Surface Paths

This tab provides the parameters and settings to control the type of toolpaths to be generated to machine the drive surfaces selected.

It is categorized into 4 sections:

• Pattern

• Area

• Sorting

• Surface Quality

• Stepover

Parallel cuts

The 'Parallel cuts' option generates toolpaths with slices parallel to each other. The slice orientation is determined by two angles: X-Y,(which rotates the slices around the Z axis) and Z.

Cuts along curve

The 'Cuts along curve' pattern allows the user to create a toolpath orthogonal to a drive curve. That means that if the selected curve as 'Lead' is not a straight line the cuts are not parallel to each other.

Morph between 2 curves

This option creates a morph toolpath between two leading curves, inputted as 'First' and 'Second'. Morph means that the generated toolpath gradually interpolates between the two curves and spreads evenly over the surface. This option is well suited for machining steep areas when making moulds.

Parallel to multiple curves

The "Parallel to curve" option generates toolpath segments parallel to the leading curve, with each segment offset from the previous one, rather than simply copied. The curve must align exactly with the surface edge, ideally using the edge itself, to ensure accurate toolpath generation. Misaligned curves can result in incorrect toolpaths.

Project curves

This pattern allows for creating either a user-defined curve or a generic pattern, with options for 2D projections (radial and spiral) and 3D curve projections (offset and user-defined).

The user must specify the projection direction for the curves, with options including:

• X, Y, Z: Named directional axes

• Line: Defines the projection vector, ensuring it points correctly

• Surface Normal: Projects the curve along the surface's normal direction, available when "User defined" is selected.

Morph between 2 surfaces

This option generates a morph toolpath on the drive surface, enclosed by two check surfaces. The toolpath is evenly distributed across the drive surface, making it ideal for machining complex shapes like impeller blades.

Bi-Tangency:
The key benefit is the ability to compensate the tool to both the drive and check surfaces at the corners of the workpiece. To do this, enable the tool radius in the margin options, which sets the distance between the tool center and the surfaces.

Parallel to surface

The "Parallel to surface" option creates cuts on the drive surface that are parallel to a leading surface.

For the special case when the leading and drive surfaces form an inlaying edge, it is desired to have bi-tangency of the tool with both surfaces.

Flowline

The flowline creates a toolpath aligned to the short or long side, or along the U or V parametric dimensions of the surface.

The main advantage is that it doesn't require additional bounding geometries like walls or edge curves. It maintains a constant max step-over distance, even on complex surfaces, and has a fast calculation time.

Full, avoid cuts at exact edges

With this option the toolpath is generated on the entire drive surface, avoiding the surface edge. The first cut is not aligned exactly on the surface edge. To calculate the distance from the edge. Changing the maximum step over changes this value accordingly.

Full, start and end at exact surface edge

This option generates the toolpath on the whole surface and starts and ends at the exact surface edge or the nearest possible position.

Limit cuts by one or two points

This option allows you to limit the machining between two points on the drive surface, so you can work only on a certain parts of the surface.

2D Containment

The 2D containment contains the toolpath within a selected curve. The projection axis direction is used to project the given curve back to the part. The toolpath is then trimmed by the given curves.

Notes:

The 2D contour does not have to fit exactly on the surface. It can reach over the edges.

You can use multiple contours.

The contours must be closed contours.

Angle Range

For 5-axis parts with undercuts and a complex topology, the definition of shallow and steep areas is more abstract than the definition used for mold-making and 3-axis CAM systems.

The Angle range option allows users to define the areas to be machined by an angle range of the surface normal with respect to a user defined axis. The user has the option to machine everything inside the angle interval or outside the interval.

Extend/trim

With this option you can extend or trim the toolpath.

In case of 'extend' the toolpath will be extended tangentially and reaches over the drive surface with a straight line. This line has the same orientation as the last toolpath segment.

In case of 'trim' the toolpath will be trimmed along its way.

Round corners

This option can be set to find small radius areas and inner sharp edges in surface model. Such areas will be left out from toolpath generation. Inside corners can  cause  'fish tails' or 'dove tails' in toolpaths. Such fish tails are removed by turning on this switch. This flag can also be considered as a fillet generator. The surface model is rounded (filleted) in the direction of tool path slices with a radius to avoid small radii and inner sharp corners. The applied radius is the main tool radius plus the current stock to leave value. The fillet generation is independent of tool type and shape. In most cases, this switch is used in presence of a ball cutter, lollipop cutter or a conical cutter with ball tip. If swarf machining is applied (side cutting), then this parameter also applies to cylinder or torus cutters. With the additional radius you can increase the fillet radius in surface model. So fillet radius value is the tool radius and the stock remain plus the additional radius.

Flip Step Over

Flip step over changes the cut direction. This can change machining direction from the:

• Outside to inside in case of closed contours.

• Left to right in case of open contours (animations on the right).

Cut order

The cut order defines the sequence of the cuts.

• Standard - Sets a default cut order. Usually from one side to the other.

• From Center Away - The machining begins at center of the surface and progresses outwards.

• From outside to center - The machining begins from outside of the surface and progresses inwards.

Cutting Method

With the cutting method you define whether the machining is 'one way', 'zig zag' or 'spiral'.

• One way - The tool moves always in one cutting direction.

• Zig Zag - The tool moves in opposite cutting direction with every new cut. With this type of cutting, direction of machining cannot be determined. Only for the first cut, the direction will be established as "direction one" or "direction two".

• Spiral - Spiral will generate spiral cuts on the drive surface.

Direction for one way machining

This feature defines the direction in which the tool moves along the workpiece, depending on the direction of rotation of the machine spindle.

• Climb: Tool movement and spindle rotation are in the same direction (see the tool on the left in the image).

• Conventional: The tool moves in the opposite direction to the spindle rotation.

Machine by Lanes/Regions

The toolpath generated usually has a topology of multiple contours organized in lanes or regions, on the drive surfaces. When the toolpath is generated on many zones, then it might be preferable to machine all the regions independently. This machining area mode tells the system to follow the machining by lanes or by regions.

Start point

The start point defines the start position of the first cut and for the following cuts onto the drive surface. This point can be set by

• Position: The position can be picked form the geometry or it can be defined by the coordinates X, Y and Z. The selected point must not be located exactly on the drive surface. It's enough to pick a random point which is close to the desired start point position. The system will catch the nearest surface point and apply the start point to this position.

• Surface normal direction: Here the start point will be defined by a vector. That point of the toolpath which has its surface normal direction closest to the vector defines the new start point.

Cut tolerance

The cut tolerance is the tolerance for the accuracy of the toolpath. This value is the chordal deviation of the toolpath against the surfaces to be machined. In other words, the toolpath can have a maximum error to the surfaces in the range of plus or minus cut tolerance.

Surface edge handling

Surface paths are created on individual surfaces. Afterwards toolpath segments are merged together to create longer surface paths. The decision about the merging is currently based on a merge distance. If all toolpath segments on a toolpath slice is merged, it is checked if a closed surface path can be built by connecting the start to the end. The same merge distance value is used for deciding this. So all surface paths that are within closer distance than this value will be merged together. The main benefit is that tiny gaps or overlapping drive surfaces don't cause unexpected behavior in the toolpath.

Advanced

Machining surface quality depends on toolpath points, which vary with surface curvature. Higher curvature requires more points for accuracy. Chaining tolerance affects toolpath accuracy, with smaller tolerances reducing errors but increasing computation time. Step over calculations can be approximate or exact, influencing surface accuracy. Adaptive cuts and synchronized points improve precision but extend processing time.