Tool call

Tool call by TOOL CALL

Application

The TOOL CALL function calls a tool in the NC program. When the tool is in the tool magazine, the control inserts the tool into the spindle. When the tool is not in the magazine, you can insert it by hand.

Requirement

  • Tool defined
  • To call a tool, the tool must be defined in the tool management.

    Tool management

Description of function

Upon calling a tool, the control reads the associated row from the tool management. The tool data are visible on the Tool tab of the Status workspace.

Tool tab

 
Tip

HEIDENHAIN recommends switching the spindle on with M3 or M4 after every tool call. That way you avoid problems during program run, such as when restarting after an interruption.

Overview of miscellaneous functions

Input

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

  • Change the following contents as needed:
  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions, e.g. with M91
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

11 TOOL CALL 4 .1 Z S10000 F750 DL+0,2 DR+0,2 DR2+0,2

; Call the tool

The NC function includes the following syntax elements:

Syntax element

Meaning

TOOL CALL

Syntax initiator for a tool call

4, QS4 or "MILL_D8_ROUGH"

Tool definition as a fixed or variable number or name

 
Tip

Only the tool definition as a number is unique because the tool names of several tools may be identical!

Syntax element depending on technology or application

Selection by means of a selection window

Technology-dependent differences when calling tools

.1

Step index of the tool

Optional syntax element

Indexed tool

Z

Tool axis

By default, tool axis Z is used. Other possibilities might be available, depending on the machine.

Syntax element depending on technology or application

Technology-dependent differences when calling tools

S or S( VC = )

Spindle speed or cutting speed

Optional syntax element

Spindle speed S

F, FZ or FU

Feed rate

Alternative feed specifications: feed per tooth or feed per revolution

Optional syntax element

Feed rate F

DL

Delta value of tool length

Optional syntax element

Tool compensation for tool length and radius

DR

Delta value of the tool radius

Optional syntax element

Tool compensation for tool length and radius

DR2

Delta value of the tool radius 2

Optional syntax element

Tool compensation for tool length and radius

Technology-dependent differences when calling tools

Milling cutter tool call
  • The following tool data of a milling cutter can be defined:
  • Fixed or variable number or name of tool
  • Step index of the tool
  • Tool axis
  • Spindle speed
  • Feed rate
  • DL
  • DR
  • DR2

Calling a milling cutter requires the number or the name of the tool, the tool axis and the spindle speed.

Tool table tool.t

Tool call of a turning tool (option 50)
  • The following tool data of a turning tool can be defined:
  • Fixed or variable number or name of tool
  • Step index of the tool
  • Feed rate

Calling a turning tool requires the number or the name of the tool.

Turning tool table toolturn.trn (option 50)

Tool call of a grinding tool(option 156)
  • The following tool data of a grinding tool can be defined:
  • Fixed or variable number or name of tool
  • Step index of the tool
  • Tool axis
  • Spindle speed
  • Feed rate

Calling a grinding tool requires the number or the name of the tool and the tool axis.

Grinding tool table toolgrind.grd (option 156)

Tool call of a workpiece touch probe (option 17)
  • The following tool data of a workpiece touch probe can be defined:
  • Fixed or variable number or name of tool
  • Step index of the tool
  • Tool axis

Calling a workpiece touch probe requires the number or the name of the tool and the tool axis!

Touch probe table tchprobe.tp

Updating tool data

A TOOL CALL allows updating the data of the active tool even without tool change, e. g. change the cutting data or delta values. The tool data that can be changed depend on the technology.

  • In the cases below, the control updates only the data of the active tool:
  • Without tool number or tool name and without tool axis
  • Without tool number or tool name and with the same tool axis as in the previous tool call
 
Tip

When a tool number or a tool name or a changed tool axis is programmed in the TOOL CALL data record, the control runs a tool change macro.

This may cause the control to insert a replacement tool because the service life has expired.

Automatically inserting a replacement tool with M101

Notes

  • The machine manufacturer uses the machine parameter allowToolDefCall (no. 118705) to specify whether a tool can be defined by its name, its number or both in the TOOL CALL and TOOL DEF functions.
  • Tool pre-selection by TOOL DEF

  • The machine manufacturer uses the optional machine parameter progToolCallDL (no. 124501) to define whether the control will consider delta values from a tool call in the Positions workspace.
  • Tool compensation for tool length and radius

    Positions workspace

Cutting data

Application

The cutting data consist of spindle speed S or alternatively constant cutting speed VC and feed rate F.

8H000_06

Description of function

Spindle speed S

Effect

The spindle speed or the cutting speed is effective until a new spindle speed or cutting speed is defined in a TOOL CALL data block.

