Roughing

Resource Parameters

Resource Tab

The Resource tab allows you to select a tool.

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

Only End Mill tools are available for these operations.

Geometry

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

Mandatory Parameters

Parameter	Description
Part	Selects the part to machine.
Rough Stock	Define a rough stock if you have not already defined one in the Part Operation. If you do not have a rough stock, you can create one. See Creating a Rough Stock. The stock used in Roughing needs to be fully defined and closed (like a solid). Deviation to this policy may lead to inaccurate tool path computation (potential collision) and to error during video simulation. Therefore, it is no longer accepted.
Tool Axis	Defines the tool axis.

Optional Parameters

Parameter	Description
Check	Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Limiting Contour	Defines the outer machining limit on the part. You can also activate the Part autolimit option, with the Side to machine, Stop position, Stop mode and Offset parameters.
Zone Order	Lets you set the order in which the zones on the part are machined.
Imposed Point(s)	Specifies the imposed point.
Top	Defines the highest plane machined on the part.
Bottom	Defines the lowest plane machined on the part.
Safety Plane	It is the plane that the tool rises at the end of the tool path to avoid collisions with the part.

Limit Definition

Parameter	Description
Side to Machine	Specifies the side to machine.
Stop Position	See Selecting Geometry

Strategy Parameters

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

Machining

Parameter	Description
Machining Mode	Specifies the machining mode. By Area The whole part is machined area by area. By Plane The whole part is machined plane by plane.
Machining Tolerance	Specifies the maximum allowed distance between the theoretical and computed tool path.
Cutting Mode	Defines the tool path style duting machining. Climb Cutting mode where the front of the tool (advancing in the machining direction) cuts into the material first. Conventional Cutting mode where the back of the tool (advancing in the machining direction) cuts into the material first.
Tool Path Style	Defines the tool path style duting machining. Back and Forth The tool path alternates directions during successive passes. Helical Moves the tool in successive concentric passes from the boundary of the area to machine towards the interior. Concentric Builds a safe-cutting trajectory by controlling the engagement of the tool. The created trajectory adapts itself dynamically to ensure a safe cutting at nominal speed. Notes: This strategy is recommended for hard-material milling. In this type of material, the tool needs to be protected. Offset on Part Defines an offset from the part.
Helical Movement	Defines the helical movement. You can select one of the following options: Inward Outward Both
Pocket Tool Path Style	Defines the pocket tool path style. Back and Forth The tool path alternates directions during successive passes. Concentric Builds a safe-cutting trajectory by controlling the engagement of the tool. The created trajectory adapts itself dynamically to ensure a safe cutting at nominal speed. Notes: This strategy is recommended for hard-material milling. In this type of material, the tool needs to be protected.

Radial Strategy Parameters

Parameter	Description
Pass Overlap Mode	Specifies the passs overlap mode: Overlap Ratio Overlap between two passes, given as a percentage of the tool diameter (Tool diameter ratio). Overlap Length Overlap length between two passes. Stepover Ratio Step over between two passes, given as a percentage of the tool diameter ( Tool diameter ratio). Stepover Length Step over length between two passes given by the Maximum distance between pass.
Overlap Length	Specifies the overlap length between two passes. Available only in Overlap Length mode.
Tool Diameter Ratio	Defines the percentage of the tool diameter. Available only in Overlap Ratio and Stepover Ratio modes.
Maximum Distance Between Pass	Specifies the maximum distance between pass. Available in Stepover Length only.
Chaining Strategy	Defines the chaining strategy. None No chaining strategy defined. Part Contouring The tool goes round the area to machine first. Note: In a roughing operation, each area is machined, then there is a contouring pass around each area. This is followed by a contouring pass around the whole part when the remaining material is less than the tool radius. Approach and retract motions are computed for all those tool paths. When Part Contouring is selected, all the tool paths around the part are chained, thus reducing the number of air cuts as there are fewer approaches and retract motions. Radial First Reduces air cut, using a radial strategy first.
Contouring Pass	Adds an end contouring pass to the tool path. This ensures that no material is left at the direction changes between two passes.
Contouring Pass Ratio	Adjusts the position of the contouring pass to optimize scallop removal (given as a percentage of the tool diameter).
Always Stay on Bottom	Forces the tool to remain in contact with the pocket bottom when moving from one domain to another. This avoids unnecessary linking transitions. Note: This parameter becomes available when at least one tool path style is set to Helical or Concentric.
Clearance	Avoids previous motions to remain in contact with the bottom.
	Defines a feedrate on the linking part of these motions.

