Pocketing

Resource Parameters

The Resource tab allows you to select a tool.

Resource Tab

Parameter	Description
Select a Tool from Session	Selects a tool in Resource Configuration View.
Select from Catalog	Selects a tool from a reference tool file or PLM catalog.
Select from Database	Selects a tool from the database.
Display Tool Properties	Accesses tool parameters.
Define Tool Axis	Defines the tool axis.
Tool Number	Defines the number of tools.
Display Tool	Displays the tool position.
Default	Displays the tool at default position.
User Defined	Displays the tool at a position defined by the user. Note: You can define the tool position using Select a Tool from Session .

Tools

End Mill tools , Face Mill tools , TSlotter tools and Conical tools are available for these operations.

Geometry Parameters

The Geometry tab allows you to define the geometric parameters that are machined.

Machining Area Feature

Specifies a prismatic machining area feature. Clicking displays a brief summary of the computed parameters.

Once a feature is selected, the bottom plane direction is overridden by the tool axis direction of the operation. That is to say, the direction of the virtual bottom plane is guided by the operation's tool axis and always remains perpendicular to the tool axis.

For more information, see About Virtual Bottom Plane Concepts.

Mandatory Parameters

Mandatory Parameter	Description
Bottom	Specifies the bottom planar face or surface of the machining operation. Can be Hard or Soft.
Contour	Specifies the guide of the machining operation.
Tool Axis	Specifies the tool axis of the machining operation.

Optional Parameters

Optional Parameter	Description
Start Point	Specifies the preferred start point of the tool path. Note: If the Start Point is located outside of an open pocket, specify a clearance with respect to the pocket boundary.
End Point	Specifies the preferred end point of the tool path.
Top	Specifies the top plane with an optional offset.
Check	Specifies the check elements with an optional offset.
Island	Specifies islands that are defined by hard boundaries with an optional offset on each island.
Type	Specifies the pocket type.
Pocketing Style	Specifies the pocketing style.
Bottom Type	Specifies the bottom type on planar faces or on a surface: Hard or Soft.
Offset on Hard Boundary	Specifies the hard boundary offset.
Offset on Soft Boundary	Specifies the soft boundary offset.
Start	Specifies the preferred start of the machining operation: Inside or Outside.

Strategy Parameters

The Strategy tab allows you to specify the strategy and user parameters.

Machining

Parameter	Description
Pocketing Tool Path Style	Specifies tool path style. The Tool path style options are as follows: Outward helical: The tool starts from a point inside the pocket and follows outward paths parallel to the boundary. Inward helical: The tool starts from a point inside the pocket and follows inward paths parallel to the boundary. Back and forth: The machining direction is reversed from one path to the next. Offset on part One-Way: The machining direction is offset on the part one way. Offset on part Zigzag: The machining direction is offset on the part zigzagging. Concentric: The tool follows successive arc motions. For more information, see the section below. Outward and Inward Spiral Morphing: The tool follows a true spiral motion evolving smoothly to match the boundary of the pocket. For more information, see the section below.
Direction of Cut	Specifies how machining is to be done: Climb milling: The front of the advancing tool (in the machining direction) cuts into the material first. Conventional milling: 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.
Limit Machining Area with Fixture	Relimits the area to machine for computing the tool path without jump motions around the check elements. If selected: There is a contour around the check, and no jump motion. If not selected: There is a jump motion around the check element.
Compensation Output	Manages the generation of cutter compensation (CUTCOM) instructions for the pocketing operation side finish pass. None Both the tool and cutter profile are visualized during tool path replay. Cutter compensation instructions are automatically generated in the NC data output. Note: An approach macro must be defined to allow the compensation to be applied. 2D Radial Profile The tool is visualized during tooltip path replay. Cutter compensation instructions are automatically generated in the NC data output. Note: An approach macro must be defined to allow the compensation to be applied. 2D Radial Tip Cutter compensation instructions are not automatically generated in the NC data output. However, CUTCOM instructions can be inserted manually. For more information, see Procedures for Generating CUTCOM Syntaxes
Compensation	Specifies the tool corrector identifier to be used in the operation. The corrector type, corrector identifier, and corrector number are defined on the tool. When the NC data source is generated, the corrector number is generated using specific parameters.
Roughing	Removes material before the bottom finishing paths. Limits are defined with points along the revolution axis of the bottom or plane perpendicular to this axis. Only cylindrical or conical bottoms are accepted. If selected: The Air Cut Optimization parameter is available. See Create and Edit a Part Operation The Offset on Island Contours is available. See Geometry Parameters
Finishing	See Strategy Parameters > Finishing Strategy Parameters.

