Cut Pattern: Triangular Mesh
Use the Cut Pattern page to set parameters for a Triangular Mesh toolpath. Use a Triangular Mesh toolpath to machine where the tool is always in contact with the machining surfaces.
Not all options are available for all Pattern types.
Pattern
From the drop-down list, select the type of pattern for your Triangular Mesh toolpath.
Machining geometries
Click the Select arrow button to return to the graphics window for surface selection. When you have completed selection from the graphics window, press End Selection to return to the dialog box.
Select Clear all to deselect all previous selections.
Type
Select the type of projection to use from the drop-down list. Not all of these options are available for all pattern types.
- Offset: Creates offset patterns of the selected curve based on the stepover value.
- Parallel: Creates parallel cuts on multiple depths based on the machining angle.
- Adaptive: Ensures that the cutting conditions remain constant. This type avoids full-width cuts by constantly measuring the engagement of the tool with material and gradually removes material off the remaining stock.
- Radial: Creates a radial pattern based on the center point, inner and outer radii, and included angle for the pattern.
- User-defined: Projects the user selected curves to create the pattern.
- Spiral: Creates a spiral pattern based on the start and end angles, using the stepover value for the pitch.
- U-Shape: Creates a U-Shape cut projected onto machining surface, based on the start point and length of the edges of the rectangle.
- Morph: Creates morph patterns between a set number of curves while the toolpath is contained.
High speed
Applies high speed movement to your oscillation. High speed indicates smooth direction changes in the oscillation at the upper and lower points of amplitude.
Projection
Returns you to the graphics window to select the projection curves.
Select Clear all to deselect all previous selections.
Drive curves
Returns you to the graphics window to the define the path the tool will follow along.
Select Clear all to deselect all previous selections.
Machining angle in X,Y
Enter the angle of the cuts in the X,Y plane.
Machining angle in Z
Enter the angle of the cuts in the Z plane.
Radius
Enter the maximum projection distance. The distance is measured from the line to the surfaces.
Side shift
Enter the distance to shift the tool contact point toward the side of the tool, relative to the cutting direction. Use to ensure the side of the tool makes contact with the part and to avoid cutting with the tip.
Multiple passes on full width cut
Generates multiple passes in areas of the toolpath where the tool will encounter complete engagement. Use this option to prevent tool breakage resulting from over engagement in the toolpath.
Depth step
Enter the distance between roughing passes.
Offset type
Select from the drop-down to set the offset to be Global or Radial and Axial.
Offset
Enter a value to offset the machining surfaces. The value acts as a stock to leave amount for Triangular Mesh toolpaths.
Radial offset
Enter a value to offset the radial machining surfaces. The value acts as a stock to leave amount for Triangular Mesh toolpaths.
Axial offset
Enter a value to offset the axial machining surfaces. The value acts as a stock to leave amount for Triangular Mesh toolpaths.
Constant depth step
Enter the distance between depth steps. The depth steps are of equal value throughout the toolpath.
Multi pencil
Creates multiple offset cuts from the initial cut.
Number of cuts (Multi pencil)
Enter the number of cuts to add.
Output pattern
Creates the projection toolpath based on the Radius value and Area parameters, rather than projecting to the selected surfaces.
Part support
Specifies the surfaces intended to hold the desired part. Click the Select arrow button to close the dialog box and return to the graphics window for selection. When you have completed selection, press Enter to return to the dialog box.
Select Clear all to deselect all previous selections.
Width
Enter the width of the overall toolpath. The width value should be two times greater than the radius value.
Radius
Enter the maximum projection distance. The distance is measured from the line to the surfaces.
Number of slices
Enter a maximum amount of depth cuts to the toolpath.
Center point
Returns you to the graphics window and select the center point.
Radius / Angle start
Enter the value for the inner radius or the start angle, depending on which group box you are in.
Radius / Angle end
Enter the value for the outer radius or the end angle, depending on which group box you are in. You can select Autodetect to automatically detect the outer radius or end angle, or select User defined to enter the value yourself.
Number of cuts (left / right)
Enter the number of offset passes to create.
