Index position on cnc lathe

Andrew65 · Mar 27, 2019

Hi all,
I am getting back into setting up cnc lathes after being off them for a long time.
can anyone tell me how to set index position closer to chuck without having to go back to
machine zero on every index?
I am aware of tool clearance possible issues getting closer to chuck.
is there a simple method?
any help would be great
thank you

Hazzert · Mar 27, 2019

Lets start with what kind of lathe you're running.

Are you talking about the Fanuc G28 U0.W0. ?

Have you tried adjusting those numbers?

Does this answer your question?
https://www.cncci.com/resources/tips/how g28 works.htm

Fancuku · Mar 27, 2019

Andrew65 said:
is there a simple method?

Do it in the program. Replace the block that tells the turret to go to home position with for example G00 X5.0 Z5.0 (assuming there is enough clearance for the turret to index without a tool hitting the chuck/workpiece).

litlerob1 · Mar 27, 2019

It shouldn't make any difference on a Fanuc. OTOH if it's an Okuma, you need to be against the switches. (Which is brilliant).

Why, oh why would you want to Index in an un-safe spot? Just Index, then jog, the Index, then jog. Tools caught on Chuck is bullshit and really embarrassing, when you need to tell someone. Not that I have ever done it.

R

Spruewell · Mar 27, 2019

Depends on the machine and it’s control. Some older machines require each tool to be indexed at the home position. Others do not. What are you running?

SeymourDumore · Mar 27, 2019

I for one never send SOME of my machines to home, in fact on the NL-SY I can't even do it period!

Anyway, for indexing I just code:
G00 G53 Xnn Ynn
TXXX

Where nn is a known safe position in the machine coordinate system to rotate the turret at.

litlerob1 · Mar 27, 2019

SeymourDumore said:
Where nn is a known safe position in the machine coordinate system to rotate the turret at.

If it a "known safe position" that's great. But if a guy is just randomly Indexing the Turret wherever, it's going to end up bad eventually.

R

Vancbiker · Mar 27, 2019

litlerob1 said:
If it a "known safe position" that's great. But if a guy is just randomly Indexing the Turret wherever, it's going to end up bad eventually.

When I did field service we typically trained folks to pick a known safe position to index rather than machine zero. One customer, (tier 1 automotive supplier) wanted to eke out every scrap of cycle time so they wanted to index with the next tool just a 1/2" away from the part when going from short tool to long. Actually never really caused any problem. I do not recall ever going there to fix a crash caused by indexing close in. The nature of that type work though. High volume, low mix. ~900 parts per shift. Same old, same old, day in and day out. Offset changes not allowed unless feature measurement was using 80% of tolerance. Any kind of hiccup and the operator had to get a supervisor to deal with it. Figure out how to save a couple seconds on the cycle time and you were a hero to the department head.

litlerob1 · Mar 27, 2019

I've done similar stuff, in the program.

Not during set-up. But WTF do I know.

R

SeymourDumore · Mar 27, 2019

litlerob1 said:
If it a "known safe position" that's great. But if a guy is just randomly Indexing the Turret wherever, it's going to end up bad eventually.

R

Rob, You're correct that the guys should not just randomly index the turret wherever.

But to the OP:

can anyone tell me how to set index position closer to chuck without having to go back to
machine zero on every index?

You can initially do so by writing each and every program with a toolchange as:
G00 G53 X0 Z0
Txxx

Then, during setup, the guy can move the turret to a position at which ALL tools are clear away from the part, and read the machine X and Y coordinates ( absolute mach. coords!!! )
Then he can do a change of all values on each of those lines to the read coordinates.

Sooner or later you will find a reasonably safe, common place to index your turret based on the machine's size and envelope and hard code it into your post.

OTOH If/when you have a long and high qty run, just change the same values individually for each tool.
Just as Vanc said, it can be puckerfactor close.
With inserted tooling that never change in length or position, you might as well index the freakin' thing .05 away from the part!
Guaranteed .05 might as well be a mile right?

( No joke, you can actually use a toolchange to knock off birdsnests from the part! )

Delw · Mar 28, 2019

why not just program it into the bottom of every tool

for example been doing this for 25+ years I have found
G00G97X6.0Z6.0
G00T0100
M01
for most 6 and 8" chuck machines. if your using long tools then change the Z to 8" or 10 or what ever.

my Miyanos with twin turrets I use 4" on the Z.
In the morning turn power on take machine home, jog off home switchs hit button and run parts
on the z axis I could go shorter but WHY risk it.