Axial

Parameter	Description
Maximum Depth of Cut	Depth of the cut affected by the tool at each pass.
Upward Rework Step	This parameter is dedicated to the concentric tool path style in hard material, but can be used for soft materials as well.
Variable Cut Depth	Opens the Variable cut depths dialog box. When the dialog box opens, the distance between passes from the top to the bottom of the part is constant and is the same as Maximum cut depth. Change the Distance from top value and the Max. cut depth value, then press Add to give a different depth value over a given distance.

Zone Parameters

Parameter	Description
Small Pass Filter	Activates the filter for small passes.
Tool Section	Defines the smallest area to machine according to the tool used. Only available when the Small Pass Filter parameter is selected.
Pocket Filter	Activates the filter for small passes. The noncutting diameter of the tool can be entered in the Tool tab when you click More. It is given as information only in the Zone tab. Note: Not all pockets will be machined if there is not enough depth for the tool to plunge. A null value means that tool is allowed to plunge in pockets. The size of the smallest pocket is given below the data field. However, the smallest area to machine is taken into account only if the area detected has no impact on larger areas beneath. The Tool core diameter is taken into account: In pockets (default operating mode) Also for outer parts when limiting contours are used
Automatic Horizontal Areas Detection	Automatically detects horizontal areas on the part. Limits the cutting plane effect to horizontal areas. Applies a dedicated offset on the part for horizontal areas. Detect planar surfaces accessible for the tool. Computes the exact location of the paths on the horizontal area.
Same Offset on Bottom as on Part	Applies the same offset on bottom as on part.
Offset on Areas	Value of the offset to apply on the areas.

High Speed Milling (HSM) Strategy Parameters

Parameter	Description
High Speed Machining	Activates the High Speed Machining parameter.
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.
Corner Radius on Part Contouring	Defines the corner radius of all the tool paths in contact with the part.
Radius	Specifies the radius.

Output Parameters

Parameter	Description
Circular Interpolation	Lets you generate an arc interpolation output when the tool is in contact with a revolution surface (but not with one represented by a CATNurbsSurface). This arc will be propagated to radial paths created by offset of this path, when they exist. By default, this check box is not selected.

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.

See 3/5-Axis Converter

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.
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.
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.

• Automatic
• Pre-Motions
• Post-Motions
• Clearance

Clearance

Two modes are available:

• Along tool axis: When selected, tool retract movements will be along the tool axis all the way to the selected plane. A clearance plane must be selected.
• Optimized: When selected, optimizes tool retract movements. This means that when the tool moves over a surface where there are no obstructions, it will not rise as high as the safety plane. This is because there is no danger of tool-part collisions. As a result, it saves time.
  Notes:

  • Optimized clearance takes the rough stock left by the previous operation into account.
  • If you have defined a safety plane, deactivate Clearance. If you do not, the safety plane will be ignored.

For more information, see NC Machining Apps Common Services: Using the Working Area: Creating Machining Operations: Defining Macros: NC Macros.

Feeds and Speeds Parameters

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

Feedrate

Parameter	Description
Feedrate Unit	Two available feedrate units: Linear Angular
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.
Transition	Activates the transition.
Feedrate Transition	Transition options: Machining Approach Retract RAPID Local
Local Value	Specifies the local feedrate value.
RTCP ON	When selected, activates RTCP mode on transition paths between the previous and current operations.
Slowdown Rate	Defines the slowdown rate.
Spiral Start Rate	Defines the spiral start rate.
Feedrate Reduction in Corners	Defines the feedrate reduction in corners.
Reduction Rate	Defines the reduction rate.
Minimum Angle	Defines the minimum angle value.
Maximum Radius	Defines the maximum radius value.
Distance Before Corner	Specifies the distance before corner.
Distance After Corner	Specifies the distance after corner.

Spindle Speed

Parameter	Description
Spindle Unit	Angular or linear.
Machining Spindle	Defines the speed of the spindle linear/angular advancement.