Milling Parameters Specific to Roughing and Reroughing

In addition to the common milling parameters, the following parameters control the tool path generated by a Roughing or Reroughing NC sequence:

Specifies the maximum allowed step depth. After finding the positions of the highest and lowest slices, the software calculates the actual step depth, which is less than or equal to the specified MAX_STEP_DEPTH and results in a minimum number of uniformly spaced slices.

Specifies the way the tool scans a horizontal machining slice that contains at least one "soft" wall, that is, an open side. All the options are intended for high speed machining:

• CONSTANT_LOAD—Generates a cutter path that produces an approximately constant tool load.

• SPIRAL_MAINTAIN_CUT_TYPE—Generates a spiral cutter path with reverse arc connections between cuts. When a cut is finished, the tool arcs into the next cut, reversing cutting direction to maintain the cut type with respect to remaining material (CLIMB or CONVENTIONAL). This option minimizes retracts.

• SPIRAL_MAINTAIN_CUT_DIRECTION—Generates a spiral cutter path with S-shape connections between cuts. When a cut is finished, the tool S-connects into the next cut, maintaining cutting direction, which results in the cut type with respect to remaining material changing between cuts (from CLIMB to CONVENTIONAL and back). This option minimizes retracts.

• FOLLOW_CONTOUR (default)—The shape of each cut follows the shape of the hard walls, maintaining a fixed offset between the respective points of two successive cuts.

Specifies the way the tool scans a horizontal machining slice that is completely surrounded by hard walls. All the options are intended for high speed machining:

• CONSTANT_LOAD (default)—Generates a cutter path that produces an approximately constant tool load.

• SPIRAL_MAINTAIN_CUT_TYPE and MAINTAIN_CUT_TYPE—Generates a spiral cutter path with reverse arc connections between cuts. When a cut is finished, the tool arcs into the next cut, reversing cutting direction to maintain the cut type with respect to remaining material (CLIMB or CONVENTIONAL). This option minimizes retracts.

• SPIRAL_MAINTAIN_CUT_DIRECTION and MAINTAIN_CUT_DIRECTION—Generates a spiral cutter path with S-shape connections between cuts. When a cut is finished, the tool S-connects into the next cut, maintaining cutting direction, which results in the cut type with respect to remaining material changing between cuts (from CLIMB to CONVENTIONAL and back). This option minimizes retracts.

• FOLLOW_CONTOUR—The shape of each cut follows the shape of the hard walls, maintaining fixed a offset between the respective points of two successive cuts. Because the cuts are closed, there are S-shape connections between the cuts.

For CONSTANT_LOAD, MAINTAIN_CUT_TYPE, and MAINTAIN_CUT_DIRECTION scan types, this distance determines whether the tool stays on the surface or retracts when a decision between the two states is made.

Specifies the minimum radius allowed for concave corners in high speed machining.

Specifies the radius for filleting or smooth corner machining. The minimum value must be 10% of the tool diameter if the SMOOTH_SHARP_CORNERS parameter is defined and not set to CONSTANT_RADIUS. The maximum allowable value is 50% of the step-over distance. Corner rounding is available for line-line, line-arc, and arc-arc (if they are not tangent) connections.

• NO—A rounding radius is not used while machining sharp tool path corners. This is the default.

• CONSTANT_RADIUS—Rounds sharp corners using a rounding radius having a value equal to that of the SMOOTH_RADIUS parameter.

• RADIUS_BY_ANGLE—Rounds sharp corners using a rounding radius having a value based on the angle of the sharp corner and the SMOOTH_RADIUS value as follows.

Angle	Rounding radius
less than 5 degrees	10% of the SMOOTH_RADIUS value
less than 10 degrees	20% of the SMOOTH_RADIUS value
less than 20 degrees	40% of the SMOOTH_RADIUS value
less than 30 degrees	60% of the SMOOTH_RADIUS value
less than 60 degrees	80% of the SMOOTH_RADIUS value
less than 180 degrees	100% of the SMOOTH_RADIUS value

• MAX_RADIUS—Rounds sharp corners using the largest possible radius between 10% and 100% of the SMOOTH_RADIUS value.

Specifies the use of a progressive slowdown in the feed rate before a corner followed by an acceleration to the cut feed rate after the corner. The default is NO.

Specifies the length of the move for the slowdown. The same length is used for the acceleration after the corner. The length is measured from the sharp edge or the beginning of the rounding fillet, if any. If one of the edges is an arc, the distance is taken along the arc.

Specifies the feed rate at the end of the slowdown. For example, if the cut feed rate is 30 inches per minute and the value of the SLOWDOWN_PERCENT is 10, then the feed rate at the end of the slowdown is 3 inches per minute.

Specifies the number of steps in which the slowdown takes place. A larger number of steps results in a smoother slowdown. At each step, the feed rate is reduced by (100-SLOWDOWN_PERCENT)/NUMBER_SLOWDOWN_STEPS.

Controls whether extra slices are generated to satisfy the ROUGH_SCALLOP value, and defines the machining order:

• NO—No extra slices are generated to control the scallop height.

• DURING—The software generates the extra slices and inserts them between the regular slices.

• DURING_BOTTOM_UP—The software generates the extra slices and inserts them between the regular slices, performing them from the bottom up to optimize the tool load.

• AFTER—The software generates the extra slices. The tool machines all the regular slices first, and then machines the extra slices to reduce the scallop height, where needed.

The maximum scallop height for the steps left between the machining slices. Where the scallops are greater than this value, the software generates the extra slices that just machine the area required to remove the scallop.

• TANGENT_HELIX—The tool enters a closed slice by following a helical trajectory, tangent to the start point of the slice. The diameter of the helix is specified by the HELICAL_DIAMETER parameter. The helical pitch value is controlled by the RAMP_ANGLE parameter.

• RAMP—The tool enters from the top, at an angle controlled by the RAMP_ANGLE parameter.

• TANGENT_HELIX—The tool exits by following a helical trajectory, tangent to the end point of the slice. The diameter of the helix is specified by the HELICAL_DIAMETER parameter. The helical pitch value is controlled by the RAMP_ANGLE parameter.

• RAMP—The tool exits in a straight line, at an angle controlled by the RAMP_ANGLE parameter.

• SMART (default)—Minimizes the number and the height of retracts. For each intermediate retract within the NC sequence, the software calculates a safe level for the tool to traverse to the new position. This safe level is determined as the level of the lowest slice with no obstructions on the way of the tool, plus the PULLOUT_DIST value, if specified.

• ALWAYS—The tool retracts to the retract plane after each slice.

Specifies the maximum distance between the periphery of the tool and a wall for approach and exit motions within a roughing or reroughing slice.