Spruewell · Mar 28, 2019

I’m running Miyanos with Fanuc controls and they will allow tool indexing anywhere without requiring the machine to run to the “home” position. I always end every tool path with an M1 so that during setup I can check clearance before the next tool indexes. I also try to make all my tool lengths to match whenever possible. Especially on the “Z” tooling where I can have two tools on one station.
My old Nakamura however, did require you to return the turret to the home position to index tools and cal offsets.

Andrew65 · Mar 28, 2019

I believe the place I used to work at put the same numbers at the end of each cycle.
X11. Z11. I think they used.
Question: If each cycle used same X11. Z11. numbers and say you were using a long insert drill as well as stick tools then the turret would rapid back to a different position when going to index. is that right?
if this is correct,
how does the machine know its location when it indexes to next tool?

Fancuku · Mar 28, 2019

Andrew65 said:
I believe the place I used to work at put the same numbers at the end of each cycle.
X11. Z11. I think they used.

That sounds like numbers that were spit out by the programming of the machine controller on older machines.
We have that at my job.
I changed them all to the home position. No silly numbers in my programs

Unless you run high volume low cost parts where seconds matter, no one should index anywhere else but the home position. :scratchchin:

Vancbiker · Mar 28, 2019

Fancuku said:
......Unless you run high volume low cost parts where seconds matter, no one should index anywhere else but the home position.

So a user with a lathe with a long Z travel should always go to the home position to index when doing chucker work? Better would be to just learn how to use the control and program to use a safe index point.

SeymourDumore · Mar 28, 2019

Fancuku said:
Unless you run high volume low cost parts where seconds matter, no one should index anywhere else but the home position.

It ain't about the seconds, but why on Earth would I send the turret home when 99% of the time I can index at X-8./Z-8. from it?

And again, I challenge you to send most subspindle Y axis machines home when fully tooled up!

Andrew65 · Mar 29, 2019

if you put X6. Z6. or whatever numbers work for clearance in program and say the cycle finishes and machine goes to those X6. Z6. numbers ,then machine indexes to next tool,how does machine know where it is for next tool without being at machine zero?
thats my concern.

Hazzert · Mar 29, 2019

Andrew65 said:
if you put X6. Z6. or whatever numbers work for clearance in program and say the cycle finishes and machine goes to those X6. Z6. numbers ,then machine indexes to next tool,how does machine know where it is for next tool without being at machine zero?
thats my concern.

This isn't some janky homemade 3d printer. The machine always knows it's absolute position from home unless it hits the limits and needs to be re-reference returned.

litlerob1 · Mar 29, 2019

Andrew65 said:
if you put X6. Z6. or whatever numbers work for clearance in program and say the cycle finishes and machine goes to those X6. Z6. numbers ,then machine indexes to next tool,how does machine know where it is for next tool without being at machine zero?
thats my concern.

Fuckin' magic dude. First you need a chicken, and some candles. Some Human skulls and some incense (not incensed BTW). After you light the candles and arrange the skulls in 5 points about a Circle---you say woooo, woooo, woooo, weee, weee, weee I (insert foreign language insult here) booo, booo, booo, smeee, smeee, smeee. You have to do that 42 times in a row. Then you kill the chicken by about º350 in the oven, and eat it. (potatoes optional)

After all that the Machine will know where it is, all the time.

R

You can also try; Zim Zala Bim Bombozala Dozala Dim---but I think their server is down, at least temporarily. I keep trying to use it on my wife, and she's still fat and ugly.

angelw · Mar 30, 2019

I'm with Seymour with regards to using G53. Even if the tools used from job to job are not changed, the coordinates used may have to be varied because of the different length of the work-piece, as the G53 coordinates are referenced from the Zero of the Machine Coordinate system, not the Work Zero.

Hazzert said:
Lets start with what kind of lathe you're running.

Are you talking about the Fanuc G28 U0.W0. ?

Have you tried adjusting those numbers?

Adjusting/varying these numbers will have Zero effect on where the X/Z axes finish at. It will be the Machine Reference Point irrespective of the values use in U and W (or X and Z).

It's also common to just move the X axis to the Reference Return position for a safe tool change and always go to the Z coordinate with the next tool as the first move. For example (mm Mode example):

G00 Z10.0
G28 U0.0 M09
M01
(NEXT TOOL)
G28 U0.0
G50 T0200 S4000
G97 S2652 M03
G00 Z10.0 T0202 M08
X30.0
G96 S250
--------
--------
--------
--------
G00 Z10.0
G28 U0.0 M09
M01
(NEXT TOOL)

Regards,

Bill

Index position on cnc lathe

Plastic

Stainless

Cast Iron

Diamond

Hot Rolled

Diamond

Diamond

Diamond

Diamond

Diamond

Stainless

Hot Rolled

Plastic

Cast Iron

Diamond

Diamond

Plastic

Stainless

Diamond

Diamond

Similar threads