Concentric Tool Path Style Parameters

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 style is most suitable for hard-material milling, such as milling titanium, stainless steel, and ceramic materials where the tool needs to be protected. Other tool path styles, which are based on a constant distance between passes, are not appropriate because the tool load increases significantly when milling the inside of a radius.

The Concentric style controls the tool load by modifying, for each motion, the distance between passes. As a result, the tool lifetime is increased and the machining time is optimized.

Parameter	Description
Pattern	Defines 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. This 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. This pattern is preferred by the auto mode for milling closed areas with a starting drilling hole. Dynamic: The pattern is constructed with segments and follows the stock shape. This 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. This pattern is preferred by the auto mode for milling opened areas.
Movement	One-Way: The tool path uses the selected cutting direction. 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.
Maximum Discretization	Defines the computation step for dynamic patterns. This parameter controls the general quality of the tool path. Smaller steps result in a higher quality but the computation time can be heavily affected. 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 %	Defines 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 shape 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 %)	Defines the reverse radial engagement when milling in the reverse direction, that is the direction 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 directions.

Outward and Inward Spiral Morphing Tool Path Style Parameters

Outward and Inward Spiral Morphing tool paths give priority to a continuous machining motion (the goal is to avoid retract and linking motions as much as possible) and ensures that the step over does not exceed a maximum defined.

This strategy is more appropriate for a small step over between passes and a regularly shaped contour Otherwise, a small step over is generated by the morphing algorithm.

The High Speed Milling (HSM) feature guide cornerization is available for this strategy, as it relies already on a spiral and adapted offset motion.

The end point is not supported and is silently ignored.

The start point management: Start point is supported for Outward only.

If a start point is provided, the system verifies the reachability of this point. Nonreachable points are silently ignored. If points are reachable, the spiral motion starts from this point.

Island management: If an island is selected, the tool path starts (or finish depending on inward/outward flavor) around the island. If more than one island is selected or a reachable start point is given, the tool path contains a retract and linking motion.

If start point and island with Outward flavor is specified, the spiral starts at the start point and progresses toward the external contour. It then returns to the start point (after a linking motion) and progresses toward the island (with respect to the cutting mode).

Radial Strategy Parameters

Parameter	Description
Mode	Specifies how the distance between two consecutive paths is computed: Maximum distance between paths Tool diameter ratio Step over 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: Tool diameter ratio Step over 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 the distance between paths to avoid scallops on all level.
Truncated Transition Paths	When selected, truncates the transition portion of the trajectory to follow the external profile more exactly. Available with Back and Forth tool path style.
Contouring Pass	Allows a final machining pass around the exterior of the trajectory and islands for removing scallops. Available with Back and Forth or Concentric tool path styles.
Contouring Ratio	Specifies the contouring ratio to adjust the position of the final contouring pass for removing scallops. This is done by entering a percentage of the tool diameter (0 to 50). Available with Back and Forth or Concentric tool path styles.
Always Stay on Bottom	When selected, forces the tool to remain in contact with the pocket bottom when moving from one machining domain to another. Note: Behavior is different with the Concentric tool path style: When this parameter is activated, most Return on Same Level macros are replaced by optimized linking motions. These motions 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: Approach and retract parts use the global approach and retract feedrates.

Axial Strategy Parameters

Parameter	Description
Mode	Specifies how the distance between two consecutive levels is 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.

