|
|
|
 |
|
 |
|
|
|
|
| |
Back to Main Control Tips Page
(MORE) - CONTROL TIPS for getting the most out of your Haas CNC.
Jog Keys
You can select an axis for jogging by entering the axis
letter on the input line and then pressing the HAND JOG button.
This works for the X, Y, Z, and A axes as well as for B, C, U, and
V auxiliary axes.
OVERRIDE Keys
 Jog Keys & Feedrates There are a number of ways to control
feedrate with the Haas CNC.
1) The JOG keys (+X, -X, +Y, -Y, +Z, -Z, +A, -A, +B, -B) use the
jog speeds of 100., 10., 1. and .1 inches per minute listed next
to the HANDLE JOG key (jogging with the handwheel uses the .1,
.01, .001 and .0001 inch increments).
2) You can also adjust feedrate using the Feedrate Override
buttons (10, +10, 100%), which allow you to increase or decrease
feedrate in 10% increments (up to 200%).
3) The HAND CNTRL FEED key will adjust the programmed feed by 1%,
either up or down, with every increment of the jog handle.
Spindle Speed Similarly, pressing the HAND CNTRL SPIN key will
allow you to adjust the programmed speed by 1%, up or down, with
every increment of the jog handle.
You can stop or start the spindle with CW or CCW any time youre
at a Single Block stop or a Feed Hold. When you restart the
program with CYCLE START, the spindle will be turned back on to
the previously defined speed.
 Manual Overrides for Coolant & Chip Auger The coolant pump can
be turned on or off manually while a program is running, by
pressing the COOLNT button.
This will override what the program is doing until another M08 or
M09 coolant command is executed. This also applies to the chip
conveyor, using the CHIP FWD/STOP/REV keys.
Coolant Spigot Position The coolant spigot position can be
changed manually when a program is running, with the CLNT UP or
CLNT DOWN key. This will override what the program commands until
another spigot position is commanded with an Hnn or M08 command.
Chip Conveyor The chip conveyor can be turned on or off while a
program is running, either manually using the control keys or via
program M codes. The M code equivalent to CHIP FWD is M31, CHIP
REV is M32, and CHIP STOP is M33. You can set the conveyor cycle
time (in minutes) with Setting 114, and conveyor on-time (in
minutes) with Setting 115.
Miscellaneous Things That Are Handy to Know
Actual Spindle Speed You can verify exact spindle speed
on the first page of the CURNT COMDS display. The actual speed is
displayed in the bottom right corner, as well as in the far right
column of the G-code list (ACT Snnnn).
Block Delete Program blocks beginning with a slash ( / )
will be ignored i.e., that program line will not be executed
when Block Delete is on. This takes effect four lines after the
BLOCK DELETE key is pressed when cutter compensation is in use, or
two lines later when cutter compensation is not in use.
Block Look-Ahead The Haas control looks up to 20 blocks
ahead for block interpretation. This is used to ensure that DNC
program input is never starved, and to allow cutter compensation
to have non-XY moves inserted while cutter compensation is on.
Memory Lock Key Switch This is an option that prevents
the operator from editing or deleting programs, and from altering
settings. Since the key switch (if installed) locks the settings,
it also allows you to lock other areas within the settings.
Setting 7 locks parameters; Parameters 57, 209, and 278 lock other
features. Setting 8 locks all programs. Setting 23 locks 09xxx
programs. Setting 119 locks offsets. Setting 120 locks macro
variables. In order to edit or change these areas, the key switch
(if installed) must be unlocked and the setting turned off. (Any
Mill Control ver. 9.25 and above; any Lathe Control ver. 2.23 and
above)
Rapid an Axis Home You can rapid all axes to machine zero
by pressing the HOME G28 key.
You can also send just one axis (X, Y, Z, A or B) to machine zero
in rapid motion: Enter the letter X, Y, Z, A or B, then press HOME
G28, and that axis alone will rapid home. There is no warning to
alert you of any possible collision! Care must be exercised. (Any
Mill Control ver. 9.49 and above; any Lathe Control ver. 2.24 and
above)
Search for a Program Command Searching for a specific
command in a program can be done in either MEM or EDIT mode. Just
enter the letter code, with or without a specified value (A or
A1.23), and press the up or down cursor arrow. If you enter just
the letter, the search will stop at the next use of that letter,
regardless of its assigned value.
