Pocketing Operations

	The information in this section will help you create and edit `Pocketing` operations in your `Manufacturing Program`. Select `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. Pocketing Strategy Parameters 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. `Offset on Part One-way`: tool motion is always done in the same direction following paths parallel to the boundary. `Offset on Part 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. This has also been enhanced to reduce the computation time to make it acceptable for these cases. 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. The circular pattern builds the tool path mainly with circular arcs (G2/G3 in NC code). The tool path is smooth and never exceeds the maximum engagement. On the downside, the engagement is most of the time lower than the maximum engagement, usually leading to a tool path length longer than the dynamic pattern. This pattern is preferred by auto mode for milling closed areas with a starting drilling hole. The dynamic pattern builds the tool path mainly with segments. Each point is precisely computed to match the maximum engagement, and the trajectory follows the stock shape. On the downside, the tool path cannot be as smooth as the one from the circular pattern and its computation takes more time. This pattern is preferred by the auto mode for milling opened areas.
	`Inward spiral morphing`: the tool follows an inward spiral path parallel to the boundary. End point is not supported for both `Inward\Outward spiral morphing`. `Outward spiral morphing`: the tool follows an outward spiral path parallel to the boundary. Start point is supported for the `Outward spiral morphing`. If the start point is reachable, the spiral motion starts from this point. Non reachable points are silently ignored. Only one start point is supported in this release. For parts containing island, the tool path starts and ends around the island. The too path includes retract and linking motions for parts containing many islands with reachable start points. Revamp Inward and Outward Spiral morphing to include the management of the islands Island management: if an island is selected, the tool path will start (or finish depending of inward/outward flavor) around the island. If more than one island is selected or a reachable start point is given, the tool path will contain retract and linking motions. In Case of start point and island with OUTWARD flavor: The spiral starts at the start point and progress toward the external contour. Then it comes back to the start point (after a linking motion) and progress toward the island (cutting mode respected). `Note` in `HSM` tab, `Guide Cornerization` option is accessible when `Concentric` or `Inward/Outward spiral morphing` are selected in the `Tool Path Style`. See Guide Cornerization
	`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`Limits the area to machine to compute the tool path without jumping around the chek elements. `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. `Percentage of machining feedrate`Specifies the feedrate at start of spiral. This is available only with `"Concentric"` `Tool path style`. The range of values (20% to 100%). By default, the value is 70%. `Pattern` Lets you define the concentric tool path pattern: `Auto`: The pattern is automatically selected according to the shape of the pocket. `Circular`: The pattern is constructed with circular motions. `Dynamic`: The pattern is constructed with segments and follows the stock shape. `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. `Max. discretization` Lets you define the computation step for dynamic patterns. This parameter controls the general quality of the tool path. Smaller steps results in a higher quality, but may heavily affect the computation time. The step is used internally for the computation and does not reflect the distance between each point in the final trajectory. If the option is not activated, a default value is used. `Channel width %` Lets you define the relative width of the channel opening. A channel opening modifies the tool path by opening the pocket in its center, with either a circular or a dynamic pattern. Then the dynamic pattern follows the sape that has already been machined. A value equal to 100% deactivates the feature. The channel uses the pattern defined by the `Pattern` parameter. `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.

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.
`Avoid scallops on all levels` Specifies whether or not the distance between paths can be adjusted by the program in order to avoid scallops on all levels. Do not avoid scallops: Avoid scallops:
`Truncated transition paths` Enables the tool to follow the external profile more exactly by allowing the transition portion of the trajectory to be truncated (for pocketing using a Back and Forth tool path style). Not truncated: Truncated:
`Contouring pass` For pocketing using a `Back and Forth` or `Concentric` tool path style, allows a final machining pass around the exterior of the trajectory and islands for removing scallops.
`Contouring pass ratio` For 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).
`Always stay on bottom` When activated, forces the tool to remain in contact with the pocket bottom when moving from one machining domain to another. Note that the usage is different when the tool path style is set to `Concentric`: Most `Return on Same Level` macros are replaced by optimized linking motions. These motions should automatically avoid any collision with the part and the remaining stock. Use the `Clearance` parameter if you do not want these motions to remain in contact with the bottom. Use the `Feedrate` parameter to define a feedrate on the linking part of these motions. Note that the approach and retract parts use the global approach and retract feedrates.

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.

Automatic draft angle
Specifies the draft angle to be applied on the sides of the pocket.

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.

