Arc Filter/Tolerance
Use this page to control toolpath tolerances. Typically, this involves several sets of variables.
Mastercam uses the values you enter here to convert the toolpath—originally created using G1, G2, G3 motions—to a refined set of smoothed G1 motions wherever possible, and within the tolerances you specify.
| Before refinement | After refinement |
|---|---|
|
|
Click the text below to see filtering and smoothing examples.
When you activate line and arc filtering, Mastercam replaces very small moves within the defined line/arc filter tolerance with larger ones wherever possible.
Illustration of Arc Filtering Algorithm
Example of Arc Filtering (left - unfiltered toolpath, right - filtered)
Illustration of Line Filtering
Example of Line Filtering (left - unfiltered toolpath, right - filtered)
You can apply the same maximum line and arc tolerance value to lines and arcs, or choose to tighten the tolerance more for lines or arcs as required by your application.
Line/arc filtering significantly reduces the number of NC blocks in the post, and may improve the machined precision of the part as well as its surface quality.
When to use Line/Arc Filtering:
- In 3D surface machining, line/arc filtering works best for kinematic surfaces such as planes, cylinders, cones, and spheres.
- Line/arc filtering may NOT be suitable for sculptural surfaces.
What to expect from Line/Arc Filtering:
- Improved quality of the machined surface.
- Reduced NC program length.
Line/Arc Filtering Precautions:
- May increase 3D surface faceting if applied to sculptural surfaces. To avoid this effect, independently reduce the line filtering tolerance (select Tighten Line filtering tolerance and reduce the percentage allocation), or turn off the line/arc filter by deselecting Line/Arc Filtering Settings.
- In the post processor, avoid using the Radius method of defining arcs (format: G2/3 X…Y...R…). Radius arc definitions may produce gouges on surfaces when the central angle of an arc is close to 180 degrees. To prevent this problem, use a different method of defining arcs in the post processor, such as the IJK method (format: G2/3 X…Y…I…J…).
Smoothing improves the quality of the machined surfaces and also creates better cutting conditions for the tools, decreasing tool wear.
- Represents a given set of tool motions (unsmoothed).
- Defines the curve (spline) that is the best fit for this set of points within the defined tolerance.
- Shows the smoothed redistribution of points along the curve. Point density depends on the local curvature.
The following sample images show the surface quality improvements smoothing provides.
| Before Smoothing | After Smoothing |
|---|---|
|
|
|
When to use Smoothing
- To improve any machined surface quality, especially sculptural surfaces.
- To speed up the machining process.
What to expect from Smoothing
- Improved quality of the machined surface in both roughing and finishing by reducing faceting, marks, and other surface machining defects.
- Reduced machining time for NC machines that support high speed mode where feed rate acceleration is possible.
- Reduced tool wear.
Smoothing Precautions
- Increased NC program length, especially when Use Fixed Segment Length is activated.
Common Toolpath Parameter Controls
Tolerance distribution
Allows you to dynamically adjust the toolpath's total tolerance. Total tolerance is the sum of the cut tolerance and the line/arc and smoothing tolerances. Adjust the total tolerance by entering a value in the Total tolerance field or by changing the values of the Cut, Line/Arc and/or Smoothing tolerances.
When you:
- Enter a value in the Total tolerance field, the Cut, Line/Arc and Smoothing tolerances are redistributed relative to their current percentages.
- Enter values directly into the Cut tolerance, Line/Arc tolerance and/or Smoothing tolerance fields, Mastercam updates the ratio between the inputs as well as the toolpath's total tolerance.
- Move the sliders between the Cut tolerance, Line/Arc tolerance and/or Smoothing tolerance fields, the ratios update in 5% increments and the toolpath's total tolerance remains at its current value. You can also enter a specific percentage directly into the fields.
XY (G17)
Create arcs in the XY plane. Choose this option if appropriate for your post processor configuration to handle arcs, usually designated as G17 in the NC code.