Potentiometer

The speed potentiometer allows varying the spindle speed between 0 % and 150 % while the program is running. The speed potentiometer setting is effective only for machines with infinitely variable spindle drive. The maximum spindle speed depends on the machine.

Potentiometers

Status displays
  • The control displays the current spindle speed in the following workspaces:
  • Positions workspace
  • Positions workspace

  • POS tab of the Status workspace
  • POS tab

Feed rate F

The linear axes feed rate is defined in millimeters per minute (mm/min).

The rotary axes feed rate is defined in degrees per minute (°/min).

The feed rate can be defined with an accuracy of three decimal places.

  • Alternatively, the feed rate can be defined in the NC program or in a tool call in the following units:
  • Feed rate per tooth FZ in mm/tooth
  • FZ defines the path in millimeters that the tool covers per tooth.

     
    Tip

    When using FZ, the number of teeth must be defined in the CUT column of the tool management.

    Tool management

  • Feed rate per revolution FU in mm/rev
  • FU defines the path in millimeters that the tool covers per spindle revolution.

    The feed rate per revolution is used above all when turning (option 50).

    Feed rate

The feed rate defined in a TOOL CALL can be called up within the NC program, using F AUTO.

F AUTO

The feed rate defined in the NC program is effective up to the NC block in which a new feed rate is programmed.

F MAX

When defining F MAX, the control moves at rapid traverse. F MAX is effective only in the block where it is called. Starting with the following NC block, the last defined feed rate is effective. The maximum feed rate depends on the machine and may depend on the axis.

Feed rate limit F MAX

F AUTO

When defining a feed rate in a TOOL CALL block, this feed rate can be used in the following positioning blocks, using F AUTO.

Button F of the Manual operation application
  • If you enter F=0, then the feed rate that the machine manufacturer has defined as minimum feed rate is effective
  • If the feed rate entered exceeds the maximum value that has been defined by the machine manufacturer, then the value defined by the machine manufacturer is effective
  • Manual operation application

Potentiometer

The feed rate potentiometer allows varying the feed rate between 0 % and 150 % while the program is running. The setting of the feed rate potentiometer is effective only for the programmed feed rate. As long as the programmed feed rate has not yet been reached, the feed rate potentiometer has no effect.

Potentiometers

Status displays
  • The control displays the current feed rate in mm/min in the following workspaces:
  • Positions workspace
  • Positions workspace

  • POS tab of the Status workspace
  •  
    Tip

    In the Manual operation application, the control displays the feed rate including the decimal points on the POS tab. The control displays the feed rate with a total of six decimal points.

    POS tab

  • The control displays the feed rate.
    • When 3D ROT is active the machining feed rate is shown if several axes are moved
    • If 3-D ROT is inactive, the feed rate display remains empty when more than one axis is moved simultaneously

    3-D rotation window (option 8)

Notes

  • In inch programs, the feed rate must be defined in 1/10 inch/min.
  • To move your machine at rapid traverse, you can also program the corresponding numerical value, e.g. F30000. Unlike FMAX, this rapid traverse remains in effect not only in the individual block but in all blocks until you program a new feed rate.
  • When moving an axis, the control checks whether the defined rotational speed has been reached. The control does not check the rotational speed in positioning blocks with FMAX as feed rate.

Tool pre-selection by TOOL DEF

Application

Using TOOL DEF, the control prepares a tool in the magazine, thus reducing the tool change time.

 
Machine

Refer to your machine manual.

The preselection of tools with TOOL DEF can vary depending on the individual machine tool.

Description of function

If your machine is equipped with a chaotic tool changer system and a double gripper, you can perform tool pre-selection. To do this, program the TOOL DEF function after a TOOL CALL data record and select the tool to be used next in the NC program. The control prepares the tool while the program is running.

Input

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

  • Change the following contents as needed:
  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions, e.g. with M91
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

11 TOOL DEF 2 .1

; Tool pre-selection

The NC function includes the following syntax elements:

Syntax element

Meaning

TOOL DEF

Syntax initiator for tool pre-selection

2, QS2 or "MILL_D4_ROUGH"

Tool definition as a fixed or variable number or name

 
Tip

Only the tool definition as a number is unique because the tool names of several tools may be identical!

.1

Step index of the tool

Indexed tool

Optional syntax element

This function can be used for all technologies except for dressing tools (option 156).

Application example

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

  • Change the following contents as needed:
  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions, e.g. with M91
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

11 TOOL CALL 5 Z S2000

; Call the tool

12 TOOL DEF 7

; Pre-select the next tool

* - ...

21 TOOL CALL 7

; Call the pre-selected tool