Finishing Strategy Parameters

Parameter	Description
Mode	Specifies whether or not finish passes are generated on the sides and bottom of the area to machine: No finish pass Side finish last level Side finish each level Finish bottom only Side finish at each level & bottom Side finish at last level & bottom
Side Finish Thickness	Specifies the thickness of material that is machined by the side finish pass.
Number of Side Finish Paths by Level	Specifies the number of side finish paths for each level in a multilevel operation. This can help you to reduce the number of operations in the program.
Bottom Thickness on Side Finish	Specifies the bottom thickness used for a last side finish pass, if side finishing is requested on the operation.
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 is machined by the bottom finish pass.
Spring Pass	Indicates whether or not a spring pass is 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	Adjusts the distance between paths to avoid scallops on the bottom. This is available for single-level and multi-level operations with bottom finish pass.
Compensation Output	Manages the generation of cutter compensation (CUTCOM) instructions for the pocketing operation side finish pass: 2D Radial profile: Both the tool and cutter profile are visualized during tool path replay. Cutter compensation instructions are automatically generated in the NC data output. Note: An approach macro must be defined to allow the compensation to be applied. 2D Radial tip: The tool is visualized during tooltip path replay. Cutter compensation instructions are automatically generated in the NC data output. Note: An approach macro must be defined to allow the compensation to be applied. None: Cutter compensation instructions are not automatically generated in the NC data output. However, CUTCOM instructions can be inserted manually. For more information, see Procedures for Generating CUTCOM Syntaxes.

High Speed Milling (HSM) Strategy Parameters

These parameters are disabled if a Concentric tool path style is selected.

Parameter	Description
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 an HSM operation. Value must be smaller than the tooltip radius.
Limit Angle	Specifies the minimum angle for rounding corners in the tool path for an HSM operation.
Extra Segment Overlap	Specifies the overlap for the extra segments that are generated for cornering in an HSM operation. This is to ensure that there is no leftover material in the corners of the trajectory.
Cornering on Side Finish Path	Specifies whether or not tool path cornering occurs on the side finish path.
Corner Radius on Side Finish Path	Specifies the corner radius used for rounding the corners along the side finish path of an HSM operation. Note: 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.
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.

Tool Axis Parameters

Global Tab

Defines the Tool Axis Mode. You can modify the tool axis of a tool path resulting from a machining operation without changing its contact point by:

• changing a 3-axis tool path into a 5-axis tool path.
• modifying a 5-axis tool path.

Parameter	Description
No 3/5 axis converter	Enables or disables 3/5 axis converter availability.
Fixed Axis	The tool axis arrow proposes a context menu: Select: Defines the tool axis. Analyze: Starts the Geometry Analyzer.
Thru a Point	The tool axis passes through a specified point. The label is a toggle to orient the tool axis To the point or From the point. The point in the sensitive icon lets you select a point in the work area.
Thru a Guide	The tool orientation is controlled by a geometrical curve (guide), that must be continuous. An open guide can be extrapolated at its extremities. The label is a toggle to orient the tool axis To the guide or From the guide. The red curve in the sensitive icon lets you select a curve in the work area. Angle: Specifies a lead angle.
Normal to Part	The tool axis is normal to the part. Angle: Specifies a possible frontal angle between the tool axis and the normal to the part.
Fixed Angle	The new tool axis forms an angle with the initial tool axis. Angle: Specifies this fixed angle. Privileged angle with the tool path: Defines the angle a plane defined by the direction of motion (Frontal angle) or in a plane normal to the direction of motion (Lateral angle).
Normal to Drive Surface	The new tool axis is normal to the drive surface. Angle: Specifies a possible lead angle. Note: Use a smooth surface as the drive surface.
4 Axis	Converts a 3-axis or 5-axis tool path as follows: All the tool axes are tilted and constrained with a fixed angle with the normal (N) of the given reference plane. All the tool axes are constrained along a cone defined by the angle with the normal of a reference plane (N) and a given point (P). Note: If the angle (Alpha) is defined as 90°, all the tool path axes are constrained to planes perpendicular to the normal of the given reference plane. The associated parameter is Tilted/Cone angle. The Cone constraint check box lets you define a point to define the cone axis.

