Type of Machining Strategy:

Here are the key parameters, the set of which may vary depending on the chosen strategy in the Machining strategy section:

Step. The maximum allowed width of cut.

HSC step. Define the step of the trochoidal arcs as either; a percentage of the current tool diamater or, as a set distance. If the high speed cuts are disabled then unmachined areas are possible.

Big arcs. Expands arcs between the passes of the trajectory.

Finish pass. For some strategies, a finishing pass is added. Before the finishing pass, an allowance equal to the value specified in the parameter is added.

Compensation mode. Similar to the Output group in 2D contouring. See more

Finish rounding radius. The parameter is necessary for rounding corners during the finishing pass.

Rough rounding radius. The parameter is necessary for rounding corners during the roughing pass.

Linking radius. Linking radius for the 'links' and also the transitions for the trohoidal arcs.

Angle. Assigns the cut angle direction for the plane operations.

Corners smoothing. Virtually, it is used in most operations and provides toolpath 'rounding' when machining inner corners. This reduces vibrations and increases machining speed. Rough passes inside the contour do not have rounding.

Top level. The level at which the final pass is made. By default it is the top most level of the machined part.

Bottom level. Drag the plane with the mouse or drag the plane centre circle and use 'Smart snap' to align with a feature or, click on the dimension in the graph view to set the desired bottom level for machining. If the text in the field is green in colour, the level is calculated automatically as the top of the part, wokpiece and fixtures. To return to the automatic mode, simply clear the field and press 'Enter'.

Step up. Machining is performed strictly from top to bottom.

Step up value. Distance from the already machined layer to the overlying one.

Relief angle. Inputting a positive value avoids the tool shank 'rubbing' as the machining depth increases.

Here are the key parameters, the set of which may vary depending on the chosen strategy in the Machining strategy section:

Flats on finish feed. Outputs the Clear flats path on the finishing feed. Doesn't work with Cleanup height.

Cleanup height. The function adds a new pass at the distance specified in the parameter from the Clear flats pass, when the Clear flats option is enabled.

Climb. In machining refers to a cutting strategy where the tool moves in the same direction as the rotation of the workpiece. It typically results in less tool wear and a smoother finish compared to "Conventional" cutting, where the tool moves against the rotation of the workpiece. Climb cutting is often preferred when precision and surface finish are critical.

Conventional. Cutting in machining refers to a strategy where the tool moves against the rotation of the workpiece. This cutting method is used in machining operations, but it can result in more tool wear and a rougher finish compared to "Climb" cutting, where the tool moves in the same direction as the workpiece rotation. Conventional cutting is sometimes chosen when other factors, such as tool life or chip evacuation, are more important than surface finish.

Both. Refers to the practice of using both "Climb" and "Conventional" cutting strategies during a machining operation. This approach can be employed to optimize tool performance, surface finish, and other machining factors depending on the specific requirements of different parts of the workpiece or different stages of the machining process. It allows for greater flexibility and control in achieving desired results in machining.

Here are the key parameters, the set of which may vary depending on the chosen strategy in the Machining strategy section:

By cavities. All levels of the first profile are machined first. After that all levels of the next profile are machined.

By layers. The first layer of all profiles is machined in the beginning. After that the next layer is machined.

Downwards Only. Sort the machining to be strictly from the top to bottom. This can create a non-optimal toolpath. Enable this option only if you encounter errors with the level sorting. It can sometimes eliminate the problems.

Machining Order. Defines the machining sequence in the curve machining operations.

Direct. Sort the passes in such a way that the intersection begins on the left side of the arrow (parameter Angle), when looking in the direction of the arrow. It works only with the Parallel strategy.

Inverted. Sort the passes in such a way that the intersection begins on the right side of the arrow (parameter Angle), when looking in the direction of the arrow. It works only with the Parallel strategy.

Optimal. Sort the passes in such a way that the intersection begins at the shortest distance (which reduces the number of transitions between passes). This sorting method is applicable only with the Parallel strategy.

Hole capping. Quite often a geometrical model has holes the machining of which has been performed earlier or are required to be machined in a later operation. In this case, when machining the surface that has the hole, it can be ignored. The ignored holes can be of any shape (not always round). The defined size describes the diameter of a disk that can cover the hole.

Trim waste rolls. The cutter 'rolls' around the sharp outer corners of a model. The tool path is smooth but not always optimal.

Сonsists of:

Approach/Return. This group of parameters manages the tool movements from the tool change position to the start of the engage toolpathes, and back. See more.

Safe motions. Defines the type of Safety Surface and the distance from the workpiece to it. This surface facilitates transitions between the processed surfaces or tool paths, and the first stage of approach or return occurs toward it. See more.

Advanced links settings. This group of parameters specifies the features of trajectory formation for primarily five-axis operations, considering optimal movements of rotational axes. See more.

Links. Defines the rules governing Entry/Exit links and links between work moves. See more.

Distances. Distances required to switch feeds See more.

Allow plunges. Enabling plunges allows machining of closed pockets. When CAM software encounters a closed pocket that can not be machined from the outside, it forms a Plunge move. See more.