What's new
What's new

lathe thermal growth mitagation solutions?

One thing, as mentioned before, we run a warm-up cycle in the morning, or when the machine is idling for a long time.

The best way we have found, is to also get the all the axes moving, not just warm up the spindles. So for example I will travel almost the full range of Z back and forth, and then go to around the middle of the machine (G53 Z-320) and do some XY movements, we do them in the middle just to make sure we do not hit anything because the tools change all the time... The nice thing is that you can write a relatively short program, and use the memory restart function to loop it for as long as you need. We also load and run this if the machine is idling for a prolonged time, just to keep it warm and moving.

Well still, that is a big deviation, I am really surprised. I also have one and it is sub 10 micron machine all day long. Which I consider really good given that this is the "cheap" Nak.

We regularly do some bronze bushings on it which have an +0.0005 to + 0.0010 inch OD tolerance, and after a proper warm-up we adjust the X offset just about 3-4 microns during the whole shift.
And at that point it somewhat hard to tell for me if this is thermal drift, or insert wear, since the inserts practically last the whole batch of 1000 pcs. We rarely change them, usually only if we cannot get the required Ra 0,8 surface roughness requirement.

Correct on the AS200 there is only one option for thermal compensation in the NT Nurse setting 32, which works based on coolant temperature. Still your mileage may vary according to the workload, we have this turned off, seems more stable that way.

On the higher-end Nak's with 30-series Fanuc, you can get the NT Thermo Navigator AI, but on the WT or MX it has not really been a be all end all solution to all of our problems at all times.
First, you really need to feed the system with a lot of data, if you don't, the compensation will be off. This means a lot of measuring and data input.
Second, since we do usually only do high-mix low volume, some parts are running just a couple of hours at a time, which is not a big enough sample size, to get the compensation working reliably, or I should rather say as good as on the parts where we have run over extended periods of time.

A third option, on the higher end Nak's you can also get scales, but I have never seen them anywhere in the wild, the machines seem to run well out of the box even without them. At around 16k for scales on XYZ, it might be an option for someone.
I also think you can order them just for the X axis for example at a reasonable price. However the difference between scales and no scales seems to be around the one micron mark, and I do not see a point in that for our workload.

One question regarding your AS200, what size is your coolant tank? I have noticed that for some reason, Methods delivers these with a "standard" coolant tank, which is quite small.
Over here, you can get one with an extended Coolant tank which is over 600l, and it has done wonders for thermal stability, compared to other small lathes we run with smaller tanks.
We have considered a high pressure system with coolant chiller for the AS200, but as it costs around quarter of the total machine cost, we have decided to stick with the standard Brinkmann 25bar pumps without coolant chiller for this machine, and it works really good as long as you have the extended coolant tank.
 
Took a quick look at a photo of a similar nak - seems like a normal layout. You mean you cannot just say

n20 go to some x and z location
n30 change to tool 6 offset 6
n40 come back to the part and cut metal

??

Of course you can.

For some reason that I still don't understand in spite of several discussions about it in the past, Ox wants to use T0000 which is not the normal method of acheiving this, and only works on some machines.
 
Not normal for who? It works on every other machine and control brand machine that I have here, other than the Naks. There is a lot more than the T0 issue. But as I just pointed out above - this is a perfectly good example of why you would want to use it.

The Nak doesn't want to let you dump the offset, so to rapid out to a safe zone in Z [without going all the way to end of travel and possibly crash on tailstock, sub-spindle, or other turret] you would need to consider the Z offset for each tool, and verify that again at each set-up.

In my app - that I would doo in the case of our guy here that wants to keep X travel down, on any of my other lathes, I could dump the offset w/o worry of accidentally calling a turret index at the same time (for absolutely no reason) and move to a safe zone.

In my example above (I think) I could call G0 T0 Z14. and as long as all of my tools are shorter than 14" and "Z14." clears my sub-spindle (location hinges on part length and G10 P0 Z_ value) then that is my safe zone, and anywhere in the program I can make that call, and it can run over there and change a tool w/o worry of crashing, or inducing heat into my X screw.

But this works for more than just a cool screw. If I am dooing a few on-center tools back-to-back, than I can:

G1 Z-1.4 F5. M8
G0 T0 Z14. M9

Nx T606 (next tool)
G97 G98 G20
M3 S1000
G0 X0 Z.1 M8
Z-1.3
G1 Z-1.89 F6.
G0 T0 Z14. M9

Not being able to simply dump the offset either means that you can't easily doo that, and/or precludes that you put a T600 code in there, which can either be miss-entered, or more likely the next set-up that tool could be in pocket T5, and if you forget to edit the dump code to T500, it's gunna want to index the turret during that move. And for what porpoise?

