Haas Mill User Manual

76
Quick Code
96-8000 rev R June 2007
Call Tool 1
1. While on the “Start Up Commands” menu, turn the jog handle CCW to highlight the group item titled “Call Tool.
2. Press the Write button to have the control ask you for a tool number for your program, and the control will be
flashing with a 1 in the lower left corner as the default value. Press Write to accept the number 1.
3. Highlight the group item titled “Tool Start Up Commands”.
4. Press the Write key to have the control ask you for the commands to define the start up of tool 1, and enter into
your program.
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..
O00005 ;
(PROGRAM NAME) ;
T1 M06 (T) ;
G90G54G00X0Y0;
S750 M03 ;
G43 H01 Z1. M08 ;
QUICKCODE (EDIT) O00005 N00000
QUICKCODE
Programmed with the Start Up Command Selections Entered in with Quick Code for Tool 1.
For this example, the material is aluminum and that the work coordinate zero for G54 is at the center of the
bolthole pattern.
Invoke the Spot Drilling Canned Cycle G82
1. Scroll and highlight the group titled “4. Drill/Tap/Bore Cycles”.
2. Scroll CCW two clicks. “Drill with Dwell G82” will be highlighted.
3. Press the Write button to start the prompts.
Note that Quick Code defined a block of code to execute a spot drill cycle at that present location. More X and Y
drill cycle locations can be added, if needed, by selecting “6. Drill/Tap/Bore Locations”.
Note: The part does not have a hole drilled at X0 Y0, which is the center of the bolthole circle; manually enter an L0
on the end of the G82 command line. This will ignore the G82 canned cycle until the next location.
The program will look like this:
QUICKCODE (EDIT) O00005 N00000
QUICKCODE
3. DRILL/TAP/BORE CYCLES...
Drill G81..
Deep Hole Peck Drill G83..
High Speed Peck Drill G73..
H.S.P.D. W/Return R plane G73..
Bore IN Bore OUT G85..
Bore IN Rapid OUT G86..
Bore IN Shift Rapid OUT G76..
Right Hand Tapping G84..
G80 CANCEL Canned Cycle..
Drill with Dwell G82..
O00005 ;
(PROGRAM NAME) ;
T1 M06 (T) ;
G90 G54 G00 X0 Y0 ;
S750 M03 ;
G43 H01 Z1. M08 ;
G82 G99 Z-0.109 P0.2 R0.1 F5. ;
Program with Spot Drilling Invoked.

Haas Mill Specifications

General

Travels X Axis	Varies by model
Travels Y Axis	Varies by model
Travels Z Axis	Varies by model
Spindle Speed	Varies by model
Spindle Motor	Varies by model
Table Size	Varies by model
Rapid Traverse Rates	Varies by model
Tool Capacity	Varies by model
Max Cutting Rate	Varies by model
Spindle Taper	Varies by model