XZ (G18)
Create arcs in the XZ plane. Choose this option if appropriate for your post processor configuration to handle arcs, usually designated as G18 in the NC code.
YZ (G19)
Create arcs in the YZ plane. Choose this option if appropriate for your post processor configuration to handle arcs, usually designated as G19 in the NC code.
One way filtering
Filters a toolpath in one direction to avoid small polygonal patterns on the finish that can happen with zigzag filtering.
Minimum arc radius
Determines the minimum radius of any arc added to the toolpath by the arc filter. If an arc is smaller than the minimum arc radius, Mastercam adds lines to the toolpath in place of the arc.
Maximum arc radius
Determines the maximum radius of any arc added to the toolpath by the filter. If an arc exceeds the maximum arc radius, Mastercam adds lines to the toolpath in place of the arc.
Use maximal tolerance value for both
Choose this option to filter lines and arcs with the same tolerance set in the Line/Arc filtering tolerance field.
Tighten line filtering tolerance
Choose this option to filter lines using only a portion of the total Line/Arc filter tolerance. After selecting this option, enter a specific line filtering tolerance value. Or, use the slider to specify the percentage of the total Line/Arc filtering tolerance to apply only to lines. The slider and data entry fields are linked; when you modify one, the other updates automatically.
Tighten arc filtering tolerance
Choose this option to filter arcs using only a portion of the total Line/Arc filtering tolerance defined in the Tolerances Distribution section. After selecting this option, enter a specific arc filtering tolerance value in the field below or use the slider to specify the percentage of the total Line/Arc filter tolerance to apply only to arcs. The slider and data entry fields are linked; when you modify one, the other updates automatically.
Linking arc tolerance
Specifies the tolerance at which a linking arc (an arc from the Linking page) will be linearized.
Use fixed segment length
When selected, Mastercam smooths the toolpath motion by dividing it into uniform lengths using the specified Segment Length. Using this option can help prevent patterns on surfaces machined with parallel toolpaths, eliminating a wave effect. When unselected, Mastercam smooths the toolpath motion using a variable segment length. Using fixed segment lengths increases the NC program length.
Segment length
Available only when Use fixed segment length is selected. Defines the fixed segment length value Mastercam uses to smooth the toolpath motion.
Shift points randomly along toolpath
When selected, Mastercam randomly shifts the node points backwards and forwards along the toolpath within the specified tolerance. Using this option can help prevent patterns on surfaces machined with parallel toolpaths, eliminating a wave effect without significantly increasing the NC program length.
Minimize number of points
Choose this option to minimize the number of node points in the toolpath by excluding the points that are very close to each other.
Present arcs as line segments
When selected, Mastercam replaces all arc moves in the toolpath with linear moves.
Override arc feed rate
Increases and decreases the arc feed rate when cutting around corners. Feed rate is set on the Tool page.
-
Maximum ID decrease: Enter the maximum feed rate decrease for movement around inside arcs as a percentage or an exact feed rate.
-
Maximum OD increase: Enter the maximum percent feed rate increase for movement around outside arcs as a percentage or an exact feed rate.
The example below is a 2D Contour toolpath with a Feed rate of 20. Maximum ID decrease is set to 18 (10%) and Minimum OD increase is set to 22 (10%). Using Analyze Toolpath, you can see the changes to the feed rate as you machine.
Output 3D arc entry motion
Select this option to have Mastercam create the helix with arc (G2/G3) moves. Otherwise, the helix will be rendered with many small linear moves. This can be useful for some types of machines:
- Many machines have built-in look ahead capabilities. Using small linear moves with these capabilities can be more efficient than arc moves.
- Some older controls do not support helical arcs. For these controls, deselect this option.
- When this option is deselected for a 2D Pocket toolpath, Mastercam uses the Tolerance parameter on the Entry Motion page to control the accuracy of the entry helix. Refer to the Entry Motion: Pocket Help topic for more information.
Linearize toolpath
Linearizes the toolpath at whatever tolerance is specified in Total tolerance at the top of the page.





