The information in this section will help you create and edit Facing operations in your manufacturing program.
Select Facing then select the geometry to be machined.
A number of strategy parameters are available for defining:
Specify the tool to be used , NC macros , and feeds and speeds as needed.
|Tool path style
Indicates the cutting mode of the operation:
Specifies how milling is to be done in Inward helical:
Climb milling or Conventional milling
In Climb, the front of the advancing tool (in the machining direction) cuts into the material first
In Conventional, the rear of the advancing tool (in the machining direction) cuts into the material first.
Specifies the maximum allowed distance between the theoretical and computed tool path.
Specifies a tolerance applied to the fixture thickness. If the distance between the tool and fixture is less than fixture thickness minus fixture accuracy, the position is eliminated from the trajectory. If the distance is greater, the position is not eliminated.
Indicates the contouring type of corners in Inward helical:
Specifies the tool corrector identifier to be used in the operation.
The corrector type (P1, P2, P3, for example), corrector identifier and corrector number are defined on the tool. When the NC data source is generated, the corrector number can be generated using specific parameters.
Defines how the distance between two consecutive paths is to be computed.
either Tool diameter ratio or Stepover ratio .
Defines the maximum distance between two consecutive tool paths in a radial strategy.
of tool diameter
Defines the maximum distance between two consecutive tool paths in a radial strategy as a percentage of the nominal tool diameter.
|End of path
Defines how the tool path is to start and end with respect to the boundary between two consecutive paths (In or Out). Parameter available in One way and Back and forth only.
Allows a shift in the tool position with respect to the soft boundary of the machining domain.
Specifies the clearance between the tool side and the part that must be respected when entering or leaving the material.
Defines how the distance between two consecutive levels is to be computed.
depth of cut
Defines the maximum depth of cut in an axial strategy.
Defines the number of levels to be machined in an axial strategy.
Indicates whether or not a finish pass is to be generated on the bottom of the area to machine.
Specifies the thickness used for bottom finishing.
For Facing operations using an Inward helical tool path style only.
Specifies whether or not cornering for HSM is to be done on the trajectory.
Specifies the radius used for rounding the corners along the trajectory of a HSM operation. Value must be smaller than the tool radius.
Specifies the minimum angle for rounding corners in the toolpath for a HSM operation.
Specifies the overlap for the extra segments that are generated for cornering in a HSM operation. This is to ensure that there is no leftover material in the corners of the trajectory.
Specifies the radius at the start and end of the transition path when moving from one path to the next in a HSM operation.
Specifies the angle of the transition path that allows the tool to move smoothly from one path to the next in a HSM operation.
Specifies a minimum length for the straight segment of the transition between paths in a HSM operation.
You can specify the following Geometry:
The drive contour must be closed. It can be specified in several ways:
You can select start and end points as preferential start and end positions on the operation. This allows better control for optimizing the program according to the previous and following operations.
For One way and Back and forth tool path styles, you can select the Bounding envelope checkbox to machine the maximum bounding rectangle of the part. After selecting the geometry to be machined, this rectangle is computed after defining a machining direction.
The figures below illustrate how machining is done for different machining directions.
Recommended tools for Facing are End Mills, Face Mills and T-Slotters.
In the Feeds and Speeds tab page, you can specify feedrates for approach, retract, machining and finishing as well as a machining spindle speed.
Feedrates and spindle speed can be defined in linear or angular units.
A Spindle output checkbox is available for managing output of the SPINDL instruction in the generated NC data file. If the checkbox is selected, the instruction is generated. Otherwise, it is not generated.
Feeds and speeds of the operation can be updated automatically according to tooling data and the Rough or Finish quality of the operation. This is described in Update of Feeds and Speeds on Machining Operation.
You can define transition paths in your machining operations by means of NC Macros. These transition paths are useful for providing approach, retract and linking motion in the tool path.
An Approach macro is used to approach the operation start point.
A Retract macro is used to retract from the operation end point.
A Return on Same Level macro is used in a multi-path operation to link two consecutive paths in a given level.
A Return between Levels macro is used in a multi-level machining operation to go to the next level.
A Return to Finish Pass macro is used in a machining operation to go to the finish pass.
A Clearance macro can be used in a machining operation to avoid a fixture, for example.
Note that P2 functionalities for Facing include all Finishing
parameters and Sectioning for guiding element selection.
To edit in P1 a Facing operation that was created in P2, the following parameter values must be set: