G54 shift

[Born2L8]

I want to make 3 parts at a time from bar stock - no feeder. How do I program one part, part it off, and then shift the Z face measure to cut another part? This is on a new TL-2.

Thanks!

Charlie

[Hdpg]

Set your tool offsets with no entries in the G54 work coordinate.

Make your program a subroutine.

In the main program that calls the subroutine have G10 commands to set G55 ahead by one part length and G56 by two part lengths, both including the parting allowance. Call the subroutine using G54, then G55 and G56 like this:

O00000
(Three parts from barstock)
G10 L2 G90 P1 Z0.0 (Make sure G54 is zero)
G10 L2 G90 P2 Z-one part length (Set G55 at one part length)
G10 L2 G90 P3 Z-two part lengths (Set G56 at two part lengths)
G54 M97 P1000
G55 M97 P1000
G56 M97 P1000
G28
M30
(-----)
N1000
(Part program)
M99


You can also do it using G52.

[SeymourDumore]

Tough hdpg's example is correct, a Haas without a toolsetter almost never has a Z0 in the offset page.
I would strongly suggest the G52 method in one program OR! preset the workoffsets.

O00000
(Three parts from barstock)
M97 P1000
G52 Z-one part length
M97 P1000
G52 Z-two part length
M97 P1000
G28
M30
(-----)
N1000
(Part program)
M99


The nice thing, Haas automatically clears G52 workoffsets on a lathe after an M30

The other way with preset workoffsets is:

O00000
(Three parts from barstock)
G54 M97 P1000
G55 M97 P1000
G56 M97 P1000
G28
M30
(-----)
N1000
(Part program)
M99

I use the second method because of my preference to have all changes to be made external to the program. For example switching from a .094 cutoff tool to a .125 leaves the program intact, just change the offsets instead.

[SIM]

Originally Posted by SeymourDumore

Tough hdpg's example is correct, a Haas without a toolsetter almost never has a Z0 in the offset page.
I would strongly suggest the G52 method in one program OR! preset the workoffsets.

O00000
(Three parts from barstock)
M97 P1000
G52 Z-one part length
M97 P1000
G52 Z-two part length
M97 P1000
G28
M30
(-----)
N1000
(Part program)
M99


The nice thing, Haas automatically clears G52 workoffsets on a lathe after an M30

The other way with preset workoffsets is:

O00000
(Three parts from barstock)
G54 M97 P1000
G55 M97 P1000
G56 M97 P1000
G28
M30
(-----)
N1000
(Part program)
M99

I use the second method because of my preference to have all changes to be made external to the program. For example switching from a .094 cutoff tool to a .125 leaves the program intact, just change the offsets instead.

I prefer the 2nd option myself, always starting the program with a G54 call.
It prevents the machine from starting and thinking it is several pieces into the bar.


I have used G52 to modify G54 in a loop or sub call, it works great except if you reset the program and G54 does not revert back to the original G54, or the machine alarms out and you do not reset the G54 to Zero.

[Born2L8]

Thanks, Guys

We got the stock today and will try it out tomorrow, I hope.

Charlie

[Paragon_R_N_D]

You could always cut the bars into longer lengths and use a barpuller? Just a suggestion.

[SIM]

Originally Posted by Paragon_R_N_D

You could always cut the bars into longer lengths and use a barpuller? Just a suggestion.

Sometimes the bar won't fit thru the spindle, but run several parts per slug.

I run a quick and dirty job with a bar puller...the part is done so fast that the puller is by far the longest operation, so I pull enough to make 6pcs (using multiple Work offsets) then pull. Saves alot of time on several thousand parts.

[Hdpg]

Originally Posted by Paragon_R_N_D

You could always cut the bars into longer lengths and use a barpuller? Just a suggestion.

We are talking Haas TL2 here; bar pullers are not really practical with a manual chuck.

Also on a TL2 the spindle bore is so large if the bar will fit inside the chuck it will fit through the spindle.

[Born2L8]

Gee, ain't it funny how the the bore is 3 1/4,IIRC , but the chuck hole is 2 7/8?
We, tried the program today and it will loop over but not move to G55. It just starts all over at the same G54. We used the "second method".

I'll try to post the entire program, or at least pertinent parts later.

And, yes, we did enter the offsets in the offset page.

Charlie

[Hdpg]

Spindle bore is a few thou less than 3".

You mention it will loop over but not move to G55

You do not loop the program, you have to call the subroutine after a G55 command, something like this:

G54
M97 P1000
G55
M97 P1000
M30
-----
N1000 This is the part program

[sentinal2000]

hello , newbie here , still trying to work out how to start a new thread ( wish it was as easy as the intuitive is on my new haas tl1)

does anyone know how to unlock the new tl1 ect . i want to change some parameters but the display keeps giving out " locked " on some of the functions .
any idea's? its a brand new machine , late 09
thanks all.

[Hdpg]

Setting 7 Parameter Lock, turn it off.

Regarding starting a Thread look up the top of the page and you will see ...specific machine forums > haas

Click on haas and that takes you to the main page for the forum and there you will see the New Thread button.