Using TOOL CALL to call a tool

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 is displayed on the Tool tab of the Status workspace.

The 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

Icons

The NC function TOOL CALL offers the following icons:

Icon

Meaning

Open selection window for tools

In the Tool management application, switch to the selected tool

You can change the tool as needed.

Tool management

Open the Cutting data calculator

Cutting data calculator

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

To navigate to this function:

Insert NC function All functions Tools TOOL CALL

The NC function includes the following syntax elements:

Syntax element

Meaning

TOOL CALL

Syntax initiator for a tool call

Number, Name or Parameter

Number or name of the tool

Number, text, or variable

 
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

Input

Z

Tool axis

By default, tool axis Z. 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

Selection by means of a selection window

Spindle speed S

F, FZ or FU

Feed rate

Alternative feed specifications: feed per tooth or feed per revolution

Optional syntax element

Selection by means of a selection window

Feed rate F

DL

Delta value of tool length

Optional syntax element

Tool compensation for tool length and tool radius

DR

Delta value of the tool radius

Optional syntax element

Tool compensation for tool length and tool radius

DR2

Delta value of the tool radius 2

Optional syntax element

Tool compensation for tool length and tool radius

Technology-dependent differences when calling tools

Milling cutter tool call

The following tool data of a milling cutter can be defined:

  • Number or name of the 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 for a workpiece touch probe (#17 / #1-05-1)

The following parameters of a workpiece touch probe can be defined:

  • Number or name of the 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 (#17 / #1-05-1)

Updating parameters

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

In the cases below, the control updates the parameters of only 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 tool call, 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

 
Machine

The control’s full range of functions is available only if the Z tool axis is used (e.g., PATTERN DEF).

Restricted use of the tool axes X and Y is possible when prepared and configured by the machine manufacturer.