(too old to reply)
Haas - disable mill tool changer?
dlevy
2005-02-07 18:42:25 UTC
We need to disable the tool changer on the mill (TM-1) because the part is
too tall to use the tool changer. Anyone know how to disable the tool
changer?

TIA
Black Dragon
2005-02-07 18:52:00 UTC
Post by dlevy
We need to disable the tool changer on the mill (TM-1) because the part is
too tall to use the tool changer. Anyone know how to disable the tool
changer?
Derp!

Don't program any tool changes?

Sheeze, it doesn't get any simpler than that.
--
Black Dragon

http://www.nice-tits.org/pics.html
Robin S.
2005-02-07 21:38:29 UTC
Post by Black Dragon
Derp!
Don't program any tool changes?
Sheeze, it doesn't get any simpler than that.
It's been a while since I used a Haas with a programmable coolant nozzle,
but not using an M6 may create issues with it....

Regards,

Robin
Mitch
2005-02-07 22:03:52 UTC
Post by Robin S.
It's been a while since I used a Haas with a programmable coolant nozzle,
but not using an M6 may create issues with it....
ISTR there is an M-code for that (up/down 1 position) - but in any case,
since no automatic tool changes will be programmed, you can use the clnt
up/dn buttons on the panel at manual tool changes (if any).

Probably somewhere in the parameters there are some settings to tell the
machine there is no tool changer as well...
--
Cheers,

--Mitch
Robin S.
2005-02-07 22:35:15 UTC
Post by Mitch
Probably somewhere in the parameters there are some settings to tell the
machine there is no tool changer as well...
Yeah. I would want to turn it off just so the operator doesn't try to
perform a toolchange out of habit. Expensive mistake...

Regards,

Robin
garibaldi
2005-02-08 00:25:50 UTC
Post by Black Dragon
Post by dlevy
We need to disable the tool changer on the mill (TM-1) because the part is
too tall to use the tool changer. Anyone know how to disable the tool
changer?
Derp!
Don't program any tool changes?
Sheeze, it doesn't get any simpler than that.
Doh! I have to agree on this one. Can't you call the tool and offsets
without doing a tool change, on a Haas?

What is so difficult about noticing something that is so out of the
ordinary (big ole ugly part) that only any idiot wouldn't see it ....
never mind.

<G>
BottleBob
2005-02-08 01:27:42 UTC
Post by Black Dragon
Post by dlevy
We need to disable the tool changer on the mill (TM-1) because the part is
too tall to use the tool changer. Anyone know how to disable the tool
changer?
Derp!
Don't program any tool changes?
Sheeze, it doesn't get any simpler than that.
BD:

Our Haas mill automatically does a tool change to tool #1 as part of
its start-up procedure. The part would have to be done before the
machine is shut off, or perhaps don't shut the machine off.

--
BottleBob
http://home.earthlink.net/~bottlbob
Anthony
2005-02-08 01:50:36 UTC
Post by garibaldi
Doh! I have to agree on this one. Can't you call the tool and
offsets without doing a tool change, on a Haas?
What is so difficult about noticing something that is so out of the
ordinary (big ole ugly part) that only any idiot wouldn't see it ....
never mind.
<G>
See my sig line.....
--
Anthony

You can't 'idiot proof' anything....every time you try, they just make
better idiots.

Remove sp to reply via email
yourname
2005-02-08 03:32:31 UTC
Post by BottleBob
Our Haas mill automatically does a tool change to tool #1 as part of
its start-up procedure. The part would have to be done before the
machine is shut off, or perhaps don't shut the machine off.
the more I read about some stupid ass machines, the gladder I am I aint
got one.

I mean in order to change the tool, ithas to know which one it has, if
it already knows what tool it has, why the hell does it change it,
unless you ask it to
BottleBob
2005-02-08 03:57:07 UTC
Post by yourname
Post by BottleBob
Our Haas mill automatically does a tool change to tool #1 as part of
its start-up procedure. The part would have to be done before the
machine is shut off, or perhaps don't shut the machine off.
the more I read about some stupid ass machines, the gladder I am I aint
got one.
I mean in order to change the tool, ithas to know which one it has, if
it already knows what tool it has, why the hell does it change it,
unless you ask it to
Yourname:

Catchy handle there.

I don't know why it would be programmed from the factory to do that. I
suppose there 'might' be a parameter that could be changed, or if it
were really important, the start-up macro could be altered. It was
never a that big a deal to us to bother with.