Collisions Checking

Parameter	Description
Activate collisions checking	Activates or deactivates collisions checking.
Collision checking strategy	Defines the strategy: Automatic or Manual.
Part, Check, Design Part	Enables collision checking on one or multiple elements. Note: For collision checking with design parts, make sure that you have selected a valid Design Part in the Part Operation.
Check from Part Operation	Considers Check defined in Part Operations.
Fixtures on Part Operation	Takes into account Check defined with the Part Operation
Offset on Tool	Defines the tolerance distance specific to the tool radius and tool length.
Offset on Tool Assembly	Defines the tolerance distance specific to the tool assembly radius and tool length.
Max Discretization Angle	Specifies the maximum angular change of tool axis between tool positions.
Minimum Length	Specifies the minimum distance that must exist between two collision points to allow the modification of the tool axis between those two points.
Angle Mode	Defines the angle mode: Frontal or Lateral.
Minimum Angle	Defines the minimum angle range within which the tool axis can vary.
Maximum Angle	Defines the maximum angle range within which the tool axis can vary.
Step Angle	Defines the computation step used to find the optimal angle to avoid collisions. The smaller the Step Angle, the longer the computation time.

Machine Kinematics

This tab lets you correct problems encountered with respect of the machine kinematics.

Parameter	Description
Optimize Machine Rotary Axis	If selected, minimizes the variations of rotary degree of freedom, as well as tool axis variations.
Correct Out of Limit Points	When this check box is selected, the points out of limits are removed: If the point is out of limits in the X, Y, or Z-Axis, it is removed. If the point is out of limits in the A, B, or C-axis, the tool axis is corrected and locked in the position limit. If the point with the corrected axis is in collision, the point is removed.
Correct Large Angular Variation on Machine Rotary Axis	If, between two points of the tool path, the variation on a rotary DOF (angular join of the machine) exceeds the Maximum variation, you can select one or several check boxes to modify the machine configuration. When you select several check boxes, the most appropriate one is applied to any given point. Linking macro: The modification is done within the existing linking macro of the tool path. Tool pass: When the tool is in contact with the part, you can define a Fanning Distance. Note: Entering 0mm deactivates the Fanning Distance. Retract macro: A retract pass is added to reconfigure the machine.

Notes:

• If problems subsist after computing the tool path with those options, a message is displayed.
• These corrections apply to the tool path of the current machining operation.
• The machine configuration on the first point of the current machining operation is seen as the result of a motion from the Home position to this first point. Thus, it may differ from the actual one, resulting from previous machining operation and machine instructions.
• Angular variations between two points cannot be detected on the first point of the tool path, because the position of the machine before this point is unknown.

Macros Parameters

The Macros tab allows you to specify the macros to be used on the operation.

Activate or deactivate a macro by clicking on the name. Select a macro type from the list: None, Build by user, Horizontal axial, Axial, or Ramping.

Select Edit to edit the macro, Copy Macro to copy a macro, Paste Macro to paste a macro, or More to display the macro's context menu.

For more information, see Defining Macros and Macros.

Feedrate and Spindle Speed Parameters

The Feeds and Speeds tab allows you to define the following feeds and speeds parameters.

For more information, see About Feeds and Speeds.

Feedrate Parameters

Parameter	Description
Feedrate Unit	Defines the feedrate unit: Angular or Linear.
Approach Feedrate	Defines the speed of linear/angular advancement of the tool during its approach, before cutting.
Machining Feedrate	Defines the speed of linear/angular advancement of the tool during machining.
Retract Feedrate	Defines the speed of linear/angular advancement of the tool during its retract, after cutting.
Finishing Feedrate	Defines the speed of linear/angular advancement of the tool during finish machining.
Transition	You can locally define the feedrate for a transition path to a machining operation B from a machining operation A or from a tool change activity. For more information, see Setting a Transition Feedrate.
Local Value	Specifies the local feedrate value.
Slowdown Rate	Reduces the current feedrate by a given percentage. The reduction is applied to the first channel cut and to the transitions between passes.
RTCP ON	When selected, activates RTCP mode on transition paths between the previous and current operations.
Spiral Start Rate	Is defined as a percentage of the machining feedrate. By default, it is defined as 70% and can vary from 20% to 100%. Available with the Concentric tool path style.

Spindle Speed Parameters

Parameter	Description
Spindle Unit	Specifies the spindle unit: Angular or Linear.
Spindle Output	Activates or deactivates the NC output of the spindle speed.
Machining Spindle	Defines the speed of the spindle advancement.