Search for a Program When in EDIT or MEM mode, you can
quickly select and display another program by simply entering the
program number (Onnnnn) and pressing either the cursor down arrow
or F4.
 TOOL OFFSET MEASURE and PART ZERO SET
Use these keys to
enter either a tool length offset or a work offset, to help save
time during part setup. The NEXT TOOL key is then used to send the
machine home for a tool change to the next tool. The cursor will
then move to the next offset register, and the increment for the
handle will go back to 10.0 inches per minute.
Rotate Tool Carousel You can rotate the tool carousel
without changing tools by using M39 and Tnn. This can be used to
recover from some unusual conditions. However, it will also tell
the control that there is a different tool in the spindle, which
may not be the case. You can disable this command by turning on
Setting 86 (M39 Lockout). (Any Mill Control ver. 2.3 and above)
Tool Change Command It is not necessary to turn off the
coolant, stop the spindle, or move the Z axis prior to a tool
change (M06). The control will do this for you. When the Haas CNC
reads M06, it will:
1) retract the Z axis to the tool change position;
2) stop the spindle;
3) orient the spindle;
4) turn off the coolant; and
5) change the tool
Transferring an MDI Program You can transfer and save a
program from MDI to your list of programs. When in the MDI
display, make sure that the cursor is at the beginning of the MDI
program. Enter a program number (Onnnnn) thats not being used.
Then press ALTER, and this will transfer the MDI data into your
list of programs under that program number.
|
|
Run-Stop-Jog-Continue (RSJC)
This feature allows the operator to interrupt
program execution, jog away from the part to
perform a desired task, and then return to the
interruption point and resume program execution.
Once RSJC is initiated, the operator is able to
stop and start the spindle, jog the XYZ axes
individually (axes other than X, Y, and Z cannot
be jogged), or command a tool release. The
following describes the RSJC procedure. (Any
Mill Control ver. 11.10 and above)
1) While a program is running, press FEED HOLD.
This will stop all motion (after any canned
cycle in process has been completed).
2) Press X, Y or Z followed by the HANDLE JOG
key. The control will store the current X, Y or
Z position. (Axes other than X, Y, and Z cannot
be jogged.)
3) At this point, the control will display the
message JOG AWAY, and will tick once each second
or so. The operator can use the jog handle,
remote jog handle, the HANDLE JOG increment
buttons (.0001/.1, .001/1., .01/10., .1/100.) or
the JOG LOCK buttons to move the tool away from
the part.
a) Now you can use the COOLNT key to cycle the
coolant, and CW, CCW, STOP to operate the
spindle. You can also use the TOOL RELEASE
button, and turn Through-Spindle Coolant (TSC)
on and off using the AUX CLNT key (note: use of
this key requires that the spindle be rotating
and the door closed).
b) At this point tools can be swapped out and
the associated length and diameter offsets
adjusted. However, when the program is
continued, the old offsets will still be used
for the return position and for any motion
commands already in the queue. It is therefore
unsafe to swap out tools and adjust offsets when
the program is interrupted during a cut.
4) When youre ready to continue, jog to a
position as close as possible to the stored
position, or to a point where there will be an
unobstructed rapid path back to the stored
position.
5) Return to the previous mode by pressing MEM
or MDI/DNC. The control will only continue
normally if the mode that was in effect at the
time of the interruption is re-entered.
6) Press CYCLE START. The control will display
the message JOG RETURN and rapid X and Y at 5%
to the position where FEED HOLD was pressed;
then it will do the same for Z. The rapid rate
override keys have no effect during JOG RETURN.
a) Note that the control will not follow the
path the operator used to jog away. Instead, it
will perform simple moves without regard for
obstacles; therefore, a crash is possible.
b) If FEED HOLD is pressed during this motion,
the control will go into a feed hold state and
display the message JOG RETURN HOLD. Pressing
CYCLE START will cause the control to resume the
JOG RETURN motion. When the motion is completed,
the control will again go into a feed hold
state.
|
|
|
|
|
|
|
|
|
|
|
