Haas Automation VF Series, Книга управления

Страница: 75 / 127

68
January 2004
QUICKCODE (EDIT) O00005 N00000
QUICKCODE
END OF BLOCK
START UP COMMANDS...
Program Name..
Set Machine Defaults..
Sequence Comment..
Call Tool..
Done--Choose an Operation..
------------------------------------------------------
1. MACHINE MOVES...
2. CUTTER COMP. MOVES...
3. DRILL /TAP/BORE CYCLES...
Tool Start Up Commands..
EXAMPLE: G90 G54 G00 X0. Y0.
. . . . S750 M03
. . . . G43 H01 Z1. M08
ENTER fixture offset, x y location,
Spindle Speed and Z start position.
O00005 ;
(PROGRAM NAME) ;
T1 M06 (T) ;
G90 G54 G00 X0 Y0 ;
S750 M03 ;
G43 H01 Z1. M08
;
Programmed with the Start Up Command selections entered in with Quick Code for tool 1.
Remember that after pressing WRITE you can always edit the program to make minor adjustments to code
that Quick Code inserts into your program. You do not have to leave the Quick Code display to do this. But you
must remember to reposition the cursor back to the block where you want to add the next item. Quick Code
will automatically seek the end of the current block that the cursor is on, so there is no need to cursor to the
end of the block.
We will assume that the material is aluminum and that the work coordinate zero for G54 is at the center of the
bolt hole pattern. The Quick Code source file (O9999) was created with a common program format and menu
selections. You could have a different Quick Code source file (O09998 or O09997) for different menu selections
and formats. By changing parameter 228 (to 9998 or 9997) you can quickly change the file that Quick Code
works with if you had created one.
- INVOKE THE SPOT DRILLING CANNED CYCLE G82
1. JHCW and highlight the group titled 4. DRILL/TAP/BORE CYCLES.
2. JHCCW two clicks. DRILL with Dwell G82 will be highlighted.
3. Press the WRITE key to have the control query you, and answer the questions, to set up drilling
with G82.
Note that Quick Code defined a block of code to execute a spot drill cycle at that present location. You can
add more X and Y drill cycle locations if needed by selecting 6. DRILL/TAP/BORE LOCATIONS .
Note: We do not want to drill a hole at X0 Y0, which is the center of the bolt hole circle, so manually edit in an
L0 on the end of the G82 command line. This will ignore the G82 canned cycle until the next location.
Your program will look like this.