Tool compensation for tool length and tool radius
Application
Delta values allow implementing tool compensation of the tool length and the tool radius. Delta values influence the calculated and therefore the active tool dimensions.
The tool length delta value DL is active in the tool axis. The tool radius delta value DR is active exclusively for radius-compensated traverses with the path functions and cycles.
Related topics
- Tool radius compensation
- Tool compensation with compensation tables
Description of function
The control distinguishes between two types of delta values:
- Delta values within the tool table serve for permanent tool compensation that is required (e.g., due to wear).
These delta values can be determined, for example, by using a tool touch probe. The control automatically enters the delta values in the tool management.
- Delta values within a tool call serve for a tool compensation that is active exclusively in the current NC program (e.g., a workpiece oversize).
Delta values represent deviations from the length and radius of a tool.
A positive delta value enlarges the current tool length or the tool radius. The tool then cuts less material during machining (e.g., for a workpiece oversize).
A negative delta value reduces the current tool length or the tool radius. The tool then cuts more material during machining.
For programming delta values in an NC program, define the value within a tool call or by using a compensation table.
Using TOOL CALL to call a tool
Tool compensation with compensation tables
Delta values within a tool call can also be defined by using variables.
Tool length compensation
The control takes the tool length compensation into account as soon as a tool is called. The control performs tool length compensation only on tools of length L>0.
In tool length compensation, the control takes delta values from the tool table and the NC program into account.
Active tool length = L + DLTAB + DLProg
L: | Tool length L from the tool table |
DL TAB: | Tool length delta value DL from the tool table |
DL Prog : | Tool length delta value DL from the tool call or the compensation table The most recently programmed value becomes active. |
- Always define the actual tool length of a tool (not just the difference)
- Use TOOL CALL 0 only to empty the spindle
Tool radius compensation
The control takes the tool radius compensation into account in the following cases:
- If tool radius compensation RR or RL is active
- Within machining cycles
- For straight lines LN with surface normal vectors
In tool radius compensation, the control takes the delta values from the tool table and the NC program into account.
Active tool radius = R + DRTAB + DRProg
R: | |
DR TAB: | Tool radius delta value DR from the tool table |
DR Prog: | Tool radius delta value DR from the tool call or the compensation table The most recently programmed value becomes active. |
Tool data within variables
When executing a tool call, the control calculates all tool-specific values and saves them within variables.
Active tool length and tool radius:
Q parameters | Function |
---|---|
Q108 | ACTIVE TOOL RADIUS |
Q114 | ACTIVE TOOL LENGTH |
After the control has saved the current values within variables, the variables can be used in the NC program.
Application example
You can use the Q parameter Q108 ACTIVE TOOL RADIUS in order to shift the tool center point of the ball-nose cutter to the sphere center using the delta value for the tool length.
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 "BALL_MILL_D4" Z S10000 |
12 TOOL CALL DL-Q108 |
This allows the control to monitor the complete tool for collisions and the dimensions used in the NC program can still be programmed with reference to the ball center.
Notes
- The control shows delta values from the tool management graphically in the simulation. For delta values from the NC program or from compensation tables, the control changes only the position of the tool in the simulation.
- 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.