--
BottleBob
http://home.earthlink.net/~bottlbob
garibaldi
2005-02-08 05:04:19 UTC
Post by BottleBob
Our Haas mill automatically does a tool change to tool #1 as part of
its start-up procedure. The part would have to be done before the
machine is shut off, or perhaps don't shut the machine off.
--
BottleBob
http://home.earthlink.net/~bottlbob
Bob,

I thought you had Fadals. If so, is this one of their little quirks
as well?

<G>
PrecisionMachinisT
2005-02-08 05:29:16 UTC
Post by garibaldi
Post by BottleBob
Our Haas mill automatically does a tool change to tool #1 as part of
its start-up procedure. The part would have to be done before the
machine is shut off, or perhaps don't shut the machine off.
--
BottleBob
http://home.earthlink.net/~bottlbob
Bob,
I thought you had Fadals. If so, is this one of their little quirks
as well?
No, a Fadal remembers what tool is in the spindle and so it doesnt need to
index on startup.
--
SVL
Mitch
2005-02-08 06:45:19 UTC
Post by BottleBob
I don't know why it would be programmed from the factory to do that. I
suppose there 'might' be a parameter that could be changed, or if it
were really important, the start-up macro could be altered. It was
never a that big a deal to us to bother with.
As far as I know, the control doesn't know where the tool changer is at
startup - tool changer needs to find its reference (there's a switch), which
is at tool #1. Mine doesn't do an automatic tool change on startup
(unless I hit powerup/restart), but the first time you want to change a
tool, it will go to #1 first to reference. But my machine is 5 years old,
something may have changed since.
--
Cheers,

--Mitch
Black Dragon
2005-02-08 08:55:29 UTC
Post by BottleBob
Post by Black Dragon
Post by dlevy
We need to disable the tool changer on the mill (TM-1) because the part is
too tall to use the tool changer. Anyone know how to disable the tool
changer?
Derp!
Don't program any tool changes?
Sheeze, it doesn't get any simpler than that.
Our Haas mill automatically does a tool change to tool #1 as part of
its start-up procedure. The part would have to be done before the
machine is shut off, or perhaps don't shut the machine off.
Not perhaps don't turn the machine off, just don't turn the machine off
period if there's a large work piece that's going to prevent the machine
from being referenced in it. The last two places I've worked the machines
were never shut off except for maintenance and long weekends.

It has been quite a while since I've used a Haas, 6 years to be exact,
and I don't remember how they behaved at start up. I have though, for the
past 25 years, been shoe-horning oversize work in undersize machines, and
know for a fact because I've done it on a Haas, that a work piece that just
barely clears the tool carousel can be *programmed* around vs disabling it
via a parameter or somesuch.
--
Black Dragon

http://www.nice-tits.org/pics.html
Mitch
2005-02-08 09:02:49 UTC
Post by Mitch
Probably somewhere in the parameters there are some settings to tell the
machine there is no tool changer as well...
It's right on the first parameters page.
Parameter 57, second position:

DISABLE T.C.

Set it to 1 to disable the toolchanger.
--
Cheers,

--Mitch
Why
2005-02-08 09:04:05 UTC
Post by Mitch
As far as I know, the control doesn't know where the tool changer is at
startup - tool changer needs to find its reference (there's a switch), which
is at tool #1. Mine doesn't do an automatic tool change on startup
(unless I hit powerup/restart), but the first time you want to change a
tool, it will go to #1 first to reference. But my machine is 5 years old,
something may have changed since.
Mine is only 6 months old & does the same. I changed the prms to load
T10 (empty pocket) which I shut it down with T10 so as to have no tool
holder in the spindle. On powerup/restart it will go thru all tool
pockets & re-load the empty T10.
Black Dragon
2005-02-08 09:19:13 UTC
Post by Robin S.
Post by Black Dragon
Derp!
Don't program any tool changes?
Sheeze, it doesn't get any simpler than that.
It's been a while since I used a Haas with a programmable coolant nozzle,
but not using an M6 may create issues with it....
If the tool carousel is in the way, it's possible a programmable coolant
nozzle may get in the way too. I have temporarily removed said nozzles
and jury rigged some lock line in place to be able to reach down into
some deep mold cavities, and even cut some tall cores, in Haas's.

When doing oversize work, you need to be on your toes. And you *must*
think outside the box, or you're going to be smashing the work piece
into it, guaran-fucking-teed.
--
Black Dragon

http://www.nice-tits.org/pics.html
Mitch
2005-02-08 12:23:29 UTC
Post by Why
Mine is only 6 months old & does the same. I changed the prms to load
T10 (empty pocket) which I shut it down with T10 so as to have no tool
holder in the spindle. On powerup/restart it will go thru all tool
pockets & re-load the empty T10.
I always leave T1 empty. I start my tools with T2 (unless I've got all 20
tools loaded - rare). I shut the machine off with T1 (no tool in the
spindle). This way, at startup, the toolchanger is already "homed" , so as
soon as the machine starts it's ready to go, a tool change will go directly
to the desired tool.
--
Cheers,

--Mitch
CNC Solutions
2005-02-08 13:59:16 UTC
Post by BottleBob
Post by yourname
Post by BottleBob
Our Haas mill automatically does a tool change to tool #1 as part of
its start-up procedure. The part would have to be done before the
machine is shut off, or perhaps don't shut the machine off.
the more I read about some stupid ass machines, the gladder I am I aint
got one.
I mean in order to change the tool, ithas to know which one it has, if
it already knows what tool it has, why the hell does it change it,
unless you ask it to
Catchy handle there.
I don't know why it would be programmed from the factory to do that. I
suppose there 'might' be a parameter that could be changed, or if it
were really important, the start-up macro could be altered. It was
never a that big a deal to us to bother with.
--
BottleBob
http://home.earthlink.net/~bottlbob
on the Hass go to the "settings" page and look for "tool at power down" It
is set to "1" for the factory. If you want it to not do a tool change at
power up or power up/restart, set this setting to "0" the it will not do a
tool change. If you need to program a manual tool change, do not use the m06
command, have the machine stop at m00 and have the operator switch to handle
jog, replace the tool with the new one , then switch back to memory mode.
there is also a setting for tool calls "H and T much match" which you can
turn off.(dangerous in some cases). Then call for a g43 height offset # that
is set for the new tool.
T1
G0 X0 Y0
G43 H1 Z1.0

(YOUR PROGRAM GOES HERE)

G0 G91 G28 Z0
G90
M00 (SWITCH TO MANUAL MODE AND LOAD NEXT TOOL)
M00 (DID YOU?)

T1
G0 X0Y0
G43 H2 Z1.0 (NOTE DIFFERENT H CALL)

The setting page provides a lot of control over the machine and it's
options.
--
Darcy Norton
CNC Solutions
Edmonton, Alberta, Canada

***@shaw.ca
CNC Solutions
2005-02-08 14:13:11 UTC
Post by CNC Solutions
Post by BottleBob
Post by yourname
Post by BottleBob
Our Haas mill automatically does a tool change to tool #1 as part of
its start-up procedure. The part would have to be done before the
machine is shut off, or perhaps don't shut the machine off.
the more I read about some stupid ass machines, the gladder I am I aint
got one.
I mean in order to change the tool, ithas to know which one it has, if
it already knows what tool it has, why the hell does it change it,
unless you ask it to
Catchy handle there.
I don't know why it would be programmed from the factory to do that. I
suppose there 'might' be a parameter that could be changed, or if it
were really important, the start-up macro could be altered. It was
never a that big a deal to us to bother with.
--
BottleBob
http://home.earthlink.net/~bottlbob
on the Hass go to the "settings" page and look for "tool at power down" It
is set to "1" for the factory. If you want it to not do a tool change at
power up or power up/restart, set this setting to "0" the it will not do a
tool change. If you need to program a manual tool change, do not use the
m06 command, have the machine stop at m00 and have the operator switch to
handle jog, replace the tool with the new one , then switch back to memory
mode. there is also a setting for tool calls "H and T much match" which
you can turn off.(dangerous in some cases). Then call for a g43 height
offset # that is set for the new tool.
T1
G0 X0 Y0
G43 H1 Z1.0
(YOUR PROGRAM GOES HERE)
G0 G91 G28 Z0
G90
M00 (SWITCH TO MANUAL MODE AND LOAD NEXT TOOL)
M00 (DID YOU?)
T1
G0 X0Y0
G43 H2 Z1.0 (NOTE DIFFERENT H CALL)
The setting page provides a lot of control over the machine and it's
options.
--
Darcy Norton
CNC Solutions
Edmonton, Alberta, Canada
I forgot to add that the tool changer does have a "HOME" position at
station #1. Use T1 in your program and park it overnight at T1 and it will
not have to search for tool home at power up.

Next Page >
Page 1 of 2