What's new
What's new

Method of positioning lathe turret for tool changes

cuttergrinder

Hot Rolled
Joined
Mar 16, 2007
Location
Salem,Ohio
how do most guys position a lathe turret with fanuc for a tool change on a long lathe. Our recently purchased lathe has about 12' of z travel. I realize you can use G28 but that will send it all the way home. If I am working on a part in the chuck say 8" long what should I use to position the turret for tool changes. Ive read you can use a G53 with an X and Z value but why is this better than just using a G00. I realize the G53 is in relation to the machine coordinates and the G00 will be in relation to the part coordinates but I would think you would want to index the turret in relation to the part rather than the machine coordinates. I realize this is probably a dumb question but I am used to mazatrol. It always positions the turret for a tool change according the longest tool automatically.
 
safe bet
6 inch chucks x6.0 z6.0
8 inch chucks x8.0 z8.0
10 inch chucks x10.0 z10.0
from Z0.0 which is front of part in most cases

oh did you say you had 12' ie 12 feet or did you mean 12" inchs.
if its 12 inchs of travel you obviously cant move the z back to far thats why you always move the x at chuck dia or higher for clearance
 
G00 still maintains the tool offset as part of it's criteria during movement. At least it likely would at the end of the tools work and heading for the next tool. G53 has no relation other then to the machine itself. That Mazak functionality sounds great. You could mimic that in your program by positioning the longest tool at a safe position for turret rotation, and use the numbers you see in the Machine Coordinate display as your tool change position for that job. With all that travel and if no tail stock to worry about, you could even do both X and Z moves in one line simultaneously, (G53X-4.Z-110.) which is not something you always want to do on tight envelope machines.

There is a certain amount of impracticality to this idea, as you would need to set up the machine and measure the longest tool before you could learn the info to enter before every tool change in your program. One way you could get around that is to have a small subroutine resident on your lathe that you call as a matter of course before every tool change in your programs. You might even be able to set up your post processor to do this for you. Then all you do is change the G53 call in your control resident Tool Change Position Subroutine to the current jobs needs. Just one idea. There are likely other ways to do this. I just made this up while sitting here typing, and I don't have a long history with CNC lathes.

I will say that after working in a tight envelope lathe were every move is practically a blonde one away from a crash, hearing about your 12 feet of travel makes me a good bit jealous. Talk about breathing room!
 
Yes the rookie fanuc programmer has to learn on a 12' long lathe. I know its kind of scarey. I have run large manual lathes up to 22' long and a shorter cnc lathe but it a mazak with mazatrol.
 
Yes the rookie fanuc programmer has to learn on a 12' long lathe. I know its kind of scarey. I have run large manual lathes up to 22' long and a shorter cnc lathe but it a mazak with mazatrol.

sweet miss those big cncs. used to run them all the time but we didnt have tool changers just huge tool posts.
just back off a couple of inches past the front of part in Z .
 
How you position your turret greatly depends on if your program is for high production or low production. On repeat high production jobs I rapid the turret just enough so the next tool is 1/2 away from the front of the part. Sometimes less.

If low production set a G53 so turret can index in any position and be at least 1 Inch or more away from the part. Keep in mind if you would do this on a high production environment you would get your ass reamed very quickly. Seconds count.
 
This is how I program my 0TC for tool change/home position:


T0_00 (cancels offset for whatever tool was used)
G0 X11.527 Z5. (the X value is what my machine homes to from X zero being center of rotation of spindle) The Z is enough off the part so that no tool will hit the work or chuck when indexing.
 
There are a few ways to do this.
When I was teaching the classes I used to tell the students that on large lathes, those with 36" or more of Z travel, to set a secondary home, via G30 that was somewhere in the middle of the travel. This gave you clearance for boring bars, drills and other big stuff.
On lathes that are more standard sized, you can back up the same as chuck dia and guarantee clearance, most of the time. A lot of this is just good judgement on your part.
The G30 is set via parameter 1241 on most Fanuc controls.
 
