4-Axis Pocketing Operations

	The information in this section helps you to 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: machining criteria radial stepover conditions axial stepover conditions finishing high-speed milling. Specify the tool to be used , NC macros , and feeds and speeds as needed. 4-axis Pocketing Strategy Parameters 4-axis Pocketing Machining Parameters
	`Tool path style` Indicates the cutting mode of the operation: `Inward helical`: the tool starts from a point inside the pocket and follows inward paths parallel to the boundary. `Outward helical`: the tool starts from a point inside the pocket and follows outward paths parallel to the boundary. `Back and forth`: the machining direction is reversed from one path to the next `Part offset One-way`: tool motion is always done in the same direction following paths parallel to the boundary. `Part offset Zig-zag`: tool motion is done alternately in one direction then the other following paths parallel to the boundary.
	`Concentric`: Builds a safe-cutting trajectory by controlling the engagement of the tool. The trajectory created by the `Concentric` strategy adapts itself dynamically to ensure a safe cutting at nominal speed. The engagement of the tool is controlled to never exceed a maximum value, even in corner areas. This strategy is particularly recommended for hard-material milling. In this type of material(e.g. titanium, stainless steel, ceramic, ...) the tool needs to be protected. Other tool path styles -based on a constant distance between passes- are not appropriate because the tool load increases significantly when milling the inside of a radius. whereas the engagement is equal to the step over when milling in a straight line. The `Concentric` strategy controls the tool load by modifying the distance between passes for each motion. As a result, the tool lifetime is increased and the machining time is optimized.
	`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.
	`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.
	`Limit Machining Area with Fixture` Select this check box to re-limit the area to machine for computing tool path without jump around the check elements. This is de-activated by default.
	`Compensation` 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. `Movement` When `Movement` is set to `One-Way`, the tool path uses the selected cutting direction. When `Movement` is set to `Zig-Zag`, the tool path is optimized using both cutting directions (`Climb` and `Conventional`). The selected cutting mode is the main direction. Modifying it could change the trajectory. `Reverse pass (radial %)` Lets your define the reverse radial engagement when milling in the reverse direction, that is in the direction that is not selected as the `Direction of cut`. The value is a percentage of the main radial engagement. A value equal to 100% keeps the same engagement for the main and the reverse direction.

4-axis Pocketing Radial Stepover Parameters

Radial mode
Specifies how the distance between two consecutive paths is to be computed:

Maximum distance between paths

Tool diameter ratio

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. Depending on the selected Radial mode this value is used as

either Tool diameter ratio

or Stepover ratio .

Overhang
Allows a shift in the tool position with respect to the soft boundary of the machining domain.

Contouring pass
For 4-axis pocketing using a Back and Forth or Concentric tool path style, allows a final machining pass around the exterior of the trajectory for removing scallops.

Contouring pass ratio
For 4-axis pocketing using a Back and Forth or Concentric tool path style, 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).

4-axis Pocketing Axial Stepover Parameters

Axial strategy mode
Specifies how the distance between two consecutive levels is to be computed:

Maximum depth of cut

Number of levels

Number of levels without top.

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.

Breakthrough
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.

4-axis Pocketing Finishing Parameters

`Finishing mode` 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.
`Spring pass` 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.

4-axis Pocketing High Speed Milling (HSM) Parameters

`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.
`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.
`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.

4-axis Pocketing Geometry

A 4-axis Pocketing operation can be created for machining:

Closed pockets: the tool machines the area delimited by hard boundaries

Open pockets: the tool machines the area that has a least one soft boundary.

You can specify the following Geometry:

Pocket Bottom (cylindrical or conical surface) with possible Offset on Bottom. Bottom may be Hard or Soft.
Pocket Boundary (edges or sketch) with possible:

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.

Pocket Top (cylindrical or conical surface) with possible Offset on Top.
Fixture or check elements with possible Offset on Check.

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.

Specifying the Pocket Boundary

The pocket boundary must be closed. It can be specified in several ways:

If the Contour Detection contextual command is set, select the pocket bottom. The boundary of the selected face will be proposed as pocket boundary.

Select edges. In this case the Edge Selection toolbar appears to help you specify the pocket boundary.

Select the By Boundary of Faces contextual command. In this case the Face Selection toolbar appears to help you specify the pocket boundary.

4-axis Pocketing Tools

Recommended tools for 4-axis pocketing are End Mills, Face Mills, Conical Mills and T-Slotters.

4-axis Pocketing 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 check box is available for managing output of the SPINDL instruction in the generated NC data file. If the check box 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.

Feedrate Reduction in Corners

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 Pocketing, feedrate reduction applies to machining and finishing passes:

for all corners in Back and forth, and Concentric mode
for inside corners in Inward and Outward Helical modes, in offset on Part One-Way and Zigzag, in Inward and Outward Spiral Morphing.

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.

Slowdown Rate

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.

Combining Slowdown Rate and Feedrate Reduction in Corners

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 is:
100%, 70% (entry in slowdown), 70% (entry in corner: 75% ignored), 70% (end of corner, still in slowdown), 100% (end of slowdown).

4-axis Pocketing 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 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:

to link two non consecutive paths

to access finish and spring passes.

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.

Checking for Collisions with Part from Part Operation

When you select Collision checking on the Geometry tab page, the following dialog box appears.

When the Include Part from Part Operation check box is selected, the part is retrieved from the Part Operation if part is not defined at the Machining Operation level and used in collision check for approach/retract macro.
By default, the check box is not selected.

When the Include only selected faces check box is selected, faces are selected in the authoring window for collision checking. Face selection is activated only on selection of this check box, and the selected faces are considered for collision checking with the macro.
The Include Part from Part Operation and Include only selected faces options are mutually exclusive.
By default, the check box is not selected.