3D Tool Path Refinement
Most CAM systems have a 3D tool path refinement feature.
1 - Surface without tool path refinement.
2 - Surface with tool path refinement.
Filters and Tolerances
Mastercam's Refine Toolpath screen.
Depending on the type of toolpath or part complexity you may want to use MasterCam's Line/Arc Filtering Settings.
Set the Line/Arc filter to 25% and the Smoothing tolerance to 75%.
Mastercam features several different options to filter a particular tool path.
In general, try to set the cut tolerance between 0.0002” and 0.0005”. This may be different on different types of materials and cutters.
This option allows you to create tight linear segments on a 3D model and then convert them to arc segments when you post the G-code. This results in smoother transitions and a better surface finish.
Third-party filters, like this software from Cimco, take the G-code created in your CAM system and convert the linear segments to arc segments. This produces smoother transitions and a better surface finish.
This software is useful for CAM systems that do not have an internal arc filter.
Setting 191, DEFAULT SMOOTHNESS alters the feed acceleration parameters.
- Medium = default acceleration and corner rounding values.
- Rough = double the default acceleration and corner rounding values (shorter cycle times).
- Finish = half the default acceleration and corner rounding values (longer cycle time).
DEFAULT SMOOTHNESS Values can be overridden in the program with a G187 Px where:
- P1 = Rough
- P2 = Medium (default)
- P3 = Finish
Use G187 P1 to speed up roughing operations, leave stock, some corner rounding is possible.
Use G187 P3 to smooth out finishing operations.
Parameter786 , COMMAND FIR FILTER ORDER
The COMMAND FIR FILTER ORDER parameter for each axis provides smoothing at the start and finish of each acceleration/deceleration cycle.
If the machine has Sigma V motors, the FIR COMMAND ORDER paramter for each axis must be set to 64.
Most machines have had their natural frequency mapped, and parameters established.
The notch filter monitors the machine's commanded motion.
If a machine is about to execute a move that is near its natural frequecy, the notch filter will slightly alter the speed to avoid vibrations.
Use the features in the CAM system to get the best surface finish.
Test different tool paths with different cut tolerance and smoothness settings in a block of material.
Record the techniques that work best for your part style and CAM system for future use.