Profile Contouring

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

For the Profile Contouring operations, the following tools are available:

• End Mill tools
• Face Mill tools
• Conical tools
• TSlotters tools
• Drills tools
• Spot Drills tools
• Center Drills tools
• Countersinks 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.

Contouring Mode

Parameter	Description
Between Two Planes	The tool follows a contour between top and bottom planes while respecting user-defined geometry limitations and machining strategy parameters.
Between Two Curves	The tool follows a trajectory defined by the guide contour and auxiliary guide contour while respecting user-defined geometry limitations and machining strategy parameters.
Between Curve and Surfaces	The tool follows a trajectory defined by a top guide curve and bottom surfaces while respecting user-defined geometry limitations and machining strategy parameters.
By Flank Contouring	The tool flank machines a vertical part surface while respecting user-defined geometry limitations and machining strategy parameters.

Mandatory Parameters

Mandatory Parameter	Description
Bottom	Specifies the bottom planar face or surface of the machining operation. Can be Hard or Soft. Available for Between Two Planes and Between Curve and Surfaces modes only.
Guide	Specifies the guide of the machining operation.
Tool Axis	Specifies the tool axis of the machining operation.

Optional Parameters

Optional Parameter	Description
First Relimiting Element	Defines the starting point of the relimiting element.
First Relimiting Mode	Allows you to specify the Go-Go type positioning of the tool with respect to the end element. Select one of the following modes: In On Out
Second Relimiting Element	Defines the ending point of the relimiting element.
Second Relimiting Mode	Allows you to specify the Go-Go type positioning of the tool with respect to the end element. Select one of the following modes: In On Out
Top	Specifies the top plane with an optional offset. Available for Between Two Planes mode only.
Check	Specifies the check elements with an optional offset.
Auxiliary Guide	Positions the tool tip along the tool axis (axial positioning). Available for Between Two Curves mode only.
Soft Boundary	Lets you select a soft boundary and define an offset on the boundary.
Material Side	Selects the material side.Available for Between Two Planes, Between Two Curves and Between Curve and Surfacesmodes only.
Bottom Type	Specifies the bottom type on planar faces or on a surface: Hard or Soft. Available for Between Two Planes mode only.
Top Type	Specifies the bottom type on planar faces or on a surface: Hard or Soft. Available for Between Two Planes mode only.
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.
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.

Parameters

The following parameters ae available for Between Two Curves and Between Curve and Surfaces modes only.

Optional Parameter	Description
Axial Offset 1	Defines an offset on the Guide contour.
Axial Offset 2	Defines an offset on the Auxiliary Guide contour.
Minimum Depth	Restricts machining to a specific zone. Available for Between Two Curves mode only.
Maximum Depth	Restricts machining to a specific zone
Depth Limitation	Enables machining restrictions to a specific zone.

Strategy Parameters

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

Machining

Parameter	Description
Tool Path Style	Specifies tool path style. Zig-zag The tool path alternates directions during successive passes. One-way The same machining direction is used from one path to the next. Helix The tool moves in successive concentric passes from the boundary of the area to machine toward the interior. The tool moves from one pass to the next by stepping over. Concentric The tool follows successive arc motions.
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.
Type of Contouring	Specifies the type of contour. 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 composed of two line segments Optimized The tool follows a contour derived from the corner that is continuous in tangent Forced Circular 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).
Close Tool Path	Specifies whether or not the program must close the tool path.
Tool Position ON Guide	Specifies the position of the tool tip on the guiding elements. The system already accounts for Offset on contour and driving mode.
Percetage Overlap	Specifies the amount that the tool must go beyond the end point of a closed tool path according to a percentage of the tool diameter.
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 Extended Radial Profile Generates Angular contours in sharp corners of a part.
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.
Compensation Application Mode	Specifies how the corrector type specified on the tool defines the position of the tool. You can specify: Output point Guiding point
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 The Offset on Island Contours is available. See
Finishing	See Strategy Parameters > Prismatic 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.

Radial Strategy Parameters

Parameter	Description
Sequencing	Specifies the order in which machining is done. Radial first Radial machining occurs first, then axial. Axial First Axial machining occurs first, then radial.
Side Step First	Handles each disconnected guide for all the passes (radial, axial, and finishing). Then the tool moves to the next guide and finishes all the passes for that guide.
Mode	Specifies how the distance between two consecutive paths is computed: Maximum distance between paths Step over ratio
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
Distance Between Paths	Defines the maximum distance between two consecutive tool paths in a radial strategy.
Number of Paths	Specifies the number of tool paths in a radial strategy.
Overhang for Rework Areas	Allows a shift in the tool position with respect to the soft boundary of the rework area.

Axial Strategy Parameters

Parameter	Description
Axial Strategy	Specifies how the distance between two consecutive levels is computed. The following options are available: Maximum depth of cut Number of levels Number of levels without top
Number of Levels	Defines the number of levels to be machined in an axial strategy.
Maximum Ramping Angle	Specifies the maximum ramping angle. This option is available when Tool Path Style is Helix in Between two planes mode.
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.
Smoothing Tool Path Along Tool Axis	Specifies the value (N%) to smooth the tool path when the tool path is going rapidly from a direction into a Z direction, without transition.

Prismatic 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 Path	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.

High Speed Milling (HSM) Strategy Parameters

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

Parameter	Description
Cornering Tool Path	Specifies whether or not cornering for HSM is to be done on the trajectory.
Cornering Radius	Specifies the radius used for rounding the corners along the trajectory of an HSM operation. Value must be smaller than the tooltip radius.

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 define transition paths in your machining operations by means of NC 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.