Groove Milling

The Groove Milling dialog box appears when you select Groove Milling. This dialog box contain controls for:

This page discusses:

See Also
About Groove Milling Tool Path Concepts
Creating a Groove Milling Operation

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
Only TSlotter 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.
Tool Axis Defines the tool axis.
Optional Parameters
Optional Parameter Description
Bottom Defines the lowest plane machined on the part.
Guide Specifies the guide of the machining operation.
Top Defines the highest plane machined on the part.
Tool Axis Defines the tool axis.
Other Parameters
Optional Parameter Description
Material Side Selects the material side.Available for Between Two Planes, Between Two Curves and Between Curve and Surfacesmodes only.
First Relimiting Element Defines the starting point of the relimiting element.
Limit 1 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.
Limit 2 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
Soft Boundary Lets you select a soft boundary and define an offset on the boundary.
Check Specifies the check elements with an optional offset.
Bottom Specifies the bottom type on planar faces or on a surface: Hard or Soft.
Top Specifies the top plane with an optional offset. Available for Between Two Planes mode only.

Strategy Parameters

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

Machining
Parameter Description
Tool Path Style Defines the tool path style duting machining.

Zig-zag The tool path alternates directions during successive passes.
One-way The same machining direction is used from one path to the next.

Sequencing Defines the first axe to machined. You can select Radial First or Axial First.
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.
Close Tool Path Specifes whether or not the program must close the tool path.
Percentage 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

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 on Bottom Specifies the tool corrector identifiers used in the operation. This point is switched automatically during a Return between levels macro whenever the next level to machine requires a different compensation point. 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.
Radial Strategy Parameters
Parameter Description
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.
Axial Strategy Parameters
Parameter Description
Axial Strategy Defines how the tool path is ordered for machining the groove/ You can select the following options:
  • Standard
  • Middle
  • Middle Alternate
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.
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 each level
  • Top and/or bottom finish
  • Side and top and/or bottom finish

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.
Top/Bottom Finish Thickness Specifies the thickness of material that is machined when finishing the top/bottom of the groove.
Bottom Finish Thickness Specifies the thickness of material that is machined by the bottom finish pass.
Bottom Finish Path Style Defines the finish path style for the top and bottom finish passes. Y
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.

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
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.

  • Approach
  • Retract
  • Clearance
  • Linking Retract
  • Linking Approach
  • Returnn in Level Retract
  • Returnn in Level Approach
  • Return Finish Pass Retract
  • Return Finish Pass Approach
  • Return Between Levels Retract
  • Return Between Levels Approach

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

Type Defines the transition type. You can select one of the following types:
  • Machining
  • Approach
  • Retract
  • RAPID
  • Local
  • Finishing
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.
Feedrate Reduction in Corner 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
  • Distance before corner
  • Distance after corner
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.