Classic Haas Control (CHC) - Advanced Tool Management - Mill


Advanced Tool Management Introduction

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 used in each tool group and compares it to your defined limits. When a tool reaches a limit (e.g. number of times used, or tool load), 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 flashes orange and the tool life screen automatically displays.

The ATM page is located in the Current Commands mode. Press [CURRENT COMMANDS], and then [PAGE UP] until you see the ATM screen.
While on the ATM page, press [F4] to navigate between the three windows. Use the cursor arrows to navigate within the these windows. 
  1. Tool group window
  2. Allowed limits window
  3. Tool data window


Tool Group Window Explained

The Tool Group Window defines the tool groups used in the programs.


  • Previous – Highlight <PREVIOUS> and press [ENTER] to change the display to the previous group.
  • Next – Highlight <NEXT> and press [ENTER] to change the display to next group.
  • Add – Highlight <ADD>, enter a number between 1000 and 2999, and press [ENTER] to add a tool group.
  • Delete – Use <PREVIOUS> or <NEXT> to scroll to the group to delete. Highlight <DELETE> and press [ENTER]. Confirm the deletion; answering [Y] completes the deletion; answering [N] cancels the deletion.
  • Rename - Highlight <RENAME>, enter a number 1000 and 2999 and press [ENTER] to renumber the group ID.
  • Search - To search for a group, highlight <SEARCH>, enter a group number and press [ENTER].
  • Group Id – Displays the group ID number.
  • Group Usage – Enter the order in which the tools in the group are called. Use the left and right cursor keys to select how the tools are used.
  • Description – Enter a descriptive name of the tool group.

Allowed Limits Window Explained

The Allowed Limits window contains the user-defined limits to determine when a tool is worn out. These variables affect every tool in the group. The control ignores any variable set to zero.


  • Feed Time – Enter the total amount of time, in minutes, a tool is used in a feed.
  • Total Time – Enter the total time, in minutes, a tool is used.
  • Tool Usage – Enter the total times a tool is used (number of tool changes).
  • Holes – Enter the total number of holes a tool is allowed to drill.
  • Tool Load – Enter the maximum tool load (in percent) for the tools in the group.
  • TL Action – Enter the automatic action to be taken when the maximum tool load percentage is reached. Use the left and right cursor keys to select the automatic action.

Tool Data Window Explained

The Tool Data Window is used to establish the tools within a tool group. 


  • Tool# – Used to add or remove a tool from a group.  Use the cursor keys to highlight any of the areas under the Tool heading and enter a tool number. You can type zero to clear the tool, or highlight the tool number and press [ORIGIN] to reset the H-Code, D-Code, and Flutes data to the default values.
  • EXP (Expire) – Used to manually obsolete a tool in the group. To obsolete a tool, press [*] ([SHIFT], then [1]). To remove an obsolete tool (indicated with an asterisk), press [ENTER]. 
  • Life – The percentage of life left in a tool. This is calculated by the CNC control, using actual tool data and the limits the operator entered for the group.
  • CRNT PKT – The tool changer pocket that contains the highlighted tool.
  • H-Code (Tool Length) – You cannot edit the H-code unless Setting 15 is set to OFF. To change an H-code (if allowed), type a number and press [ENTER]. The number entered corresponds to the tool number in the tool offsets display.
  • D-Code (Tool Diameter) – To change a D-code, type a number and press [ENTER]. By default, the H and D-codes in Advanced Tool Management are set to equal the tool number that is added to the group.
  • Flutes – The number of flutes on the tool. To edit this, type a new number and press [ENTER]. This is the same as the Flutes column listed on the tool offsets page.
  • Load – The maximum load, in percent, exerted on the tool.
  • Holes – The number of holes that the tool has drilled/ tapped/ bored using Group 9 canned cycles. 
  • Feed Time – The amount of time, in minutes, that the tool has been in a feed.
  • Total Time – The total amount of time, in minutes, that the tool has been used.
  • Usage – The number of times the tool has been used.

NOTE: Highlight the Holes or Load field, and then press [ORIGIN] to clear their values. To change the values, highlight the value you want to change, type a new number, and press [ENTER].

Tool Group Setup

Setup a tool group:
  1. Press [F4] until the Tool Group window is highlighted.
  2. Use the cursor keys to highlight <ADD>.
  3. Type a group ID number between 1000 and 2999.
  4. Press [ENTER].
  5. Press [F4] until the Allowed Limits window is highlighted.
  6. Enter the tool life limit you wish the use.  
  7. Highlight the the limit type you want to set for the group.
  8. Type the limit and press [ENTER].
  9. Press [F4] until the Tool Data window is outlined.
  10. Highlight the <Tool#> column to add tools to the group.
  11. Type the tool number you want to add to the group and press [ENTER].
  12. Repeat steps 10 and 11 to add more tools to the group.

