Facing Operations

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.

Facing Strategy Parameters

Facing Machining Parameters

Tool path style
Indicates the cutting mode of the operation:
  • Inward helical: the tool starts from a point inside the area to machine and follows inward paths parallel to the boundary.
  • One way: the same machining direction is used from one path to the next.
  • Back and forth: the machining direction is reversed from one path to the next.
Direction of cut
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.

Machining tolerance
Specifies the maximum allowed distance between the theoretical and computed tool path.
Fixture accuracy
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.
Type of contour
Indicates the contouring type of corners in Inward helical:
  • Circular: the tool pivots around the corner point, following a contour whose radius is equal to the tool radius
  • Angular: the tool does not remain in contact with the corner point, following a contour comprised of two line segments
  • Optimized: the tool follows a contour derived from the corner that is continuous in tangent
  • Forced circular: This option may be used in certain complex cases when the Circular option does not give satisfactory results.

    It creates tool paths comprising of portions of circular arcs (for example, when grooves are present along the trajectory and the tool is too big to penetrate).

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. 

Facing Radial Stepover Parameters

Radial mode
Defines how the distance between two consecutive paths is to be computed. 

You should either set a Maximum distance between paths or give a Percentage of tool diameter to be used as:

either Tool diameter ratio or Stepover ratio .

Distance between paths
Defines the maximum distance between two consecutive tool paths in a radial strategy.
Percentage 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.

Tool side approach clearance
Specifies the clearance between the tool side and the part that must be respected when entering or leaving the material.

Facing Axial Stepover Parameters

Axial strategy mode
Defines how the distance between two consecutive levels is to be computed.
Maximum depth of cut
Defines the maximum depth of cut in an axial strategy.
Number of levels
Defines the number of levels to be machined in an axial strategy.

Facing Finishing Parameters

Finishing mode
Indicates whether or not a finish pass is to be generated on the bottom of the area to machine.
Bottom finish thickness
Specifies the thickness used for bottom finishing.

Facing High Speed Milling (HSM) Parameters

For Facing operations using an Inward helical tool path style only.

High Speed Milling
Specifies whether or not cornering for HSM is to be done on the trajectory.
Corner radius
Specifies the radius used for rounding the corners along the trajectory of a HSM operation. Value must be smaller than the tool radius.
Limit angle
Specifies the minimum angle for rounding corners in the toolpath for a HSM operation.
Extra segment overlap
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.
Transition radius
Specifies the radius at the start and end of the transition path when moving from one path to the next in a HSM operation.
Transition angle
Specifies the angle of the transition path that allows the tool to move smoothly from one path to the next in a HSM operation.
Transition length
Specifies a minimum length for the straight segment of the transition between paths in a HSM operation.

Facing Geometry

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.

Facing Tools

Recommended tools for Facing are End Mills, Face Mills and T-Slotters.

Facing Feeds and Speeds

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.

Facing NC Macros

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.

Facing P1/P2 Considerations

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: