|
|
|
 |
|
 |
|
|
|
|
| |
Back to Main Control Tips Page
(MORE) -
CONTROL TIPS for getting the most out of your Haas CNC.
SETNG Display
 Because the settings give users a great deal of powerful and
helpful command over the control, we recommend reading the entire
Settings section of the operators manual. Listed below are some
of the most useful settings.
Scrolling through Settings with Jog Handle The jog handle can
now be used to scroll through the settings. In previous versions,
the jog handle could be used to scroll through (cursor-highlight)
the parameters, but not the settings. This has been corrected.
(Any Mill Control ver. 10.15 and above; any Lathe Control ver.
3.05 and above)
Setting 1 AUTO POWER OFF TIMER This turns the machine off
after it has been idle for the number of minutes defined in this
setting.
Setting 2 POWER OFF AT M30 This will power off the machine
when an M30 command is executed. In addition, for safety reasons,
the control will turn itself off if an overvoltage or overheat
condition is detected for longer than 4 minutes.
Setting 8 PROG MEMORY LOCK When this is Off, program memory
can be modified. When this setting is turned On, memory edits
cannot be done and programs cannot be erased.
Setting 9 DIMENSIONING This allows the user to choose inch or
metric dimensioning, which will change all Offset values and
Position displays accordingly. This setting will not change
program dimensions to or from inch or metric.
Setting 15 H & T CODE AGREEMENT When this is Off, no special
functions occur. When it's On, a check is made to ensure that the
H offset code matches the tool presently in the spindle. Usually
you have one offset per tool, and it's usually the same number as
the tool number. If it is not the same and this setting is On, you
will get an alarm: H and T Not Matched. This check can help
prevent crashes. If you need to use a different offset number or
more than one, this setting will need to be switched Off. In
program restart, this check is not done until motion begins.
Setting 31 RESET PROGRAM POINTER When this is On, the RESET
key will send the cursor back to the beginning of the program.
Setting 36 PROGRAM RESTART When this setting is Off, starting
from anywhere other than the beginning of a program or a tool
sequence may produce inconsistent results. When it is On, you are
able to start a program from the middle of a tool sequence. Cursor
onto the line where you want to start and press CYCLE START. The
control will scan the entire program to ensure that tools,
offsets, G codes, and axis positions are set correctly before
starting or continuing from the block where the cursor is
positioned. Note: Some alarm conditions are not detected prior to
motion starting. Its best to turn this setting Off when not in
use.
Setting 51 DOOR HOLD OVERRIDE When this is Off, a program
cannot be started when the doors are open, and opening the doors
will cause a running program to stop, just like using the FEED
HOLD key. When it is turned On, and Parameter 57 bits DOOR STOP SP
and SAFETY CIRC are set to zero, this door condition is ignored.
This is one of a few settings that automatically switches back to
its default condition (Off) when the machine is powered down.
Setting 77 SCALE INTEGER F This can be used to change how the
control interprets a feedrate. A feedrate that is entered in your
program can be misinterpreted if you do not enter a decimal point
in the Fnn.nn command. The selections for this setting are
DEFAULT, which assumes a 4-place decimal if no decimal point is
entered (i.e., if you enter F10, it assumes you mean 0.0010);
INTEGER, which assumes a whole number (enter an F10, it assumes
10.0); or .1 (enter F10, it assumes 1.0), .01 or .001 (you get the
idea), or .0001, which is the same as the Default setting.
Setting 84 TOOL OVERLOAD ACTION This is used to determine tool
overload conditions as defined by the Tool Load monitor page in
the Current Commands display (use page down in Current Commands to
get there). A tool overload condition can result in one of four
actions by the control, depending on Setting 84. ALARM will
generate an alarm when overload occurs; FEED HOLD will cause a
feed hold; BEEP will sound an audible alarm; or AUTOFEED will
automatically decrease the feedrate.
Setting 85 MAX CORNER ROUNDING This setting is used to set the
corner rounding accuracy required by the user. The accuracy
defined in Setting 85 will be maintained even at maximum feedrate
the control will only slow at corners when it is needed. This
setting defeats all the years of discussion by competitors who say
you need multiple blocks of look-ahead. The Haas control actually
does look ahead for block interpretation, up to 20 blocks. This is
not needed for high-speed operation. It is instead used to ensure
that DNC program input is never starved, and to allow non-XY moves
to be inserted while Cutter Compensation is on.
Setting 88 RESET RESETS OVERRIDE When this is On, the RESET
key sets all overrides back to 100%.
Setting 101 FEED OVERRIDE > RAPID When this setting is Off,
the machine will behave normally. When it is On and HANDLE CONTROL
FEEDRATE is active, the jog handle will affect both the feedrate
override and the rapid rate override simultaneously. That is,
changing the feedrate override will cause a proportional change to
the rapid rate. The maximum rapid rate will be maintained at 100%
or 50%, according to setting 10. (Any Mill Control ver. 10.22 and
above. Any Lathe Control ver. 4.11 and above)
Setting 103 CYC START / FH SAME KEY This is really good to use
when youre carefully running through a program. When this setting
is On, the CYCLE START button functions as the Feed Hold key as
well. When CYCLE START is pressed and held in, the machine will
run through the program; when its released, the machine will stop
in a feed hold. This gives you much better control when testing a
new program. When youre done using this feature, turn it Off.
This setting can be changed while running a program. It cannot be
On when Setting 104 is On (when one of these is turned on, the
other will automatically turn off). (Any Mill Control ver. 9.06
and above; any Lathe Control ver. 4.11 and above)
Setting 104 JOG HANDL TO SNGL BLK When this is On and you are
running a program in MEM mode, in the Program or Graphics display,
you can use the SINGLE BLOCK key to cycle through your program one
line at a time, with each press of the CYCLE START button. Again,
this works either when the machine is running or youre in
Graphics. Also, if you first press the CYCLE START button, then
each counterclockwise click of the jog handle will step you
through a program line. Turning the handle clockwise will cause a
feed hold. This setting can be changed while running a program. It
cannot be On when Setting 103 is On (when one of these is turned
on, the other will automatically turn off). (Any Mill Control ver.
9.06 and above. Any Lathe Control ver. 4.11 and above)
Setting 114 CONVEYOR CYCLE (MIN) If this is set to zero, the
conveyor will operate normally. If a number is entered, it defines
how long (in minutes) each cycle will be when the chip conveyor is
turned on. The chip conveyor cycle is started with either an M
code (M31 or M32) or with the control CHIP FWD and CHIP REV keys.
It will stay on for the time defined in Setting 115, then turn off
and not restart until the cycle time in Setting 114 has elapsed.
Short programs looped (M99) many times will not reset the chip
conveyor if the intermittent feature is activated. The conveyor
will continue to start and stop at the commanded times.
Setting 115 CONVEYOR ON TIME (MIN) This setting works with
Setting 114, which defines the conveyor cycle time. Setting 115
defines how long the chip conveyor will stay on during each cycle.
Setting 118 M99 BUMPS M30 CNTRS When this setting is On, an
M99 command (used to run a program repeatedly) will activate the
M30 counters that are in the CURNT COMNDS display (page down
twice). Note that an M99 will only activate the counters when it
is used in a loop mode in a main program, not a subprogram. An M99
that's used as a subprogram return, or with a P value to jump to
another part of the program, won't be counted. (Any Mill Control
ver. 9.58 and above; any Lathe Control ver. 3.00 and above)
Setting 130 TAP RETRACT SPEED This feature augments one
introduced in version 10.13, the quick reversal out of a G84
rigid-tapped hole. If Setting 130 is set to 0 or 1, the machine
behaves normally. Setting it to 2 is the equivalent of a G84
command with a J value of 2; that is, the spindle will retract
twice as fast as it went in. If it is set to 3, the spindle will
retract three times as fast. NOTE that specifying a J value in a
G84 command for rigid tapping will override Setting 130. (Any Mill
Control ver. 10.18 and above).
Setting 144 FEED OVERRIDE>SPINDLE This feature is intended to
keep the chip load constant when an override is applied. When this
setting is Off, the control behaves normally. When it is On, any
feedrate override that is applied will be applied to the spindle
speed also, and the spindle overrides will be disabled. (Any Mill
Control ver. 11.10 and above; any Lathe Control ver. 4.11 and
above).
Communications
Program Format to Receive You can receive program files from a floppy
disk or the RS-232 port on the Haas control. A program must begin
and end with a line containing only a % sign. The next line must
begin with the letter "O" followed by the program number (newer
machines use five digits, older machines four). If you want to
identify a program by name as well as program number, enter the
name between parentheses (Program Name), either on the same line
as the program number (after the number) or on the next line. The
program text name will show up with the program number in the list
of programs..
Advanced Editor I/O Edit Menu
Loading Programs from Disk You can load program files from a
floppy disk using the I/O menu and the DISK DIRECTORY item of the
Advanced Editor. Pressing WRITE/ENTER when this menu item is
selected will display a list of the programs on the program disk.
Use the cursor arrow keys or the handwheel to select the file you
need to load, and press WRITE/ENTER. After loading that file, the
disk directory will remain on display to allow more files to be
selected and loaded into the control. RESET or UNDO will exit this
display.
SEND RS232 or SEND DISK You can send programs to the RS232 port
or a floppy disk from the Advanced Editor. After selecting the
menu item you want (SEND RS232 or SEND DISK), a program list will
appear. Select the program you want to save, or ALL (at the end
of the list) if you wish to send all programs under one file name.
Select any number of programs using the up and down cursor arrow
keys or the handwheel plus the INSERT key to mark the specific
programs to send. If no programs are selected from the list using
the INSERT key, the currently highlighted program will be sent.
LIST PROG Mode
Sending a Program File You can send a file or files to a program
disk or through the RS-232 port from the LIST PROG display. Use
the cursor arrow to select the program you want, or select ALL
if you want to send all of the programs under one file name. When
you press F2 to send the selected program(s), the control will ask
for a file name, which can be up to eight characters long with a
three-letter extension (8CHRCTRS.3XT). Then press F2 again to send
it. (You can also use the I/O menu in the Advanced Editor to send
and receive program files.)
Sending Multiple Program Files Several programs can be sent
through the RS-232 serial port from the LIST PROG display, by
typing in all the program numbers together on the input line
without spaces. Each program number should start with the letter
O, and you can leave off any leading zeros if you choose (e.g.,
O123O4545O13579). Then press SEND RS232.
Send and Receive Offsets, Settings, Parameters and Macro Variables
You can save offsets, settings and parameters to a floppy disk,
retrieve them from a floppy, and send/retrieve them via the RS-232
port. To send, press LIST PROG first, then select an OFFSET, SETNG
or PARAM display page. Type in a file name, and then press F2 to
write the display information to disk (or F3 to read that file
from a disk). Press SEND RS232 to send the display page to the
RS-232 port under the file name you entered, or RECV RS232 to read
the file via RS-232. You can also do this with macro variables by
first pressing LIST PROG, then selecting a macro variable display
page (PAGE DOWN from CURNT COMDS).
Deleting a Program from a Floppy Disk Haas machines allow you to
delete files from a floppy disk. (Note that this requires the
latest floppy driver EPROM chip version FV 2.11.) Go to the LIST PROG display page and type DEL <filename> where <filename> is,
naturally, the name of the floppy disk file you want to delete.
Press WRITE/ENTER. The message FLOPPY DELETE will appear, and
the file will be deleted from the floppy disk. If you need to see
the list of remaining file names on the floppy, press F4 and then,
when the DISK DONE message is displayed, press EDIT or MEM.
(Haas mill control software version 9.63 and above; Haas lathe
control ver. 3.00 and above)
RS-232 Communications Using X-Modem If you are seeing occasional
errors when using RS-232 communications, X-Modem (Setting 14) is a
standard communications mode which is very reliable when only a
few errors occur. Our control supports this, as do almost all
software communication packages for PCs.
Haas Rotary Table Using the Serial Port and Macros It is
possible to regulate a Haas rotary table using the serial port and
macros from the Haas control (or any Fanuc-compatible control).
There is a set of sample macros available from the Haas
Applications department.
|
|
|
|
|
|
|