Actually, on the Nak's, I haven't tested this, but it does seem that the turret may not index until the Z has moved. At least that's how I think that I am seeing it so far as I have a Z move in my toolchange lines, and either the turret is slow to the draw, or it may actually not perform both acts at once. And if that is the case, then the concern over the turret indexing during retract may not be a thing? But I haven't tested that for sure yet.

-----

Like I said - 14 pages of M codes!
The thing is safety lock-out city!
Sometimes with an M code to allow you to pay no nevermind to that issue.

There is another thread currently going here about another brand machine that won't let him perform an act that he wants to doo b/c of a safety regarding collet open and spindle synch. This stuff is NOT a Fanuc thing.

On my Hardinge Twin Turn 65 (WT300 equiv - and same 18i control) I can doo anything that I want to. If I break a tool or skid a collet, it's on me. And that machine has 2 pages of M codes, and the machine will perform anything that I tell it to. It's not gunna tell me that "This is not a Hardinge sanctioned act - bugger off Hoser!"

I have at least 3 other Fanuc and Mits lathes beyond Hardinge that allow me to use T0.
This is NOT an odd application at all. and I see absolutely no reason that this would be diss-allowed?

But - as the fella above touched on, maybe a G53 X_ Z_ call would accomplish the same thing.
I will have to try that sometime. And in the case here where this fella wants to keep his X ballscrew cool, that could very well be the ticket to his app! (Just G53 Z_)


---------------------

I am Ox and I approve this here post!
 
Last edited:
Not normal for who? It works on every other machine and control brand machine that I have here, other than the Naks. There is a lot more than the T0 issue. But as I just pointed out above - there is a perfectly good example of why you would want to use it.

The Nak doesn't want to let you dump the offset, so to rapid out to a safe zone in Z [without going all the way to end of travel and possibly crash on tailstock, sub-spindle, or other turret] you would need to consider the Z offset for each tool, and verify that again at each set-up.

In my app - that I would doo in the case of our guy here that wants to keep X travel down, on any of my other lathes, I could dump the offset w/o worry of accidentally calling a turret index at the same time (for absolutely no reason) and move to a safe zone.

In my example above (I think) I could call G0 T0 Z14. and as long as all of my tools are shorter than 14" and "Z14." clears my sub-spindle (location hinges on part length and G10 P0 Z_ value) then that is my safe zone, and anywhere in the program I can make that call, and it can run over there and change a tool w/o worry of crashing, or inducing heat into my X screw.

But this works for more than just a cool screw. If I am dooing a few on-center tools back-to-back, than I can:

G1 Z-1.4 F5. M8
G0 T0 Z14. M9

Nx T606 (next tool)
G97 G98 G20
M3 S1000
G0 X0 Z.1 M8
Z-1.3
G1 Z-1.89 F6.
G0 T0 Z14. M9

Not being able to simply dump the offset either means that you can't easily doo that, and/or precludes that you put a T600 code in there, which can either be miss-entered, or more likely the next set-up that tool could be in pocket T5, and if you forget to edit the dump code to T500, it's gunna want to index the turret during that move. And for what porpoise?

Actually, on the Nak's, I haven't tested this, but it does seem that the turret may not index until the Z has moved. At least that's how I think that I am seeing it so far as I have a Z move in my toolchange lines, and either the turret is slow to the draw, or it may actually not perform both acts at once. And if that is the case, then the concern over the turret indexing during retract may not be a thing? But I haven't tested that for sure yet.

-----

Like I said - 14 pages of M codes!
The thing is safety lock-out city!
Sometimes with an M code to allow you to pay no nevermind to that issue.

There is another thread currently going here about another brand machine that won't let him perform an act that he wants to doo b/c of a safety regarding collet open and spindle synch. This stuff is NOT a Fanuc thing.

On my Hardinge (WT300 equiv) I can doo anything that I want to. If I break a tool or skid a collet, it's on me. And that machine has 2 pages of M codes...

I have 3 other Fanuc and Mits lathes beyond Hardinge that allow me to use T0.
This is NOT an odd application at all. and I see absolutely no reason that this would be diss-allowed?

But - as the fella above touched on, maybe a G53 X_ Z_ call would accomplish the same thing.
I will have to try that sometime. And in the case here where this fella wants to keep his X ballscrew cool, that could very well be the ticket to his app! (Just G53 Z_)


---------------------

I am Ox and I approve this here post!
We've discussed this at length before, and I just can't wrap my head around why you wouldn't just use G53 or G30...
 
