Adapting the feed rate for circular paths with M109
Application
With M109 the control maintains a constant feed rate at the cutting edge for internal and external machining on circular paths, for example to produce a uniform milled surface during finishing.
Description of function
Effect
M109 takes effect at the start of the block.
In order to reset M109, program M111.
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.
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 L X+5 Y+25 RL F1000 | ; Approach first contour point at programmed feed rate |
12 CR X+45 Y+25 R+20 DR- M109 | ; Activate feed rate adaptation, then perform the operation on the circular path at the increased feed rate |
In the first NC block the control moves the tool at the programmed feed rate, which refers to the tool center-point path.
In NC block 12 the control activates M109 and maintains a constant feed rate at the tool cutting edge when machining on circular paths. At the beginning of each block the control calculates the feed rate at the tool cutting edge for the respective NC block and adapts the programmed feed rate depending on the contour radius and tool radius. This means that the programmed feed rate is increased for external operations and reduced for internal operations.
The tool then cuts the external contour at an increased feed rate.
Without M109 the tool cuts along the circular path at the programmed feed rate.
Notes
- Do not use M109 for machining very small outside corners (acute angles)
If you define M109 before calling a machining cycle with a number greater than 200, the adjusted feed rate is also active for circular paths within these machining cycles.