Tool Group Usage

You must set up a tool group before you run a program with ATM. To use a tool group in a program:
1. Set up a tool group.
2. 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 new programming format. 

%
O30001 ;
(Tool 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 ;
(T1000 COMPLETION BLOCKS) ;
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 Macros

Advanced Tool Management 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 will expire tool 1 and it will no longer be used)
8001 = 0 (if tool 1 was expired manually or with a macro, then setting macro 8001 to 0 will make tool 1 available again for use)

Macro variables 8500-8515 enable a G-code program to get information about a tool group.
Start by specifying a tool group ID number with macro 8500. Once the the tool group is specified the control will then return the  information on the tool group in macro variables #8501 through #8515.

Macro Address Description
#8500 Advanced Tool Management (ATM). Group ID
#8501 ATM. Percent of available tool life of all tools in the group.
#8502 ATM. Total available tool usage count in the group.
#8503 ATM. Total available tool hole count in the group.
#8504 ATM. Total available tool feed time (in seconds) in the group.
#8505 ATM. Total available tool total time (in seconds) in the group.
#8510 ATM. Next tool number to be used.
#8511 ATM. Percent of available tool life of the next tool.
#8512 ATM. Available usage count of the next tool.
#8513 ATM. Available hole count of the next tool.
#8514 ATM. Available feed time of the next tool (in seconds).
#8515 ATM. Available total time of the next tool (in seconds).


Macro variables #8550-#8564 enable a G-code program to get information about individual tools.

Start by specifying an individual tool ID number with macro 8550. Once specified the control returns the individual tool information in macro variables #8551-#8564.

Additionally, you can specify an ATM group number using macro 8550. In this case, the control will return the individual tool information for the current tool in the specified ATM tool group using macro variables 8551-8564. 

Macro Address Description
#8550 Individual tool ID
#8551 Number of Flutes of tools
#8552 Maximum recorded vibrations
#8553 Tool length offsets
#8554 Tool length wear
#8555 Tool diameter offsets
#8556 Tool diameter wear
#8557 Actual diameter
#8558 Programmable coolant position
#8559 Tool feed timer (seconds)
#8560 Total tool timers (seconds)
#8561 Tool life monitor limit
#8562 Tool life monitor counter
#8563 Tool load monitor maximum load sensed so far
#8564 Tool load monitor limit


The following table shows tool data for individual tool numbers. The first 8 sets provide access for tool data for tools 1-200; the last 6 sets provide data for tools 1-100. 

Macro Address Description Tool Range
#1601-#1800 Number of Flutes 1-200
#1801-#2000 Maximum recorded vibrations 1-200
#2001-#2200 Tool length offsets 1-200
#2201-#2400 Tool length wear 1-200
#2401-#2600 Tool diameter/radius offsets 1-200
#2601-#2800 Tool diameter/radius wear 1-200
#3201-#3400 Actual Diameter 1-200
#3401-#3600 Programmable coolant positions 1-200
#5401-#5500 Tool feed timers (seconds) 1-100
#5501-#5600 600 Total tool timers (seconds) 1-100
#5601-#5699 Tool life monitor limit 1-100
#5701-#5800 Tool life monitor counter 1-100
#5801-#5900 Tool load monitor maximum load sensed so far 1-100
#5901-#6000 Tool load monitor limit 1-100

Refer to the Macros chapter in your Operator's Manual for more details on ATM Macros.

Save and Restore Advanced Tool Management Tables

The control can save and restore the variables associated with the Advanced Tool Management (ATM) feature to the USB drive. These variables hold the data that you enter on the ATM screen. You can then save the information, either as part of an overall backup program or on its own with the [LIST PROGRAM] / Save / Load window. The control creates a file with a .ATM extension to save the data.

To Save the ATM file 
  1. Press [LIST PROGRAM].
  2. Select the <USB DEVICE> tab.
  3. Press [F4] to bring up the <SAVE AND LOAD> window.
  4. Highlight <Save ATM> or <Save All - Back Up>.
  5. Type a file name of your choice.
  6. Press [ENTER].
  7. The control saves the file to the USB device.
To Load the ATM Files
  1. Press [LIST PROGRAM].
  2. Select the <USB DEVICE> tab.
  3. Highlight the .ATM file you wish to load.
  4. Press [F4] to bring up the <SAVE AND LOAD> window.
  5. Highlight to <Load ATM>.
  6. Press [ENTER].
  7. The control loads the ATM data.

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.