Haas Tool Change Macro

[GoetzInd]

Hi Guys,

Anyone running a Fanuc style tool change macro on a haas? We've got one here and I want to put some safety stuff in that is similar to all of our other machines. Problem is, doesn't look like haas has a sub M code call like Fanuc. Any ideas?

 

TIA

Mike

[Machineguy]

I have seen it done on a VM-8. A macro was written to to change tools on the far right side. It was for picking up right angle heads that wouldnt fit in the toolchanger.

Special rack was made. Made the pgm rum without any stops.

 

Machineguy

[Craig-B]

I tried it, a while back, but I dont think the Haas will allow you to use the M6 inside the macro like the Fanuc

[mkd]

Haas has a setting to only change tool with the table (automatically) moved to home position.

i have not heard of any ablity to assign new G or M codes.

 

i would think one would have to just call a macro (or sub program) to get the specified/needed results.

[CJep]

Mike,

Are you wanting to send the table to an auxiliary position for a tool change?

You could use the reference points in the tool path to set that.

 

I also changed the G28 output in my post to G53 to send the machine to it's home position, it also allows you to stay in G90 absolute mode instead of switching to G91 incremental with the G28.

[GoetzInd]

Not really looking to move table but more of stuff like checking tool gage length, probe in spindle, wear values present during first run, stuff like that.

 

I tried it, a while back, but I dont think the Haas will allow you to use the M6 inside the macro like the Fanuc

 

Thats what I'm running into. Dang Haas's!

[mkd]

has a sub M code call like Fanuc

 

not sure of the question:

m98 pxxxx (jump to program)

m99 pxxxx (jump to block p)

G65 (sub call passing variables)

GOTO xxxx (jump to block)

m97 (internal sub)

[GoetzInd]

Ok on a Fanuc control you can assign a sub call to an executing M code (M6 Does a toolchange) and have it call a sub program. So every time you call an M06, it executes the program along with it. Very handy.

 

Mike

[cncchipmaker]

Ok on a Fanuc control you can assign a sub call to an executing M code (M6 Does a toolchange) and have it call a sub program. So every time you call an M06, it executes the program along with it. Very handy.

 

Mike

Couldn't you just write a sub routine or use a G65 call after the tool change if you cannot write to the Haas Tool Change Macro. I think I am understanding your question so here are some options:

 

T1M6

M98P0001

 

OR

 

T1M6

(A=#1 TLO)

(B=#2 PROBE IN SPINDLE)

(C=#3 WEAR VALUES)

G65P0001A1.B1.C1.

 

Either scenario will work depending on how the Haas control reads the system variables. You could write a macro that pulls all of the data you need and write them to corresponding macro variable outputs so you can read them.

I have never tried this before but I think I know what you are wanting to do with your TLO value.

Set a max TLO at the beginning of your program that corresponds to each tool like #501 equals the max stickout of tool number 1. #501=5. So #501 TLO will not be greater than five inches.

Lets pretend that your system variable for TLO is #2001=TLO#1 which on most Fanucs I believe is the case

 

If you use the G65P0001 the program will go as follows:

Main Program

#501=5.

T1M6

G65P0001A1.

M30

 

O0001

#100=#1.+2000.(Set #100 to 1.+2000./ in this case system variable #2001)

#101=#1.+500.(Set #101 to 1.+500./ in this case variable #501)

IF[#[#100]LT#[#101]]GOTO1(If the TLO is the write length go to line number 1)

M00(TOOL TOOL LONG)

(COMPARE OFFSETS #100 & #101)

N1

M99

 

Your options are unlimited.

[GoetzInd]

Yes,

And that's probably what I'll have to end up doing. Just like the idea of keeping everything clean and simple as well as having things the same across the board.

 

Thanks

Mike

[dforsythe]

Start by creating a 9### program

 

Add in your safe tool change information like:

 

G0 G91 G28 Z0

G0 G90 G53 X### Y### ( safe tool change position ) we use x-39.0 y18.5 on our vf-6 ( directly over the touch probe )

Any other code you want

M99

 

Next assign the 9### program an open variable ( we use M106 )

 

Then replace your m6 in your programs with M106

 

All tool changes will be safe.

[GoetzInd]

Next assign the 9### program an open variable ( we use M106 )

 

Then replace your m6 in your programs with M106

 

Exactly the direction I went.

 

Mike