Mori Seiki NT6000 Question

[gcode]

I'm working up a post for this machine
Kudos to Postability. They are nailing it as usual

The spindle is a Capto C8 and I've got a Sandvik CNMG turning tool oriented horizontally
At M03 it's turning OD's
I can spin it 180° run M04 and turn ID's
The machine was built in 2008, but it's been sitting for years and had 200 hours on it when we bought it.
It's in beautiful shape and so far has been deadly accurate

The problem I'm having is this
We'll touch the tool on as an OD tool with the presetter and it will cut within tenths of programmed diameters
but
If I spin it 180°, the ID's come out .020" undersized.
I'm thinking it should be closer than that and that someone tweaked a parameter years ago
Does anyone know if there is a parameter to adjust this behavior?
The instruction manuals are combo Japanese/English and nearly useless.
I'd like to avoid using separate tool work offsets as it's just one more place for an operator to make a mistake

[crazy^millman]

I'm working up a post for this machine
Kudos to Postability. They are nailing it as usual

The spindle is a Capto C8 and I've got a Sandvik CNMG turning tool oriented horizontally
At M03 it's turning OD's
I can spin it 180° run M04 and turn ID's
The machine was built in 2008, but it's been sitting for years and had 200 hours on it when we bought it.
It's in beautiful shape and so far has been deadly accurate

The problem I'm having is this
We'll touch the tool on as an OD tool with the presetter and it will cut within tenths of programmed diameters
but
If I spin it 180°, the ID's come out .020" undersized.
I'm thinking it should be closer than that and that someone tweaked a parameter years ago
Does anyone know if there is a parameter to adjust this behavior?
The instruction manuals are combo Japanese/English and nearly useless.
I'd like to avoid using separate work offsets as it's just one more place for an operator to make a mistake

Where using different Tool Offsets should be used to avoid this issue. Yes it is a parameter so where that is controlling this, but what I have done to get around using different work offsets is use different tool offsets.

[gcode]

I mispoke, I meant tool offsets

[CNCAppsJames]

If I could not ascertain the parameter(s) involved, I would make a G/M-Code to activate for ID and OD which would in turn add the necessary value to the desired offset(s).

Obviously getting the parameter right is the primo solution but a custom G/M code can do other things for you should the need to customize something arise.

JM2CFWIW 

 

[TSmcam]

Just use double/triple whatever offsets, as others have suggested.

At my last employer, we had a Mori Seiki NT4250, a MT253, and two MT4000's. We had similar issues, and yes there was a parameter that could be changed but ultimately, there was always variation.

If for whatever reason you need to use a tool at a non-nominal angle, you'd have to use a secondary offset anyway.

On the U3000 it does auto calculate the different offsets from a "master setting"" but we use differing wear comp to adjust out any discrepancies.

[JParis]

On our Integrexs, when indexing a tool in the spindle, we use a different offset...

In one position it may be H7 D7 and on the next index position it's H7.1 D7.1.....

[gcode]

We've got a 50 tool magazine and 100 offsets so using a 2nd offset isn't a problem.
I wanted to run with one offset because that's one less thing for an operator to screw up
I've thought about it some more and decided there is nothing wrong.
The Capto C8 adapter and turning tool are 8" long and the pivot distance is 254.749mm [10.0299"]
That's a gage length of 18" so even a tiny misalignment of the B axis can cause an error.
To get a .02" diametral difference between OD and ID with the same tool, I calculate the B axis to be
out of square by .0318°

[TSmcam]

So thinking out loud and in noooo way trying to wag your tail....if you use a separate offset but want to minimise screwup....perhaps add a forced toolchange at the index (2nd offset). With comments stating second offset etc.
Then when operator runs through with optional stop active.....he should see the comments before hitting the go button?

Obviously setup sheet with number highlighted in red would also help etc....

We did exactly that at the last place I worked at. When switching to a second offset, there was a M0 with an operator comment, clearly stating the warning that there was an offset change. We really only did it for one operator, who for want of a better term, was a total knuckledragger. He was responsible for several damaged tools, workpieces, and machines...

[crazy^millman]

Sorry slow coming back to this one, but all the points above give you every reason why you want to do what I suggested to being with. I realize you are trying to help the Walmart Greeter that got hired to run the machine, but he is about as good as most places are getting now a days. 63 different companies have reached out to me for someone to go to work for them. Sad state of affairs in Manufacturing.

[YoDoug]

The Capto C8 adapter and turning tool are 8" long and the pivot distance is 254.749mm [10.0299"]
That's a gage length of 18" so even a tiny misalignment of the B axis can cause an error.
To get a .02" diametral difference between OD and ID with the same tool, I calculate the B axis to be
out of square by .0318°

Not only angle, but also the X/Z difference between the B pivot point and the C8 center. I have not worked on an NT, but I have done alignment and comps in a Multus. There is a very extensive set of checks and comps to get it all aligned. Even if you get it all within factory spec it won't be perfect. Using separate offsets is your best bet. However I would still check the alignment. If your B is really off by .0318 deg you will have issues at odd angles and possibly poor drill performance. 

[gcode]

Not only angle, but also the X/Z difference between the B pivot point and the C8 center. I have not worked on an NT, but I have done alignment and comps in a Multus. There is a very extensive set of checks and comps to get it all aligned. Even if you get it all within factory spec it won't be perfect. Using separate offsets is your best bet. However I would still check the alignment. If your B is really off by .0318 deg you will have issues at odd angles and possibly poor drill performance. 

I was thinking the same thing.
The machine is currently down due to overzealous safety protocols ( the damn door won't open, but the machine thinks
it's open and won't run)
We have a service call set up. I'll ask them to check it while they are here