One thing, as mentioned before, we run a warm-up cycle in the morning, or when the machine is idling for a long time.

The best way we have found, is to also get the all the axes moving, not just warm up the spindles. So for example I will travel almost the full range of Z back and forth, and then go to around the middle of the machine (G53 Z-320) and do some XY movements, we do them in the middle just to make sure we do not hit anything because the tools change all the time... The nice thing is that you can write a relatively short program, and use the memory restart function to loop it for as long as you need. We also load and run this if the machine is idling for a prolonged time, just to keep it warm and moving.

Well still, that is a big deviation, I am really surprised. I also have one and it is sub 10 micron machine all day long. Which I consider really good given that this is the "cheap" Nak.

We regularly do some bronze bushings on it which have an +0.0005 to + 0.0010 inch OD tolerance, and after a proper warm-up we adjust the X offset just about 3-4 microns during the whole shift.
And at that point it somewhat hard to tell for me if this is thermal drift, or insert wear, since the inserts practically last the whole batch of 1000 pcs. We rarely change them, usually only if we cannot get the required Ra 0,8 surface roughness requirement.

Correct on the AS200 there is only one option for thermal compensation in the NT Nurse setting 32, which works based on coolant temperature. Still your mileage may vary according to the workload, we have this turned off, seems more stable that way.

On the higher-end Nak's with 30-series Fanuc, you can get the NT Thermo Navigator AI, but on the WT or MX it has not really been a be all end all solution to all of our problems at all times.
First, you really need to feed the system with a lot of data, if you don't, the compensation will be off. This means a lot of measuring and data input.
Second, since we do usually only do high-mix low volume, some parts are running just a couple of hours at a time, which is not a big enough sample size, to get the compensation working reliably, or I should rather say as good as on the parts where we have run over extended periods of time.

A third option, on the higher end Nak's you can also get scales, but I have never seen them anywhere in the wild, the machines seem to run well out of the box even without them. At around 16k for scales on XYZ, it might be an option for someone.
I also think you can order them just for the X axis for example at a reasonable price. However the difference between scales and no scales seems to be around the one micron mark, and I do not see a point in that for our workload.

One question regarding your AS200, what size is your coolant tank? I have noticed that for some reason, Methods delivers these with a "standard" coolant tank, which is quite small.
Over here, you can get one with an extended Coolant tank which is over 600l, and it has done wonders for thermal stability, compared to other small lathes we run with smaller tanks.
We have considered a high pressure system with coolant chiller for the AS200, but as it costs around quarter of the total machine cost, we have decided to stick with the standard Brinkmann 25bar pumps without coolant chiller for this machine, and it works really good as long as you have the extended coolant tank.
I have the “standard” tank with a little sub tank( 30L maybe) connected that houses the optional 300psi pump.
I ran with a smaller pump though ( 30psi 18 gallon 600watt)as i have limited power and a 5hp coolant pump is too much draw.
(I fear Im Outgrowing my home shop :(
The smaller pump was a little lacklustre. A 2hp would be the sweet spot I think.

A larger sump would defiantly help. But my main concern is not total growth, but how quickly is “shrinks” back making things unpredictable.

A 10 micron total deviation would be a dream!

I’ll be running the same job again soon. I will make sure to add x axis movement to my warmup cycle,
Add a temp probe to my coolant tank (but not use thermal comp) and track the shop temp and headstock temps through the day.

I wonder if it’s a more x axis thing as the sub and the main both showed near identical offset requirements?
(Cutting time on job is about even)
I’ll look into avoiding excessive x retracts to avoid screw heat.
(note: I did have the rapids set to 50 % the whole day, I guess that would reduce heat a little bit)
 
  • Like
Reactions: Ox
We've discussed this at length before, and I just can't wrap my head around why you wouldn't just use G53 or G30...

I have not looked into G30 yet. That is not incl on any of my other machine that I know of.
I never thought of the G53 route 'till this fella above mentioned it.

But that doesn't give any excuse to locking out a simple T0 code tho either, just to complicate it with some other additional codes?


----------------------

I am Ox and I approve this here post!
 
Wow, you guys like to make this hard !

Safe zones are for snowflakes :)

None of the lathes I've run would let you do T0000 cuz there is no position 0, but they would all do, if you are for example at tool 6, T0600. That'd be tool 6, offset 0 and it would physically move the tool and dump the offset.

