Lathe offset change without tool change? Is this possible?

[mmurray70]

Hey guys wondering if its possible to call a new tool offset without doing a toolchange on a lathe?

Trying to figure out best practice for toolchange position on a haas lathe. Im used to Mazak lathes figuring this out for me automatically. Just watched a video on how using a g53 position can work better then homing the machine with G28. But if you decide you need to make an adjustment to toolchange position you need to edit program in bunch of places. seems like a mess.

Was thinking I could just use a work offset to go to a safe toolchange position? Be very easy to adjust toolchange position on the fly then. Say g59 for example. This will also read tool offset, so would need to call some unused tool offset first. Something like this:

G28 G0 U0. (home X)
Call some unused tool offset without toolchange
G0 G59 Z0. (move to G59 position)
G54
M6 T0202 (toolchange in safe position)

How can I do this? Any other suggestions?

 

[atex57]

I do a lot of deep but not wide grooving using a 3mm wide tool. I use T0707 to offset for the front edge and T0717 to set the back edge of the insert. If I have retracted X to clear the part using T0717 to start the groove I just call T0707 and it simply moves over 3mm to start working toward the finish side.

Try it in MDI to get the hang of it.

On edit: This is on an old Fanuc 3T, may work on a Haas.

Ed.

 

[Nmbmxer]

We used to use 3 offsets when turning some long small diameter shafts. You'd start with the normal offset, then on the finish OD pass call the second offset with a Z halfway down the shaft, then the next line called the third offset with the final Z dim. Then you could change the second and third offset values to get all the taper out on a 1/2" OD part that is nearly a foot long using a clapped out lathe that didn't have a hyd steady. The extra offsets are less error prone IMHO than fingering in taper compensation manually in the middle of a cnc program at the control.

 

[SeymourDumore]

Unless I misunderstood your question, me thinks you're talking about two different things.
Changing tool offset numbers without an actual toolchange is easily done by simply calling it.
For example Tool 1 having offset registers 1 and 21 assigned, you just need to call it by either T0101 or T0121.
Can be in the motion block or on it's own. The offset register can change everything about the tool, X, Z, nose R, tip direction.

But, me thinks you want to change the tool change position by using a work coordinate instead of machine (G53) coordinate system.
I don't see why that's not possible, but it is a pretty dangerous practice if there is a great variation in tool lengths!
The way around that is to cancel the tool offset before calling the toolchange location that way the turret will always go to the same place.
Something like this:
T0 G59 G00 Z0
should work, but I'm not sure if it's worth the effort.

Personally, I'd stick to using G53 as it is ALWAYS explicit, does not depend on anything else and will ALWAYS put the turret in the very same place.
If you have the macro option on your Haas, then you can just define the safe X and Z coordinates in the header of your program once and make the macro call for each toolchange.

 

[mmurray70]

Yes canceling the tool offset will work, assuming it actually cancels. Ill try that tomorrow and see if it works.

Your right, basically want to move to a work offset position, ignoring the current tool offset. Use G59 as a quick way to program safe tool position.

The macro option doesnt sound too bad either assuming it works. If program was posted out again with changes it would need to be updated though. I feel like a work offset would be easy way of doing it if i can get tool offsets to cancel.

 

[Andy 000000000]

Just move to safe position and in the program have T0000 before recalling the same tool with new offset. Hope this helps.

 

[sinha]

Does Haas need M06 for a tool change on a lathe?

 

[angelw]

Does Haas need M06 for a tool change on a lathe?

Hello Sinha,
No, not at all.

Regards,

Bill

 

[sinha]

Then, it is a typo in post#1 (M6 T0202)
(Unless it is a macro with some safety instructions)

 

[Andy 000000000]

Does Haas need M06 for a tool change on a lathe?

No is the simple answer. However you need to be in a safe position or home before calling the tool.

 

[angelw]

(Unless it is a macro with some safety instructions)

Hello Sinha,
That could be the case for perhaps omitting moving the turret to a safe tool change position, However, given that the OP is looking to use a Work-shift Offset to define a tool change position, then the two would be fighting each other.

Most HAAS machines have User Macro; I've not seen one yet without it. Therefore, the cleanest method would be to do as Seymour suggested and define a Machine Coordinate System value at the head of the program, so that G53 can be used. I'd use a Common, Nonvolatile Variable so that the coordinate value is not affected by Reset, should the program have to be restarted other than at the top of the program.

Regards,

Bill

 

[Vancbiker]

One needs to keep in mind that the machine builder determines if T0000 is acceptable or not. Depends on how the ladder logic is written.

 

[sinha]

One needs to keep in mind that the machine builder determines is T0000 is acceptable or not. Depends on how the ladder logic is written.

I exactly had this question in my mind.

 

[sinha]

I believe T0000 and T0 are equivalent.