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.
`Number of side finish paths per level` Specifies the number of side finish paths for each level in a multi-level operation. This can help you reduce the number of operations in the program.
`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.
`Avoid scallops on bottom` Defines whether or not the distance between paths can be adjusted by the program in order to avoid scallops on the bottom. Available for single-level and multi-level operations with bottom finish pass.
`Compensation output` Allows you to manage the generation of Cutter compensation (CUTCOM) instructions for the pocketing operation's side finish pass. The following options are proposed: If `2D Radial profile` is selected, both the tool tip and cutter profile will be visualized during tool path replay. Cutter compensation instructions are automatically generated in the NC data output. An approach macro must be defined to allow the compensation to be applied. If `2D Radial tip` is selected, the tool tip will be visualized during tool path replay. Cutter compensation instructions are automatically generated in the NC data output. An approach macro must be defined to allow the compensation to be applied. If `None` is selected, cutter compensation instructions are not generated in the NC data output. In this case, please refer to How to generate CUTCOM syntaxes. Any user-defined PP words in macros are added to the cutter compensation instructions generated in the NC data output. Therefore, you should be careful when specifying CUTCOM instructions in macros. A negative Offset on contour (parameter in Geometry tab page) is possible for 2D radial profile output.

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.
`Limit angle` Specifies the minimum angle for rounding corners in the tool path 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.
`Guide Cornerization` Select this check box to cornerize the internal angles of the guide contour and specify the radius of the cornerization. The radius must be greater than the tool radius. By default: The check box is not selected The value for corner radius is 10mm.
`Cornering on side finish path` Specifies whether or not tool path cornering is to be done on side finish path.
`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.
`Limit angle on side finish path` Specifies the minimum angle for rounding the corners of the side finish path in a HSM operation.
`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.

Pocketing Geometry

A 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 (planar face or 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, Offset on Hard Boundary, and Offset on Island.

Pocket Top plane with possible Offset on Top.
Islands (defined by hard boundaries) with possible Offset on each island.
Fixture or check elements with possible Offset on Check.
Start and End points.

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

select the Sectioning contextual command. Please refer to Sectioning for details of how to use this capability.
Please note that the sectioning selection method is not associative.

Specifying Start and End Points

You can select a Start pointand an End point as preferential start and end positions for the operation. This allows better control for optimizing the program according to the previous and following operations.

Note that the Start point can be located outside an open pocket. In this case, you must specify a clearance with respect to the pocket boundary.

Pocketing Tools

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

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.

The figure below shows that feedrate reduction is not applied in Inward Helical for most of the corners, as these are not inside corners.

The figure below shows that feedrate reduction is applied in each corner in Outward Helical, as these are inside corners.

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).

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 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.

Specifying Ramping Approach Macros

When specifying a Ramping Approach macro in Pocketing, you can select the Parameter contextual command to access the parameters of the macro path.

If you select the Intermediate Levels check box, the approach macro is divided into three parts:

a ramping approach from the top of the pocket to the intermediate level
a horizontal path, which is the same as the first path if the machining mode is Back and Forth or the first closed path if the machining mode is Helical
a ramping approach from the intermediate level to the machining level.

The yellow path in the figure below illustrates an intermediate level for a ramping approach macro in Back and Forth mode.

Editing Parameters of Several Pocketing Operations

You can modify the common parameters of several Pocketing operations in one shot as follows:

Select two or more Pocketing operations either in the Specification tree or in the Process table.
Right-click the highlighted operations and select Selected Objects > Definition...
The Pocketing dialog box appears.
Modify any of the parameters that are available for edition.

Note: Parameters (including Geometry and macro definitions) can be edited if all the selected operations already have identical values. The parameters which are different in the selected operations are not editable; the displayed value is the one of the first operation selected. Tool parameters cannot be edited and Replay icon is disabled.

This command is enabled only if you have selected at least two operations of same type. This command is limited to the following operations: Multi Axis Flank Contouring, Multi Axis Curve Machining, Contouring, Isoparametric Machining, and Pocketing.

Click OK to apply the modified parameters of all the selected operations.

Pocketing P1/P2 Considerations

Note that P2 functionalities for Pocketing include Automatic Draft Angle, all Finishing parameters, and Sectioning for guiding element selection.
To edit in P1 a Pocketing operation that was created in P2, the following parameter values must be set:

Automatic draft angle = 0 deg

Finishing mode = No finish path

Side finish thickness = 0.0 mm

Side finish thickness on bottom = 0.0 mm

Bottom finish thickness = 0.0 mm

Spring pass = no

Avoid scallops on bottom = no

HSM Cornering on side finish path = no

HSM Corner radius = 1 mm

HSM Limit angle = 10 deg.

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.