Step direction
Select Right, Left, or Both from the drop-down list. The projection curves will be offset in the selected manner based on chaining direction.
X length
Enter the length of the rectangular edge along X.
Y length
Enter the length of the rectangular edge along Y.
Multiple passes on full width cut
Generates multiple passes in areas of the toolpath where the tool will encounter complete engagement. Use this option to prevent tool breakage resulting from over engagement in the toolpath.
Style
Select the type of style to use from the drop-down list.
- Along: The projection is made along the line.
- Around: The projection is made perpendicular to the line.
Axis of rotation
Sets the main rotation axis when Pattern is set to Rotary. Choose an option from the drop-down menu. Selecting Line returns you to the graphics window to select a line as the axis of rotation.
Select Clear all to deselect all previous selections.
Select machining angles
Returns you to the graphics window to select a plane. The plane establishes the axes for creating the toolpath slices.
Constant Z
Sets the Machining angle in Z equal to 0. Deactivates Machining angle in X,Y.
Parallel
Sets the Machining angle in Z to 90 and activate Machining angle in X,Y. Set the fields to values needed for the best parallel pattern on your part.
Exclude undercut areas
Ignores undercut areas when calculating the toolpath.
Edge rolling
Optimizes tool rolling when machining vertical surfaces in angular areas, avoiding the creation of extra toolpath slices.
Corner smoothing loop
Allows loop segments in the corners of the U shape cuts.
Loop radius (stepover percentage)
Enabled when Corner smoothing loop is selected. Enter the loop radius for the corner smoothing loop.
Round corners
Activates the Round Corners page of the tree structure. Use to add fillets to the operation for internal corners of your part. By selecting this option, Sharp corners is unavailable.
Follow containment
Machines by following the 2d containment curves. The 2d containment checkbox must be active and the 2d containment curves must have been selected on the 2d containment page. If these options were not enabled, the toolpath will not be created.
Rest rough
Activates the Rest rough page of the tree structure. Use to machine previously uncut areas of the part based on the previous roughing tool diameter.
Containment
Activates Containment and the Containment page of the tree structure. Click Select to select a chain to control the cutting area of the part.
Silhouette containment
Activates the Silhouette Containment page of the tree structure. Use to create a silhouette boundary in the machining direction.
Draft angle
Enter an angle to apply to the toolpath.
Undercuts
Enables machine undercuts. The constant Z slices will go into undercut areas.
Closed offset
Available when the Rough pattern is selected. Select this option to adjust the tool offset.
Rest finishing
Activates the Rest Finishing page of the tree structure. Use to machine previously uncut areas based on the roughing tool diameter.
Angle range
Activates the Angle Range page of the tree structure. Use to set the cutting motion by entering two angles.
Trim to flute length
Trims the toolpath to the tool's flute length. Any motion deeper than the flute length is removed.
Sharp corners
Leaves sharp corners during tool motion. By selecting this option, Round corners is unavailable.
Minimum width
Enter the minimum width for the detection of flat areas to be machined. Available only when the Flatland pattern is selected or Machine flatlands is selected.
Maximum width
Enable then checkbox and enter the maximum width for the detection of flat areas to be machined. Available only when the Flatland pattern is selected or Machine flatlands is selected.
User defined containment
Activates the User defined containment page of the tree structure. Use to select a chain to control the cutting area of the part. Available when the Geodesic pattern is selected.
Line start point
Enter the X, Y, and Z coordinates of the projection line's starting position.
Start height along line
Enter the distance from the start point to begin the projection toolpath.
End height along line
Enter the distance from the start point to end the projection toolpath.
Start angle
Enter the angle to begin the rotation of the projection toolpath.
End angle
Enter the angle to end the rotation of the projection toolpath.
Step angle
Enter the angle between projected lines. Only available when the Style is set to Along.
Reverse
Reverses the toolpath sorting.
First pass along
Select the direction to sort projected curves from the drop-down.
First pass along X
Sorts in a positive or negative direction when moving along the X axis.
First pass along Y
Sorts in a positive or negative direction when moving along the Y axis.
