallity and speed. Have you used the 50mb user memory area yet? Do you use CAPS conversational to write any programs? If you create a CAPS program you will see that even the G code produced from there has the M6 on a separate line... that's just how we do it for some reason. Do you have your M6 commanding a sub program or macro to send the machine to G30 position for a tool change? In that case, M6 has to be on its own line because you will get a macro error if there is anything on that line. I'll look into it a little further to see if i can clear up your problem. We have an NV4000 in our showroom that i can check out.

[pieface]

The M6 sub is how the machine arrived, I have only tweaked it due to the above issue. It does include the XY moves etc. I think it is sub no 9020 if memory serves (I'm on holiday over Christmas so can't check at the minute). If the M6T* are in the correct order in the main program, it sucks the T value into the sub, if they are in the wrong order, it does not 'see' the T value and sucks a blank value into the sub and just performs a plain tool swap between spindle and preselect. When running in full auto it is not noticeable, as the tool in preselect position will be correct. (We use next tool preselect directly after previous tool change in main prog). The issue only arises if the program is interrupted and the preselected and/or spindle tools are manually changed away from program sequence.
We have had no problem with the tool change sequence since then (About 4 months trouble free now). I'm not sure what the 50mb user memory is? I haven't used Caps as the machines were bought to produce one product only, so I only created one set of programs which I butchered from our existing Hitachi Seiki's (The 2 NH4000's were a capacity increase to existing product). I have had a play, but produced nothing in anger. I'll definitely have a look at the light/heavy settings when I get back. I thought it was quick as it is, if it can tool change even quicker, that could make a hefty cycle reduction as we are using around 30 tools per load.

[the thrill]

the reason it doesnt see the T if it is after the M6 is because the machine reads the lines of code from left to right. if there is a sub/macro M code call used, it will jump into the sub before reading the T code. The only way around that would be to eliminate the 9020 program and change the Fanuc parameter #6050(???) from 6 to 0 to clear it out so it doesnt jump into anything but then you will have to hard code zero returns before every tool change. in either case, its not a hard fix but it still changes the syntax you are used to on the Hitachi's. The 50mb area is used for program storage, operation and subprogram calling. Press the setting key, type 5 and hit input it will being you into the setting page where you can change the "tape mode" from RS-232 to "MAPPS DNC". Once you do that, press the tape button and you can go into the 50mb area program list. You can go into BG edit and edit any of the programs in that area and run them as if you would a regular NC program but you would run it through tape mode instead of memory. The only snag is that you cannot use any type of macro statement with the 50mb area such as variables or GOTO statements. Will there ever be a time where you will use this machine for more than just one part?

[pieface]

We may use it for other parts in time, but we do use quite a lot of macro programming due to the fact that we have multi part fixturing on cheap crap fixtures where we need to use individual datums for each part station.
I think I have led you astray with the M6 thing. The Mori works perfectly OK as long as the T* FOLLOWS the M6. It only fails to see the T* if it precedes the M6. This is exactly the same on our Hitachi's, except they automatically alarm out if they see T* and M6 in the same block in the wrong sequence. The Mori does NOT alarm if they are the wrong way round, it just ignores the T* completely. What I have done is created the same condition as with the Hitachi's, and added a line to the M6 macro sub to generate a user defined alarm if the values are input in the wrong order or if there is no T* specified at all. This means that either in program OR MDI the ONLY means of toolchanging is by inputting M6T* in that order only. It will not accept M6 on it's own any more. For experienced guys, that could be a minor nuisance, but bearing in mind the generally poor skill level we employ, I have to err on the safe side all the time.
Thanks again for the info, you've supplied quite a bit of food for thought.
PS. Sound's like a silly question, but I'm getting fed up in the UK and considering a shift abroad somewhere. Do you have any idea what the going rate is for skilled CNC guys in the States? I know that's a bit vague from state to state but a general idea would help. Manufacturing Engineer type role I suppose. Cheers.

[the thrill]

Oh, OK. I must have gotten mixed up. As far as the pay rate goes, it varies from state to state due to cost of living. In New Jersey the cost of living is very high and most of the time the only way to live here is to have a very good paying job. However, if you go to a state like Georgia, the cost of living is relatively low so despite the lower pay, you can live a better lifestyle down there than a comparable salary here in New Jersey. For example, I bought a small house for the same price that a VERY large house with 4 times the property would cost down south. The rate of pay is also varied greatly by the company you are working for. Some manufacturing engineers will make $45,000 a year while others will make $85,000 a year... hope this helps!

[pieface]

Give's me a rough idea, bearing in mind the scope over there compared to UK. I like the way you folks live, but you do have serious weather. Our weather is more of a talking point than a major issue. I digress, not much to do with CNC stuff. Thanks again for all the advice and info, if there's anything you need on Hitachi/Cincinatti style stuff, you know where I am. Nice talking to ya.
Happy New Year.