The jobs on this lathe will definitely be low production just because they will be so big. I think the lathe will turn about 32" dia. and 12' long.
 

Attachments

  • 20191221_130029.jpg
    20191221_130029.jpg
    94.4 KB · Views: 100
  • 20191223_084644.jpg
    20191223_084644.jpg
    92.8 KB · Views: 102
Depends but I don’t like the idea of always going to XZ home. Never done it that way myself. For low volume stuff I will do X8. Z8. if I’m switching from a stick tool to an ID tool (more if for some crazy reason the ID tool is that long but it usually never is). From one ID tool to another I might do Z4. since they’re generally within a couple inches on length.

Got to be careful if you’re using a tailstock, usually it’s best to retract X first then Z to keep from hitting the tailstock.
 
On a large machine like that, I would avoid G53 and set a G30 2nd home. Then make sure you G30 U0, G30 W0 on separate lines so the turret clears the steady rest and tail stock.
 
Correct me if I am wrong but I assume the G30 U0 and the G30 W0 are incremental moves to move the turret how ever far it needs to go to get to the second home position. The incremental move will happen even if you are working with absolute programming.
 
How do I set the second home position? It may already have one set, I just don't know how or where to see what it is set at.

Parameters 1240,1241,and 1242 are the second, third, and fourth home position settings. Just move the carriage to your desired tool change/home position and record the location and input in the parameters.
 
Correct me if I am wrong but I assume the G30 U0 and the G30 W0 are incremental moves to move the turret how ever far it needs to go to get to the second home position. The incremental move will happen even if you are working with absolute programming.
Hello cuttergrinder,
Unless your control is set to other than G Code System A (via parameter), there is no Absolute/Incremental mode per se. G Code System B and C use G90/G91 to select Absolute/Incremental Modes respectively, with each remaining Modal until replaced by the other. G Code System A use U/W and are the Incremental components of the Absolute X/Z.

Like G28, G30 is a two shot function that returns the axes to a Reference Return position via an intermediate point. When the command is issued with Incremental moves, the specified axes will move incrementally the distance and direction specified in the G30 Command Block, before moving to the Second Reference Return position. Accordingly, when U0.0 W0.0 is specified, the axes move no distance before moving to the Second Reference Return position. You can observe the two shot characteristic of G28 and G30 by executing the command in Single Block Mode. It takes two presses of the Cycle Start button to execute either the G28, or G30 Command Block.

The Reference Return position for G30 must be set via parameter and is an incremental distance from the Machine Reference Return position (G28). Accordingly, its the Machine Coordinate Position that is used when setting the Second Reference Return position. As G53 is also specified with a value that is a distance from the Machine Reference Return position (Machine Coordinate Position), its more convenient to use G53 than G30, as G53 can be specified directly, whereas the G30 position has to be specified in parameters and these parameters have to be edited each time you need to change the Second Reference Return position.

Regards,

Bill
 
On a large machine like that, I would avoid G53 and set a G30 2nd home. Then make sure you G30 U0, G30 W0 on separate lines so the turret clears the steady rest and tail stock.

And why would that be? Both use the Machine Coordinate System. If the Z G30 position was set 1000mm from the Z Reference position, -1000000 (-1000.000) would have to be set in parameters. If G53 is used, Z-1000.0 would be specified as in the following Block:

G53 Z-1000.0

Its far more convenient changing the Tool Change position by specifying a Machine Coordinate System position with G53 than having to change the parameter setting for G30.

Regards,

Bill
 
I wonder why Fanuc does not have a way to automatically adjust the tool change position according to the part length and the length of the longest tool like Mazak does. On the Mazak, it will change the tool change position if either the Z offset of the part or the length of the longest tool is changed. I realize this makes the Mazatrol programmer ignorant as to how to program this manually but I feel it sure is a lot easier to run the machine this way.
 








 
Back
Top