Automatically inserting a replacement tool with M101
Application
With M101 the control automatically inserts a replacement tool after a specified tool life has expired. The control then continues the machining operation with the replacement tool.
Requirements
- RT column in the tool management
The number of the replacement tool must have been defined in the RT column.
- TIME2 column in the tool management
In the TIME2 column you define the tool life after which the control inserts the replacement tool.
Use only tools with an identical radius as replacement tools. The control does not automatically check the radius of the tool.
If you want the control to check the radius, program M108 after the tool change.
Description of function
Effect
M101 takes effect at the start of the block.
In order to reset M101, program M102.
Application example
Refer to your machine manual.
The function of M101 can vary depending on the individual machine tool.
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 5 Z S3000 | ; Tool call |
12 M101 | ; Activate automatic tool change |
The control exchanges the tools and activates M101 in the next NC block. The TIME2 column of the tool management contains the maximum age for the tool life at the time the tool is called. If, during machining, the current tool age in the column CUR_TIME exceeds this value, the control inserts the replacement tool at a suitable point in the NC program. This exchange takes place after no more than one minute, unless the control has not concluded the active NC block yet. A useful application of this function is for automated programs on unattended machines.
Input
If you define M101, the control continues the dialog and prompts you for BT. With BT you define the number of NC blocks by which the automatic tool change may be delayed (up to 100 blocks). The content of the NC blocks, such as the feed rate or distance moved, influences the time by which the tool change is delayed.
If you do not define BT, the control uses the value 1 or, if applicable, a default value defined by the machine manufacturer.
The value for BT, the tool life verification, and the calculation of the automatic tool change have an influence on the machining time.
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 M101 BT10 | ; Activate automatic tool change after no more than 10 NC blocks |
Notes
- Use M101 only for machining operations without undercuts
- Deactivate the tool change with M102
- If you want to reset the current age of a tool (e.g., after changing the indexable inserts), enter the value 0 in the CUR_TIME column of the tool management.
- For indexed tools, the control does not apply any data from the main tool. You must define a replacement tool (with index, if necessary) in each table row in the tool management. If an indexed tool is worn and therefore disabled, this does not apply to all indices. This means, for example, that the main tool can still be used.
- The higher the value of BT, the smaller will be the effect of an extended program duration through M101. Please note that this will delay the automatic tool change!
Notes on tool change
- The control performs the automatic tool change at a suitable point in the NC program.
- If you do not define a replacement tool in the RT column and call the tool via its tool name, the control will switch to a tool with the same name once the maximum tool age TIME2 has been reached.
- The control cannot perform the automatic tool change at the following points in a program.
- During a machining cycle
- If radius compensation with RR or RL is active
- Directly after an APPR approach function
- Directly before a DEP departure function
- Directly before and after a chamfer with CHF or a rounding with RND
- During a macro
- During a tool change
- Directly after the NC functions TOOL CALL or TOOL DEF
- If the machine manufacturer does not define otherwise, the control moves the tool after the tool change as follows:
- If the target position in the tool axis is below the current position, the tool axis is positioned last.
- If the target position in the tool axis is above the current position, the tool axis is positioned first.
Notes on the input value BT
- To calculate a suitable initial value for BT, use the following formula:
t: average machining time of an NC block in seconds
Round the result up to an integer value. If the calculated result is greater than 100, use the maximum input value of 100.
- In the optional machine parameter M101BlockTolerance (no. 202206) the machine manufacturer defines the standard value for the number of NC blocks by which the automatic tool change may be delayed. This standard value applies if you do not define BT.
Definition
Abbreviation | Definition |
---|---|
BT (block tolerance) | Number of NC blocks by which a tool change may be delayed. |