Lathe/MTM tool change position

[double a-ron]

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

I went back and forth with them over and over about how you are supposed to move to another tools safe g54 position when the current tools offset is still active. I told them if it was a mill you could use G43 and call the next tools offset, but in a lathe you use g53. Am I right or am I missing something.

[TheEngineer]

Hi
Two possible solutions. I do not have any experience with HAAS machines but this works for Mori Seki and most Fanuc controls.

To make machine back to it's limit stop (home position) in both X & Z use the following.

G28 U0; (For X axis)
G28 W0; (For Z axis)
G28 V0; (For Y axis)

If this option does not work try

G28 Z0;
G28 X0;
G28 Y0;

Take care on this option as some machines will move to the jobs X0 Z0 first.

In both case's you can execute both on same line, but for saftey it is better to do on single lines. You will also need to sort out in which order you do the moves, normally it is X first. On the Mori Seiki's you can actually define a position on the machine as a second reference position (ie operator sets this in parameters) then by executing G30 U0 etc it returns to same position each time.

Hope this is of help, good luck

[double a-ron]

I know how to get the machine home, what I want to know is whether or not their g54 way can ever work. I had to beg them to change my post to output g53 machine coordinates instead of g54. Is it possible or am I right and it simply can never work, unless all tools have the same lengths in x and z. Oh and thanks for replying, no one has ever even given this problem a shot.

[Pondo]

You can post it as G53 and the location would be from the machine home position.
G53 X-5.
G53 Z-8.

Then they would all use the same safe point and not have to go all the way to machine 0. You can set the point at the machine so the farthest X tool and the longest Z tool clear the workpiece.
G53 is non-modal. It is active for only the line it is in.

[double a-ron]

YDNA in the haas forum solvd it for me. If you place a txxx after the position you want to move to it will move the way I was thinking it would need to move to make this work. I.E.:

x.1 z.1 t303

I have always used G53 as my toolchange position I just wanted to know how Gibb's G54 way would work. As I said in the haas forum, knowing how it works it seems stupid to me. The turret would be in a diffrent place for each tool change. G53 puts the turret in the same place for each tool change. Thank you to anyone that posted.

[sld4121]

Interesting that they argued with you about that. My standard posts now allow the user to select the tool change radio button in the documents page to specify a tool change position. And, I output a G53 position using those numbers.

[double a-ron]

The problem is in rendering. They can't render machine coordinates correctly. In fact to "prove" my program I have to put in positive numbers, say x10. z10., then render it in flash cpr. If everything checks out I change the tool change position to back to the g53 tool change position. The biggest problem is g53 is in negative numbers, if left negative and rendered it will always render a crash as soon as it gets to the that first tool change.

[cncrunner]

Hi again double a-ron,

I have a similar issue a while back where gibbs was looking for a positive value, but the controller needed a negative value. In my case it was the x stock amount in the G71 lathe cycle. To get proper cpr, you have to have a positive stock value for I.D. roughing. But that positive value needed to be negative in the cycle. So all that had to be done was reverse the polarity of the x stock command in the post. The cpr was then right, and the posted code also correct.
I am sure the same thing could be applied to your tool change position.