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.
Related topics
- Automatic tool change with M101
- Tool table tool.t
- Pocket table tool_p.tch
Requirement
- Tool defined
To call a tool, the tool must be defined in the 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.
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.
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. | |
Open the 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.
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 |
.1 | |
Z | Tool axis By default, tool axis Z. Other possibilities might be available, depending on the machine. Syntax element depending on technology or application |
S or S( VC = ) | Spindle speed or cutting speed Optional syntax element Selection by means of a selection window |
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 |
DL | |
DR | Delta value of the tool radius Optional syntax element |
DR2 | Delta value of the tool radius 2 Optional syntax element |
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 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!
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
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.
Notes
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.
- 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.
- 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.