But I guess my problem here is, I can't see why you'd want to dump an offset without changing the tool ? For what purpose ? I can see it at the end of a program so you can put the lathe to sleep with no offset (I know, fanucs work different but in my case when you put the lathe to sleep it lost its mind) but normally ? What for ?

The Cinturn had a nice method for interference avoidance, the way the turret was built for sizes up to the chuck diameter, it was impossible for the tool to crash anything, id tools all in the center, od tools around the edge. But that won't help Stirling ...

I've never done the 'safe zone' thing but am very aware when indexing if there's any long stickout tools ... then single block is your friend.

That's what makes lathes exciting :)
 
Last edited:
Good point.
This lathe does do a lot more x moves than my last one the way it’s programmed now

I’m brand new to fanuc so I’ll need to learn how to change the tool change position.
You run fanuc Nak lathes.
How do you go about this?

I’d assume either changing a parameter or something in each program that alters it temporarily?

My last lathe was all conversational and you’d set it right at the Home Screen for each job.
fer yer chip issue, get some big plastic garbage cans, or scrounge up 55 gal drums, the garbage cans are a lot easier to load by hand... but hold a helluva lot more then a 5 gal bucket, maybe enough to go several days...
 
When I write "safe zone" I am talking a self imposed safe zone for this job today, not one that is embedded into some offset in the control. It's just somewhere that all tools clear. If you have ran a lathe much at all, and changed tools some of the time, I am sure that you moved to a point that your tools cleared the chuck/workpiece before indexing.


-----------------------

I am Ox and I approve this here post!
 
I have not looked into G30 yet. That is not incl on any of my other machine that I know of.
I never thought of the G53 route 'till this fella above mentioned it.

But that doesn't give any excuse to locking out a simple T0 code tho either, just to complicate it with some other additional codes?


----------------------

I am Ox and I approve this here post!
I suggested using G53 at least the last two times we've discussed this!

I prefer using G30 though. It's enabled on every Fanuc I've encountered so far, but it is an option...

AFAIK about T0, it has to be explicitly supported in the ladder. The only Fanuc I've ever used that allowed T0 was the the first one I ever used, and I got used to using it, and it confused me when I got my next one. But I learned to use G28 instead, and later G30.
 
  • Like
Reactions: Ox
When I write "safe zone" I am talking a self imposed safe zone for this job today, not one that is embedded into some offset in the control. It's just somewhere that all tools clear.
I never did that. If the boring bar was 8" long, I'd move the turret 9" (because I am a coward) OR move up in X to clear the chuck but if the internal groove tool only stuck out 3", then I'd move 4". It all depended on the shape of the part. Probably would have been smarter to have a more generalized approach but ocd ?

Of course you had to be aware of which tool was on which side of the turret if you play that game, and you have to have a bi-directional turret you can control the direction on. And you better pay attention when setting up :)

But once running, bob's yer uncle.

Dual turret machines are actually nicer that way, because there is more freedom from potential mistakes, but if the dang thing only has one turret, that's what you're stuck with.
 
……..AFAIK about T0, it has to be explicitly supported in the ladder. The only Fanuc I've ever used that allowed T0 was the the first one I ever used, and I got used to using it, and it confused me when I got my next one…….
Allowing T0 or not is up to the machine builder’s ladder program. Fanuc cares not. In fact the Fanuc side of the control does not know or care if it’s a turret of gang type machine. All that is up to the builder’s ladder as part of the integration of the control to their machine.

If a builder decides the range of tools is 1-12 say, they typically will write their logic so that tool calls outside that range generate an error if decently written or do nothing if not so well done. If the builder understands that some folks like T0, logic for that can be added. It is also possible for a builder to make use of T0 selectable by keep relay. Best of all worlds then. During the years I worked for a Mori distributor, all their lathes had that ability.
 
Last edited:
During the years I worked for a Mori distributor, all their lathes had that ability.
I'm still puzzled tho - what good is it ? What is the point of dropping an offset unless you are changing a tool ?

Or on the rare occasion you might want to for some reason, what's difficult about calling the tool that has that offset, with a "clear offset" command?

I'm a RISC kinda guy, 4,000 special commands don't ring my buzzer ....
 
I suggested using G53 at least the last two times we've discussed this!

I prefer using G30 though. It's enabled on every Fanuc I've encountered so far, but it is an option...

AFAIK about T0, it has to be explicitly supported in the ladder. The only Fanuc I've ever used that allowed T0 was the the first one I ever used, and I got used to using it, and it confused me when I got my next one. But I learned to use G28 instead, and later G30.


