Need Help!- Tool Changer

[Doubleddaved]

I have a new vf8-50 with side mounted tool carousel. I'm trying to figure how this thing works.My other 2 vertical mills are very simple. You call up t2m6 and in rotates to #2 and does the tool change.T1 is in pocket 1 ,T2 is in 2 and so on.It basically does what you tell it to.
My question is, on the Haas when I put a tool in the spindle and set my offset for say T1 does the Haas know where this tool is in the carousel regardless of what pocket it's in?
Thanks for any help.
I'm sure I'll have my questions to follow
Thanks
Dave.

[HAILINHAAS]

Yes . it remembers where it put each tool .. as long as your calling out that tool and load the tool that corresponds ... the offset page will show you pocket number and what tool is in that pocket

[HAILINHAAS]

you can input the tool number to what pocket in the offset page also

[kurt66]

yes the machine will keep track of what tool is in each pocket regardless of the numer you see on the actuall tool changer

[PBMW]

In case nobody has already said...yes it remembers where the tool is.

[bishb25]

Doubleddaved,
It looks like you got your answer, but if I may be more specific about the side mount tool changer I believe this thread could be a lot of help to others.

As you have already pointed out the tools in a side mount tool changer do not always land in the same pocket all of the time. The machine does, however, remember which tool is in which pocket and which tool is in the spindle.

Two of the benefits of the side mount tool changer are speed and it gives you an extra tool. For example, if you have a 24 pocket tool changer, your machine can hold 25 tools counting the tool in the spindle. The speed comes from reducing the number of operations required to make a tool change.
Example:
With an umbrella style changer the machine must place the current tool in its original pocket, then index to the next tool and pick it up. This process is painfully slow as I'm sure you have already noticed.
With a side mount changer the carousal indexes to the next tool as the spindle returns "home" and the tool change arm grabs both the current tool and the next tool at the same time and swaps them both. Depending on the machine this can be done in a few seconds. I have a VF-2SS that boasts a 4 second chip to chip too change.

The tool swapping is why the tools don't end up in the same pocket each time. If tool 3 is in the spindle and tool 5 is next in the program and is in pocket 5 at the tool change tool 5 will be paced in the spindle and tool 3 will be placed in pocket 5.
If you press the "offset" button on your control panel then press "page up" a couple of times you will find a page that displays the location of each tool in the tool changer and spindle. This can help you keep track of your tooling if you need it.

Now lets suppose you are setting up a job and need a tool holder that is currently in the tool changer, but you don't know that tool's number off the top of your head. All you have to do is look at the pocket number on the tool changer then press "MDI", type "P(+pocket number)", then press "ATC forward" or "ATC reverse." The machine will index to that pocket then put whatever tool is there into the spindle. If you already know the tool number you can replace "P" with "T". This can be faster than entering T2M06 into the MDI command window and pressing "cycle start". The "P" command is way better than digging though a program looking for the right tool number especially if the programmer is sloppy and doesn't use comments or neat and orderly blocks of code.

Finally, I'll leave you with a trick I use to speed up tool change times on my VF-2's.
I find the "look ahead" on the Haas control to be lacking. It only reads maybe 3 lines at a time unless you have the "High Speed Machining" option. This left me always waiting for the tool changer to index to the next pocket. What a wast of valuable production time! So, I found out from a HAAS salesman that if you enter a "T" command without the "M06" the tool changer will index to that tool without making a tool change or affecting your "H" command.
My programs look like this:

T2M06(3/8 SPOT DRILL)
T3
G90G54G00X0.Y0.
S1500M03
G43H02G00Z1.M08
G82G99Z-.187P.1R.1F4.5
X1.
G80G00Z1.M09
G53G49G00Z0M05
M01

T3M06(F DRILL)
T4
AND SO ON....

At the last tool in the program I will call the first tool again in order speed up repetitive production cycles. It may not seem like too much time, but when you run the same job for weeks on end a few seconds can add up to hours.

I hope this helps all who see this thread
I'm sure you'll love your VF-8, Doubleddaved.

Keep makin' chips.