Cutting method
Select the cutting method from the drop-down list. Not all of these options are available for all toolpath types.
- One way: The tool cuts each pass in the same direction.
- Zigzag: The tool cuts each pass in the opposite direction from the previous one.
- Spiral: The tool cuts in a spiral motion on the part.
- Clockwise: The tool cuts in a clockwise direction.
- Counterclockwise: The tool cuts in a counterclockwise direction.
Cut order
Select the cut order from the drop-down list. Not all of these options are available for all toolpath types.
- Standard: The default option which usually cuts from one side of the part to the other.
- From center away: Cuts from the approximate center of the part to the outer edges.
- From outside to center: Cuts from the outer edges of the part to the approximate center.
- From top to bottom: Cuts from the top of the part to the bottom of the part.
- From bottom to top: Cuts from the bottom of the part to the top of the part.
Feed rate (conventional)
Set an alternate feed rate for the conventional motion of a zigzag cut. If this option is set to zero, Mastercam substitutes it with the standard feed rate. This option is only available when the Cutting method is set to Zigzag.
Direction for closed cuts
Define the moving direction of the tool on the part depending on the rotation direction of machine spindle.
- Climb: The tool movement and the spindle rotation have the same direction.
- Conventional: The tool movement is opposite to the spindle rotation.
Direction for one way machining
Select Counterclockwise, Clockwise, Climb, or Conventional from the drop-down list to set the cutting direction.
Machine by
Select an option from the drop-down list. Note that not all options are available for all toolpaths.
- Depth: Cuts the part by its depth.
- Levels: Cuts the part by alternating between pockets for each level.
- Lanes: Cuts the part with the selected pattern.
- Regions: Splits the toolpath into regions when the tool encounters a gap. Use when the part geometry creates excessive air motion around gaps.
Intermediate slices
Processes intermediate slices After each depth step or After last depth step.
- After each depth step: Processes intermediate slices after each corresponding regular slice.
- After last depth step: Processes intermediate slices after the last regular slice is cut.
Start point
Activates the Start Point page of the tree structure. Use to set the tool's initial contact point with the part.
Start corner
Select the corner of the part from the drop-down list to start the cutting motion.
Start at
Select either Top or Bottom from the drop-down list. The selection tells Mastercam where to begin sorting of the cutting passes.
Machining direction
Select to machine Counterclockwise or Clockwise.
Cut tolerance
Determines the accuracy of the multiaxis toolpath. A smaller cut tolerance value creates a more accurate toolpath, but may take longer to generate the toolpath and create a longer NC program.
Maximum distance
Enter a value for the maximum distance between toolpath positions in the cutting direction. Use in operations where you need to have more points defined, such as on flat surfaces.
Damp
Allows a more flexible application of the axial shift.
Maximum stepover
Enter a value for the maximum distance between cutting passes.
Minimum stepover
Enter a value for the minimum distance between cutting passes.
Scallop height
Specifies the height of the remaining material between passes when using a rounded tool. Mastercam calculates the stepover based on the value that you enter here and the selected tool. The Scallop height field is linked to other Stepover fields so that when you type a value in one field, Mastercam automatically updates the others.
Adaptive
Creates additional parallel cuts on steep areas.
Perpendicular
Improves steep area processing when Pattern is set to Parallel cuts. This option creates regions with passes that are perpendicular to the original ones.
Detect threshold distance
Available when Perpendicular is selected. Enter the maximum height difference between two adjacent passes.
Pass extension
Available when Perpendicular is selected. Enter the amount for overlapping perpendicular and parallel passes.
Tool diameter %
Enter a percentage of the tool diameter to use for toolpath calculation.
Desired stepover
Enter the targeted stepover for the toolpath motion. The stepover value is adjusted up to the maximum stepover while trying to maintain the desired stepover.
Climb stepover (% stepover)
Enter a percentage of the stepover to use when climb motion is used in the toolpath.
Conventional stepover (% stepover)
Enter a percentage of the stepover to use when conventional motion is used in the toolpath.
Steep stepover
Enter the stepover for cutting on steep areas.





