Sim 5x Options
This subheader enables you to define advanced options for Sim. 5-Axis operations.
Parameter Name |
Description |
PRP Name |
| Auto Angle Pair | The post-processor automatically determines which pair of angles to use. | auto_angle_pair |
| Other Angle Pair | The second angle pair, other than the first determined automatically, is used. | other_angle_pair |
| Start Angle Type | Defines the type of start angle. | start_angle_type |
| Solution Type for Start Angle | Defines the type of solution for start angle. | solution_for_start_angle |
| Preferred Start Angle | Defines the preferred start angle. | start_angle |
| Angle Tolerance for Using Machine Limits | Defines the angle tolerance for using the machine limits. | angle_tol_for_limits |
| Interpolation for Distance | Indicates whether the interpolator for distance is on or off. | interplat_for_dist |
| Enable Mx Edit | Allows editing inside the 5-Axis operation the values of Auto Angle Pair and Other Angle Pair. | enable_mx_edit |
| Use Machine Limits | Defines whether or not to use the machine limits in both translational and rotational axis. | use_machine_limits |
| Retract Distance | Determines the retract distance of the tool from the part if a large angle change is detected in accordance with the Angle Change Limit value. | retract_distance |
| Interpolation Distance | Defines the interpolation distance. The postprocessor will interpolate between two tool tip positions (relative to the part coord.) using this threshold value. | interplat_distance |
| Angle Change Limit | Defines the angle change limit in degrees from one posted tool path position to the next one. | angle_change_limit |
| Interpolation Angle Step | Defines the interpolation angle step in degrees; the post-processor will interpolate between posted tool path positions using this angle. | interplat_angle_step |
| Pole Angle Tolerance | Defines the pole areas where the rotary axis and spindle direction are parallel. | pole_angle_tolerance |
| Use Tool H Length | Determines whether the tool length offset (H length) will be added to the NC code values (GCode) or will be regarded as 0, and tool length correction will be added by activating it on the machine. | Use_Tool_H_Length |
| Use Part Shifting | Defines whether to use shifting from machine reference point value defined in Machine Coordinate System (e.g., MAC 1 (1- Position)) or declare it as 0 for GCode calculation only. |
Use_part_shifting |
| Use Rot Axis Base Point2 | Defines whether to use distance from rotational axis value defined in rot_axis_base_point2 or declare it as 0 for GCode calculation only. | Use_rot_axis_base_point2 |
| G-code Ref. to Part Coordinate | Resolves both the kinematic and tool length compensation for controls that can directly use the part coordinates based X, Y and Z values to inform the NC-program that the coordinates are relative part coordinates. | GCode_part_coordinate |