I have been using G28 U0 on the Nak, and that is fine for X - no worries.
But it is not a good app for Z.
On my other machines, well ... mostly on the single turret machines I guess... I like to run my turret clear in Z on my retract move as well. And with G28, this ends up being 2 separate lines of code and takes 2wiced as long.

What I have been dooing is G28 home in X, and then call a G0 Z0 move on my turret index line, so that the tool is pre-positioned so that it is not behind Z0 before it's move in X. This is mostly just an issue with on-center tools that could clip the chuck or maybe a large OD on the way to X0 Z.1 staging position. It's also an issue for the cut-off tool as that can easily be behind the chuck. But I have been puting it on every tool change line for safety's sake - in case of mid program start from unknown position.

I will need to pull up the G30 sometime and look at that.
When you mentioned that the first time, I looked through my Hardinge G code list and it was not there.

Maybe you did mention the G53 before. IDK. But this is the first time that I thought about how it could work.
I use that on the mill, but never tried it on a lathe, but it should work the same.


-------------------------

Think Snow Eh!
Ox
 
I'm still puzzled tho - what good is it ? What is the point of dropping an offset unless you are changing a tool ? ....
IMHO, it’s just a personal preference thing. Obviously, Ox likes it as it conforms to how he has learned to program other machines. I learned on machines that one called T0x00 so that’s what I do. I do kind like that if one can use T0 and you need to rearrange the tools on the turret you have fewer edits to do if hand coding is your method.
 
I'm still puzzled tho - what good is it ? What is the point of dropping an offset unless you are changing a tool ?

Or on the rare occasion you might want to for some reason, what's difficult about calling the tool that has that offset, with a "clear offset" command?

I'm a RISC kinda guy, 4,000 special commands don't ring my buzzer ....


I have went to length of describing "the point".
And you are talking Acramatic language on a Fanuc thread.
And if you would otherwise call a "Clear Offset" command, then you already know why you would want to doo so.


---------------------

I am Ox and I approve this here post!
 
I have been using G28 U0 on the Nak, and that is fine for X - no worries.
But it is not a good app for Z.
On my other machines, well ... mostly on the single turret machines I guess... I like to run my turret clear in Z on my retract move as well. And with G28, this ends up being 2 separate lines of code and takes 2wiced as long.

What I have been dooing is G28 home in X, and then call a G0 Z0 move on my turret index line, so that the tool is pre-positioned so that it is not behind Z0 before it's move in X. This is mostly just an issue with on-center tools that could clip the chuck or maybe a large OD on the way to X0 Z.1 staging position. It's also an issue for the cut-off tool as that can easily be behind the chuck. But I have been puting it on every tool change line for safety's sake - in case of mid program start from unknown position.

I will need to pull up the G30 sometime and look at that.
When you mentioned that the first time, I looked through my Hardinge G code list and it was not there.

Maybe you did mention the G53 before. IDK. But this is the first time that I thought about how it could work.
I use that on the mill, but never tried it on a lathe, but it should work the same.


-------------------------

Think Snow Eh!
Ox
G53 is the best solution if you don't have the G30 option. But G30 is great in that works exactly like G28 but allows you to set 4 different home positions. These home positions are set by parameter, but you can use G50 L10 to set these parameters at the start of your program if you know its always going on the same machine.
 
fer yer chip issue, get some big plastic garbage cans, or scrounge up 55 gal drums, the garbage cans are a lot easier to load by hand... but hold a helluva lot more then a 5 gal bucket, maybe enough to go several days...
Only issue would be lifting them after no?
if I cannot lift by hand it’s a no go for me. No lifting equipment.

Very open to options there if there is something I’m missing

Currently I use x20 5 gal buckets.
For bigger jobs I’ll get a liquid tote (cubic meter) and leave that in the truck and toss the chips by the bucket load in as I go.

Downside of a garage shop.

I love the “work from home” thing, but it defiantly has its drawbacks. (Space, amps, distractions)
 
G53 is the best solution if you don't have the G30 option. But G30 is great in that works exactly like G28 but allows you to set 4 different home positions. These home positions are set by parameter, but you can use G50 L10 to set these parameters at the start of your program if you know its always going on the same machine.

OK, so I have seen that, but I was thinking that was another M code, but either way, I think that I did mention to this fella in my first post that there is a staging location option on the Nak's, but I haven't spent time looking into those yet as what I am dooing currently is working fine for now.

And loading a parameter adjust in the header is certainly no problem at all.
And again - this may very well be a perfectly good option for this fella to set that up as a Z home location.


----------------------

Think Snow Eh!
Ox
 








 
Back
Top