Lathe tool change position

[double a-ron]

I have posted this in the GibbsCam forum twice now and I thought I would try it here. I want to make it clear that I allready know how to properly code a safe tool change position using either G28 or G53. I want to know if GibbsCams way can work or not. Here is what I posted in the Gibbs forum:

I have asked this question before and never gotten a straight answer. Maybe someone can help me out. The machine in question is a Haas lathe. In GibbsCam MTM, they make you specify a global tool change position. Global meaning any time a tool change happens it moves the machine to the x and z coordinates I enter in the "tool change position" field. Sounds reasonable right? Here is where things get funny. The tool change position is in G54. This made me so confused because in my eyes there is no way you can set a "global" g54 tool change position for all tools. Example: Tool 2 is in position, therefore, you are on tool 2's offset. Tool 2 is an od turning tool in pocket 2. It has a large x offset, but a short z offset. Your now changing to tool 3. Tool 3 is a drill bit in a vdi pocket in pocket 3. It has a small x offset, but a long z offset. You set the tool change position to .1 clearance in x and .1 clearance in z. When changing from tool 2 to tool 3 how do you avoid crashing tool 3 into the workpiece? Remember tool 2's offset is still active until tool 3 is in position. See:

O1( 1.NCF )
(TOOL 2 IN POSITION)
G54 X.1
Z.1
N1 T202
X.1
Z.1
M01
N2 T303 (crashes in z because it was only.1 away from the workpiece in z based on t2's offset because it was still active.)
X.1
Z.1
N3 T202
M30

[Ydna]

It might be as simple as the Txxxx code being all by itself. I think if you place the Txxxx code on the end of a line with your desired position change, the turret will activate the new offset BEFORE moving to the coordinates, then execute the toolchange once it gets there. Example:
T101
G0 X1.
....
X5 Z8 T303
(machine uses offset 3 and moves to its X5Z8, then changes to pocket 3 once the turret gets there).

That's how our HL-2 does it anyway. It's a bit of an older lathe though so I can't speak to anything else without toying around with any of our newer machines.

[double a-ron]

You got it! Also using your method you can move each axis individually with another tools offset without changing to that tool. Example:

O1( 1.NCF )
(TOOL 2 IN POSITION)
G54 X.1
Z.1
N1 T202
X.1 T203
Z.1 T203
M01
N2 T303
X.1T302
Z.1T302
N3 T202
M30

Now that I see how a G54 tool change position would work I hate it even more. I believe that a tool change position should move the turret to the same "safe spot" in the machine no matter what the tools offset is. My lathe being the dual spindle TL-15, this is even more important. So I simply jog the turret to a safe spot between the two spindles and index the turret through all the tools. If nothing crashes, I record were I am in machine coordinates and use that as my G53 tool change position. Well thanks again, no one has ever been able to answer that question before.

[Ydna]

Yeah, that's how I program toolchanges too, for safety. Although I will admit I've altered the positions of individual toolchanges in the past, so that they only move as far as needed for the index to occur. Going from tool 1 to tool 2, rotating int he correct direction, for instance. But that's obviously a very risky move since the program has to be totally and completely proven first.
I only do that when I'm the one running the parts, since someone not familiar with the program structure/sequence might change something on their own and cause a humongous crash...ouch