The information in this section will help you create and edit 4-axis pocketing operations in your manufacturing program.
Select 4-axis Pocketing 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:
Direction of cut
Specifies how milling is to be done:
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.
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.
Specifies how the distance between two consecutive paths is to be computed:
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. Depending on the selected Radial mode this value is used as
either Tool diameter ratio
or Stepover ratio .
Allows a final machining pass around the exterior of the trajectory for removing scallops (for 4-axis pocketing using a Back and Forth tool path style).
Contouring pass ratio
For 4-axis pocketing using a Back and Forth tool path style, this parameter adjusts the position of the final contouring pass for removing scallops. This is done by entering a percentage of the tool diameter (0 to 50).
Axial strategy mode
Specifies 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.
Specifies the distance in the tool axis direction that the tool must go completely through the part. Breakthrough is applied on the bottom element, which must be specified as soft.
Indicates whether or not finish passes are to be generated on the sides and bottom of the area to machine. There are several possible combinations:
Side finishing can be done at each level or only at the last level of the operation.
Bottom finishing can be done without any side finishing or with different combinations of side finishing.
Side finish thickness
Specifies the thickness of material that will be machined by the side finish pass.
Side thickness on bottom
Specifies the thickness of material left on the side by the bottom finish pass.
Bottom finish thickness
Specifies the thickness of material that will be machined by the bottom finish pass.
Bottom thickness on side finish
Specifies the bottom thickness used for last side finish pass, if side finishing is requested on the operation.
Indicates whether or not a spring pass is to be generated on the sides in the same condition as the previous Side finish pass. The spring pass is used to compensate the natural spring of the tool.
High Speed Milling
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.
Corner radius on side finish path
Specifies the radius used for rounding the corners of the side finish path in a HSM operation. Value must be smaller than the tool 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.
A 4-axis Pocketing operation can be created for machining:
You can specify the following Geometry:
- Offset on Hard Boundary
- Offset on Soft Boundary
- Offset on Contour. If you specify an Offset on Contour, it is added to any defined Offset on Hard Boundary and Offset on Hard Boundary.
Note: Start points are computed automatically and are located inside the pocket boundary. However, for open pockets, you can specify that the Start point is to be located inside or outside the pocket. If outside the pocket, you must specify a clearance with respect to the pocket boundary.
The pocket boundary must be closed. It can be specified in several ways:
Recommended tools for 4-axis pocketing are End Mills, Face Mills, Conical 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 reduce feedrates in corners encountered along the tool path depending on values given in the Feeds and Speeds tab page: reduction rate, maximum radius, minimum angle, and distances before and after the corner.
Feed reduction is applied to corners along the tool path whose radius is less than the Maximum radius value and whose arc angle is greater than the Minimum angle value.
For 4-axis Pocketing, feedrate reduction applies to machining and finishing passes:
Feedrate reduction does not apply for macros or default linking and return motions.
Corners can be angled or rounded, and may include extra segments for HSM operations.
You can use Slowdown rate in the Feeds and Speeds tab page to reduce the current feedrate by a given percentage.
The reduction is applied to the first channel cut and to the transitions between passes.
If a corner is included in a Slowdown path, the general rule is that the lowest percentage value is taken into account.
For example, if the Slowdown rate is set to 70 % and Feedrate reduction rate
in corners is set to 50%, the feedrate sequence is:
100%, 70% (entry in slowdown), 50% (entry in corner), 70% (end of corner, still in slowdown), 100% (end of slowdown).
If Feedrate reduction rate in corners is then set to 75%, the feedrate sequence
100%, 70% (entry in slowdown), 70% (entry in corner: 75% ignored), 70% (end of corner, still in slowdown), 100% (end of slowdown).
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 particular case of Ramping Approach macro for pocketing is described in Ramping Approach macro.
A Retract macro is used to retract from the operation end point.
A Linking macro may be used, for example:
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: When a collision is detected between the tool and the part or a check element, a clearance macro is applied automatically. If applying a clearance macro would also result in a collision, then a linking macro is applied. In this case, the top plane defined in the operation is used in the linking macro.