The control can capture and save an image of the current screen to an attached USB device or the User Data memory.

Enter a filename if desired. If no filename is entered, the system will use the default filename (see note).

Press SHIFT.

Press F1.

NOTE: The control uses the default filename snapshot#.png. The # starts from 0 and increments each time you capture a screen. This counter resets at power off. Screen captures that you take after a power cycle overwrite previous screen captures that have the same filename on the User Data memory.

Result: 

The control saves the screen capture to your USB device or control memory. The message Snapshot saved to USB or Snapshot saved to User Data appears when the process finishes.

The control can generate an error report that saves the state of the machine that is used for analysis. This is useful when helping the HFO troubleshoot an intermittent problem.

1. Press SHIFT.
2. Press F3.

NOTE: Be sure to always generate the error report with the alarm or the error is active.

Result: 

The control saves the error report to your USB device or control memory.The error report is a zip file that includes a screen capture, the active program, and other information used for diagnostics. Generate this error report when an error or an alarm occurs. E-mail the error report to your local Haas Factory Outlet.

You can use this function to quickly find code in a program.

NOTE: This is a quick-search function that finds the first match in the search direction that you specify. You can use the Editor for a more full-featured search. Refer to Chapter 6.5 for more information on the Editor search function.

NOTE: This is a quick-search function that finds the first match in the search direction that you specify. You can use the Editor for a more full-featured search. Refer to The Search Menu for more information on the Editor search function.

1. Type the text you want to find in the active program.
2. Press the UP or DOWN cursor arrow key.

Result: 

The UP cursor arrow key searches from the cursor position to the start of the program. The DOWN cursor arrow key searches to the end of the program. The control highlights the first match.

NOTE: Putting your search term within parentheses (), will search only within comment lines.

The purpose of Safe Run is to reduce damage to the machine in the event of a crash. It does not prevent crashes, but it raises an alarm sooner and backs off from the crash location.

NOTE: The Safe Run feature is available starting in software version 100.19.000.1300.

 NOTE: If the machine is equipped with a spindle head accelerometer, and when safe mode is enabled and active (ie. during rapids), the accelerometer alarm behavior will be suppressed so the machine can do the normal back off behavior, then the 9941 Alarm will generate.  The G force value will still be recorded at the time of the event.

Safe Run Supported Machines

• VF-1 through VF-5
• VM-2/3
• UMC-500/750/1000
• All DM’s
• All DT’s
• All TM’s
• ST-10 through ST-35

Common causes for crashes are:

• Incorrect tool offsets.
• Incorrect work offsets.
• Wrong tool in the spindle.

NOTE: The Safe Run feature will only detect a crash in handle jog and rapid (G00), it will not detect a crash in a feed move.

Safe Run does the following:

• Slow down the speed of the motion.
• Increases the position error sensitivity.
• When a crash is detected, the control will immediately reverse the axis by a small amount. This will prevent the motor from continuing to drive into the object it has crashed into as well as relieve pressure from the crash itself. After Safe Run has detected a crash, you should be able to easily fit a piece off paper between the two surfaces that crashed.

NOTE: Safe Run is intended for running a program for the first time after writing or changing it. Is it not recommended to run a reliable program with Safe Run, as it increases cycle time significantly. The tool may break and the work piece may still be damaged in a crash.

Safe Run is active during jogging as well. Safe Run can be used during job setup to protect against accidental crashes due to operator error.

This feature lets you stop a running program, jog away from the part, and then start the program again.

1. Press FEED HOLD.
   
   Axis motion stops. The spindle continues to turn.
   
   
2. Press X, Y, Z, or an installed Rotary Axis (A for A Axis, B for B Axis, and C for C Axis), then press HANDLE JOG. The control stores the current X, Y, Z, and rotary axes positions.
3. The control gives the message Jog Away and displays the Jog Away icon. Use the jog handle or jog keys to move the tool away from the part. You can start or stop the spindle with FWD, REV, or STOP. You can command optional Through Spindle Coolant on and off with the AUX CLNT key (you must stop the spindle first). Command optional Through Tool Air Blast on and off with SHIFT + AUX CLNT keys. Command Coolant on and off with the COOLANT key. Command the Auto Air Gun / Minimum Quantity Lubrication options with SHIFT + COOLANT keys. You can also release the tool to change inserts.
   
   CAUTION: When you start the program again, the control uses the previous offsets for the return position. Therefore, it is unsafe and not recommended to change tools and offsets when you interrupt a program.
   
   
4. Jog to a position as close as possible to the stored position, or to a position where there is an unobstructed rapid path back to the stored position.
   
   
5. Press MEMORY or MDI to return to run mode. The control gives the message Jog Return and displays the Jog Return icon. The control continues only if you return to the mode that was in effect when you stopped the program.
   
   
6. Press CYCLE START. The control rapids X, Y, and rotary axes at 5% to the position where you pressed FEED HOLD. It then returns the Z Axis. If you press FEED HOLD during this motion, axis motion pauses and the control gives the message Jog Return Hold. Press CYCLE START to resume the Jog Return motion. The control goes into a feed hold state again when the motion is finished.
   
   CAUTION: The control does not follow the same path that you used to jog away.
   
   
7. Press CYCLE START again and the program resumes operation.
   
   CAUTION: If Setting 36 is ON, the control scans the program to make sure the machine is in the correct state (tools, offsets, G- and M-codes, etc.) to safely continue the program. If Setting 36 is OFF, the control does not scan the program. This can save time, but it could cause a crash in an unproven program.

A safe way to troubleshoot a program is to press GRAPHICS to run it in graphics mode. No movement occurs on the machine, instead the movement is illustrated on the screen.

5) Tool Path Window The large window in the center of the display gives a simulated view of the work area. It displays a cutting tool icon and simulated tool paths.

NOTE: Feed motion appears as a black line. Rapid moves appear as a green line. Drill cycle locations appear with an X.

NOTE: If Setting 253 is ON, the tool diameter is shown as a thin line. If it is OFF, the tool diameter specified in the Tool Offsets Diameter Geometry table is used.

6) Zoom Press F2 to display a rectangle (zoom window) that shows the area that the zoom operation will move to. Use PAGE DOWN to decrease the size of the zoom window (zoom in), and use PAGE UP to increase the size of the zoom window (zoom out). Use the cursor arrow keys to move the zoom window to the location you want to zoom, and press ENTER to complete the zoom. The control scales the tool path window to the zoom window. Run the program again to display the tool path. Press F2 and then HOME to expand the Tool Path window to cover the entire work area.

7) Z-Axis Part Zero Line The horizontal line on the Z-Axis bar at the top-right corner of the graphics screen gives the position of the current Z-axis work offset plus the length of the current tool. While a program simulation runs, the shaded portion of the bar indicates the depth of the simulated Z-Axis motion relative to the Z-Axis work zero position.

8) Position Pane The position pane displays axis locations just as it would during a live part run.

This section describes tool management in the Haas control: commanding tool changes, loading tools into holders, and Advanced Tool Management.

There are several different spindle options for Haas mills. Each of these types requires a specific tool holder. The most common spindles are 40- and 50-taper. 40-taper spindles are divided into two types, BT and CT; these are referred to as BT40 and CT40. The spindle and tool changer in a given machine are capable of holding only one tool type.

Pull Studs:

A pull stud (sometimes called a retention knob) secures the tool holder into the spindle. Pull studs are threaded into the top of the tool holder and are specific to the type of spindle. Refer to the 30, 40, and 50-taper spindle and tooling information on the Haas Service website for descriptions of the pull studs you need.

 CAUTION: Do not use short-shaft or pull studs with a sharp right-angle (90-degree) head; they will not work and will cause serious damager to the spindle.

The Tool Usage tab contains information about the tools used in a program. This display will tell you information about each tool used in a program and statistics about each time it was used. It starts to collect information when user Main program start and clear information when meet codes M99, M299, M199.

Macros Interface

You can use these macros variables to set and collect the tool usage data

This section tells you how to use the tool table to give the control information about your tools.

 NOTE: If your machine has an umbrella-style tool changer, you will not use the tool pocket table.

• Set pocket as heavy [H] [5] - Use this flag when a Heavy, Small Diameter 40-taper tool (4 lb or heavier) or a 50-taper tool (12 lb or heavier) is loaded into the spindle. Scroll to the pocket of interest and press [H] to set the flag.
• Set pocket as XL [X] [6] - Use this flag when two adjacent pockets are each side of the tool are needed. Scroll to the pocket of interest and press [X] to set the flag.
  
   NOTE: This option only appears if your machine is a 50-taper.
  
  
• Clear category [SPACE] [7] - Highlight the desired tool and press [SPACE] to clear the flag.
• Set tool [###] + [ENTER] [8] - Highlight the desired pocket and type in the tool number along with [ENTER] to set the desired tool number.
  
   NOTE: You cannot assign a tool number to more than one pocket. If you enter a tool number that is already defined in the tool pocket table, you see an Invalid tool error.
  
  
• Clear tool [0] + [ENTER] [9] - Highlight the desired pocket and press [0] along with [ENTER] to clear out the tool number.
• Reset table [Origin] [11] - Press [ORIGIN] with the cursor in the center column to use the [ORIGIN] menu. This menu lets you:  

  • Sequence All Pockets - Makes all of the tool numbers sequential based on their pocket location, starting with 1.

  • Zero All Pockets - Removes all of the tool numbers from all of the pocket numbers.
  
  
  • Clear Category Flags - Removes the category designations from all of the tools.

Advanced Tool Management (ATM) lets you set up groups of duplicate tools for the same or a series of jobs.

ATM classifies duplicate or backup tools into specific groups. In your program, you specify a group of tools instead of a single tool. ATM tracks the tool use in each tool group and compares it to your defined limits. When a tool reaches a limit, the control considers it “expired.” The next time your program calls that tool group, the control chooses a non-expired tool from the group.

When a tool expires:

• The beacon will flash.


• ATM puts the expired tool in the EXP group


• Tool groups that contain the tool appear with a red background.

Allowed Limits

This table gives data about all of the current tool groups, including default groups and user-specified groups. ALL is a default group that lists all of the tools in the system. EXP is a default group that lists all of the tools that are expired. The last row in the table shows all of the tools that are not assigned to tool groups. Use the cursor arrow keys or [END] to move the cursor to the row and see these tools.

For each tool group in the ALLOWED LIMITS table, you define limits that determine when a tool expires. The limits apply to all tools assigned to this group. These limits affect every tool in the group.

The columns in the ALLOWED LIMITS table are:

• GROUP - Displays the tool group’s ID number. this is the number you use to specify the tool group in a program.


• EXP # - Tells you how many tools in the group are expired. If you highlight the ALL row, you see a list of all of the expired tools in all groups.


• ORDER - Specifies the tool to use first. If you select ORDERED, ATM uses the tools in tool number order. You can also have ATM automatically use the NEWEST or OLDEST tool in the group.


• USAGE - The maximum number of times the control can use a tool before it expires.


• HOLES - The maximum number of holes a tool is allowed to drill before it expires.


• WARN - The minimum value for tool life remaining in the group before the control gives a warning message.


• LOAD - The allowed load limit for tools in the group before the control does the ACTION that the next column specifies.
  
   WARNING: Load limit should not be used for applications where spindle speed and feed change rapidly. For example, tapping or constant surface speed.
  
  
• ACTION - The automatic action when a tool reaches its maximum tool load percentage. Highlight the tool action box to change and press [ENTER] . Use the [UP] and [DOWN] cursor keys to select the automatic action from the pull down menu ( ALARM, FEEDHOLD, BEEP, AUTOFEED, NEXT TOOL).
  
  
• FEED - The total amount of time, in minutes, that the tool can be in a feed.
  
  
• TOTAL TIME - The total amount of time, in minutes, that the control can use a tool.

Tool Data

This table gives information about each tool in a tool group. To look at a group, highlight it in the ALLOWED LIMITS table, and then press [F4] .

• TOOL# - Shows the tool numbers used in the group.


• LIFE - The percentage of life left in a tool. This is calculated by the CNC control, using actual tool data and the allowed limits the operator entered for the group.


• USAGE - The total number of times that a program has called the tool (number of tool changes).


• HOLES - The number of holes the tool has drilled/ tapped/ bored.


• LOAD - The maximum load, in percent, exerted on the tool. This limit should not be used for applications where spindle speed and feed change rapidly. For example tapping or constant surface speed.
  
  WARNING: Load limit should not be used for applications where spindle speed and feed change rapidly. For example tapping or constant surface speed.
  
  
• LIMIT - The maximum load allowed for the tool


• FEED - The amount of time, in minutes, the tool has been in a feed.


• TOTAL - The total amount of time, in minutes, the tool has been used.


• H-CODE - The tool-length code to use for the tool. You can edit this only if Setting 15 is set to OFF.


• D-CODE - The diameter code to use for the tool.
  
  NOTE: By default, the H- and D-codes in Advanced Tool Management are set to equal the tool number that is added to the group.

To add a tool group: 

1. Select the ALLOWED LIMITS table.
2. Use the cursor arrow keys to highlight an empty row.
3. Type the group identification number (between 1000 and 2999) that you want to use for the new tool group.
4. Press [ENTER].
   

Manage Tools in a Group

To add, change, or delete a tool in a group: 

1. Highlight the group you want to work with in the ALLOWED LIMITS table. 
2. Press [F4] to switch to the TOOL DATA table. 
3. Use the cursor arrow keys to highlight an empty row. 
4. Type an available tool number between 1 and 200. 
5. Press [ENTER]. 
6. To change a tool number assigned to a group, use the cursor keys to highlight the tool number you want to change. 
7. Type a new tool number
    NOTE: You can type 0 if you want to delete the tool from the tool group.
8. Press [ENTER].

To use a tool group in a program, substitute the tool group ID number for the tool number and for the H-codes and D-codes in the program. Refer to this program for an example of the program format.

Example:

    % O30001 (Tool change ex-prog);

    (G54 X0 Y0 is top right corner of part) ;

    (Z0 is on top of the part) ;

    (Group 1000 is a drill) ;(T1000 PREPARATION BLOCKS) ;

    T1000 M06 (Select tool group 1000) ;

    G00 G90 G40 G49 G54 (Safe startup) ;

    X0 Y0 (Rapid to 1st position) ;

    S1000 M03 (Spindle on CW) ;

    G43 H1000 Z0.1 (Tool group offset 1000 on) ;

    M08 (Coolant on) ;

    (T1000 CUTTING BLOCKS) ;

    G83 Z-0.62 F15. R0.1 Q0.175 (Begin G83);

    X1.115 Y-2.75 (2nd hole);

    X3.365 Y-2.87 (3rd hole);

    G80 ;

    G00 Z1. M09 (Rapid retract, coolant off) ;

    G53 G49 Z0 M05 (Z home, spindle off) ;

    M01 (Optional stop) ;

    (T2000 PREPARATION BLOCKS) ;

    T2000 M06 (Select tool group 2000) ;

    G00 G90 G40 G49 G54 (Safe startup) ;

    G00 G54 X0.565 Y-1.875 (Rapid to 4th position) ;

    S2500 M03 (Spindle on CW) ;

    G43 H2000 Z0.1 (Tool group offset 2000 on) ;

    M08 (Coolant on) ;

    (T2000 CUTTING BLOCKS) ;

    G83 Z-0.62 F15. R0.1 Q0.175 (Begin G83);

    X1.115 Y-2.75 (5th hole) ;

    X3.365 Y2.875 (6th hole) ;

    (T2000 COMPLETION BLOCKS) ;

    G00 Z0.1 M09 (Rapid retract, Coolant off) ;

    G53 G49 Z0 M05 (Z home, Spindle off) ;

    G53 Y0 (Y home) ;

    M30 (End program) ;

    %

Advanced Tool Management (ATM) can use macros to obsolete a tool within a tool group. Macros 8001 to 8200 represent tools 1 through 200. You can set one of these macros to 1 to expire a tool. For example:

8001 = 1 (this expires tool 1)

8001 = 0 (this makes tool 1 available)

Macro variables 8500 - 8515 enable a G code program to obtain tool group information. When you specify a tool group ID number with macro 8500, the control returns the tool group information in macro variables #8501 through #8515. Refer to the variables #8500 - #8515 in the Macros chapter for the macro variable data label information.

Macro variables #8550 - #8564 let a G-code program obtain information about individual tools. When you specify an individual tool ID number with macro #8550, the control returns the individual tool information in macro variables #8551 - #8564. You can also specify an ATM group number with macro 8550. In this case, the control returns the individual tool information for the current tool in the specified ATM tool group in macro variables 8551 - 8564. Refer to the description for variables #8550 - #8564 in the Macros chapter. The values in these macros provide data that is also accessible from macros starting at 1601, 1801, 2001, 2201, 2401, 2601, 3201, and 3401 and for macros starting at 5401, 5501, 5601, 5701, 5801, and 5901. These first 8 sets provide access for tool data for tools 1-200; the last 6 sets provide data for tools 1-100. Macros 8551 - 8564 give access to the same data, but for tools 1-200 for all data items.

You can save to USB the variables associated with Advanced Tool Management (ATM).

To save the ATM information:

1. Select the USB device in the Device Manager ([LIST PROGRAM] ).
2. Type a filename on the input line.
3. Press [F4] .
4. Highlight SAVE ATM in the pop-up menu.
5. Press [ENTER] .

You can restore from USB the variables associated with Advanced Tool Management (ATM).

To restore the ATM information:

1. Select the USB device in the Device Manager ([LIST PROGRAM] ).
2. Press [F4] .
3. Highlight LOAD ATM in the pop-up menu.
4. Press [EMERGENCY STOP] .
5. Press [ENTER] .