Custom tool change position

[gpcoe]

We have an '06 VF3SS with a 5X trunnion table on it. We would like to have the machine go to a pre-determined X,Y position when doing tool changes to be sure that the tools clear the trunnion. Is there a way to do this with just the M06? In other words I could hand edit in a reposition move, but I'd like to be able to edit the M06 subprogram so that it does this automatically whenever an M06 is called up. Is there a way to see the behind the scenes programming and edit it?

Thanks

Greg

[txcncman]

You should be able to do this, but then you would be stuck doing this even when it was no longer needed. A better solution might just be to call a G0 G53 Xxx.xxx Yxx.xxx position before a tool change. You should be able to change your CAM post processor to do this for you and label it for this particular machine. If you think you need to edit the machine control, read up on macros.

[Machineit]

+1

Since you are running a five axis machine, I would assume that you don't do a bunch of hand programming at the machine.

Modify a post processor for your CAD/CAM system that adds the appropriate line and use it for that particular machine.

For current programs, just write the new line of code, add the M06 for the next line and do a global search and replace. Bamm, you're done.

Mike

[tc26]

I have a sub program in the control that puts the tool change at the extreme left of the table on our vf2.
I use M98P28 before all tool changes.
My post processor has been modified to output this sub call before every tool change.
I am sure there are other ways to do the same thing, but this one worked for me.
Here is the sub program:

%
O28
( M6 HOME )
G10 P99 L20 G90 X-30.
G91 G28 Z0
G28 D0 Y0
G0 G90 G154 P99 X0
M99
%

[glovebox20]

We have an '06 VF3SS with a 5X trunnion table on it. We would like to have the machine go to a pre-determined X,Y position when doing tool changes to be sure that the tools clear the trunnion. Is there a way to do this with just the M06? In other words I could hand edit in a reposition move, but I'd like to be able to edit the M06 subprogram so that it does this automatically whenever an M06 is called up. Is there a way to see the behind the scenes programming and edit it?

Thanks

Greg

Easy!

Change Setting #82 to 6 (M-code to run O9001). E-spot must be on to change this setting.

Now create a O9001 program with all the codes nessary to do a safe tool change.
ex.

%
O9001
G91G28G0Z0M9
G90G53G0X-38.5Y-2.5M19
M16 (CHANGE TOOL)
M99
%

Now when use T3 M06 in your program, it will run the sub program #9001 and swap tools. Also work in MDI as long as you type T# & M6 and run the MDI program. The 'Next Tool' and T# ATC FWD/ ATC REV will not use program O9001!!!!!! Works great for swing arm tool changers. The only down fall is you must turn T&H agreement off if you want to 'graph/verfiy' your program.

Being a 5 axis, I'm sure you may want to add a few code to ensure a safe TC.


What? Safe TC no longer needed. Just set Setting #82 back to Zero and your back in business. I do this All the time when working with extremly tall parts/tooling.

[gunome]

Under parameters look for tool change offsets for the axis you want. In debug under position raw data page get your encoder count for the axis you want to position. (joged to postion out of way). Use actual enter value from actual and you should be set, may depend on software. Your dealer should be able to provide you info on this.

[gpcoe]

Tried the debug/parameter trick and it still wouldn't move in X/Y so I went ahead and made the subprogram O9001 and that worked like a charm.

Thanks a lot guys

Greg

[extanker59]

glovebox20, very nice. That went into my notes.

[glovebox20]

Caution!!!

When useing Program Restart & the 'subbing' of you Tool Change Program, Be sure to restart the mill with the correct tool!!. It will skip the TC code altogether and use what ever tool is in the spindle to do the operation, which could be very bad.

I thought I would give you guys a head up.


glovebox20

[Jimmy Oxford]

I had the same problem and called my Haas rep. He had me change the home location in the parameters. The problem with this was the z axis did not move by itself when directed home but moved all three at the same time for tool change or home position. Talk about a crash waiting to happen. So I program the best way in and out for each tool depending on the angles of the trunnion.

[Kevinckb3]

Under parameters look for tool change offsets for the axis you want. In debug under position raw data page get your encoder count for the axis you want to position. (joged to postion out of way). Use actual enter value from actual and you should be set, may depend on software. Your dealer should be able to provide you info on this.

There are two parameters for each axis. If set correctly the machine will move to this position under any tool change circumstance. Powerup restart , next tool atc fwd etc. Call your dealer for more info they should be able to help you over the phone set up a safe tool change
When not wanting to move to this tool change position you only need to change one parameter

[Kevinckb3]

I had the same problem and called my Haas rep. He had me change the home location in the parameters. The problem with this was the z axis did not move by itself when directed home but moved all three at the same time for tool change or home position. Talk about a crash waiting to happen. So I program the best way in and out for each tool depending on the angles of the trunnion.

how did you direct the Z axis home?