Filter Settings: Art
Use the Filter Settings Dialog box to optimize the Art toolpath by combining small toolpath
segments into longer ones. This reduces the file size, decreases the part
run-time, and allows the CNC machine to run more efficiently by cutting
longer line segments.
Mastercam Art creates very accurate and large toolpaths, often cutting
complex, shapely surfaces. The toolpath calculation is mathematically
precise which creates small toolpath segments. The segments are often
beyond the CNC machine's accuracy. The goal of filtering is to remove
these small segments and make them as long as possible, without affecting
the quality of the finished part
Accept the filter default settings
and use verification to see if the surface is what you want. If it is
too rough, try reducing the filter cut tolerance. The challenge is to
increase the filter size to as large as possible. However, increasing
the filter too far produces facets or flats in your model verification.
For best results, try increasing the filter cut tolerance until you see
facets in the verification, and then reduce it slightly.
Parameters
Prefilter
Select to reduce the Art model tolerance, before applying the toolpath filter. This function pre-filters the Art model by the value you enter before applying the Cut Tolerance and other filter parameters to the toolpath. Pre-filtering reduces the amount of processing that the filter needs to do, allowing for faster toolpath generation.
Always enter a Prefilter value that is smaller than the filter Cut tolerance. Otherwise, large facets appear in the toolpath, preventing the toolpath from creating a smooth finish.
Cut tolerance
Determines the accuracy of the surface toolpath using chordal deviation to linearize the toolpath. A smaller cut tolerance value creates a more accurate toolpath. However, the resulting toolpath might take longer to generate and might result in a longer NC program. On smaller parts, increase the tolerance. On larger parts, lower the tolerance.
Look ahead
Sets how many segments to consider at one time for reduction.
Create arcs in XY / XZ / YZ
Select the planes in which you want Mastercam to create arcs. Selections must be compatible with the current control definition.
Minimum arc radius
Defines the smallest arc that can be created in the Art toolpath. Some CNC controls have limits.
Maximum arc radius
Defines the largest arc that can be created in the Art toolpath.