Sequential Axial and Sequential Groove Operations

The Sequential Axial dialog box appears when you select Sequential Axial and the Sequential Groove dialog box appears when you select Sequential Groove. This dialog box contains controls for:

This page discusses:

See Also
Creating a Sequential Groove Operation with the Legacy Interface
Creating a Sequential Axial Operation with the Legacy Interface

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
Milling tools and Drilling tools are available with these operations (except Barrel Mills ).
See Assigning a Tool Element to a Machining Operation

Geometry

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

Mandatory Parameters
Parameter Description
Hole Selects the part to machine.
Optional Parameters
Optional Parameter Description
Check Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Number of Planes Defines the number of planes. You can then edit each plane.
Other Parameters
Parameter Description
Tool Axis Strategy Defines the tool axis strategy.

Fixed Axis The tool axis orientation is the same for all the selected points.
Variable Axis The tool axis orientation can vary from one point to another.
Normal to PS Axis The tool axis orientation is determined by the normal to the selected part surface.

Projection Mode The reference pattern points are projected onto the selected part surface.
Ordering Mode Defines the ordering mode.

Closest Enables you to obtain the shortest possible tool path.
Manual Enables you to define a numbered sequence.
By Hand A Band Ordering dialog box appears allowing you to obtain a Zig-Zag or One-Way ordering in bands. You can also define bands width.

Jump Distance Allows an extra clearance for moving in Rapid motion between the holes to be drilled whenever this distance is greater than the approach clearance.
Geomery Parameters
Parameter Description
Origin Offset Defines the origin offset.
Diameter Defines the geometry diameter.
Depth Defines the geometry depth.
Inverse Pattern Ordering Reverses the order of machining holes.
Relimit Hole Origin Determines the hole origin according to tool axis.

Strategy Parameters

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

Machining
Parameter Description
Sequential Drilling Mode Defines the sequential drilling mode.

Sequential Axial Defines planes (and offset) or depth value to manage the axial tool path between planes.
Sequential Groove Defines planes, diameters, offsets, or values to manage axial and circular motions.

Power Specifies power options for the operation.

From Tool Assembly The Power value defined in the tool assembly is taken into consideration for that operation.
Fixed This value is specific to the operation and there is no impact of the Power value chosen for tool assembly.
Powered This value is specific to the operation and there is no impact of the Power value chosen for tool assembly.

Approach Clearance Specifies a safety distance along the tool axis for approaching the hole reference.
Machining Tolerance Specifies the maximum allowed distance between the theoretical and computed tool path. Only available with Sequential Groove mode.
Compensation Application Mode Specifies how the corrector type specified on the tool is used to define the position of the tool.

Guiding Point The tool motion is computed according to the tool compensation point and the tool compensation point is generated in the output file..
Output Point The tool compensation point is generated in the output file. The tool path computation is generated according to the tool tip.

Compensation Output Manages the generation of Cutter compensation (CUTCOM) instructions in the NC data output. Available for Sequential Groove mode only.

None Cutter compensation instructions are not automatically generated in the NC data output.
2D Radial Profile Both the tool tip and cutter profile are 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.
2D Radial Tip The tool tip is 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.

Automatic ROTABL Generates rotation motions between drilling points that have different tool axes.
Output CYCLE Syntax Generates the output in CYCLE mode.
Main Strategy Parameters
Enables you to specify the following features:
  • Spindle Speed
  • Spindle Stop
  • Delay
  • Go To Plane
  • PP Word
  • Go Delta
  • Go To Clearance
  • Circular
  • Helical
Each feature is editable through its own dialog box.
You can navigate in the features table using the commands Up , Down, and remove any features using the command Remove.

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

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.
Rapid Approach Feedrate Activates the RAPID value set on the machine.
Plunge Feedrate Specifies the feedrate on plunge motions.
Rapid Plunge Feedrate Activates the RAPID value set on the machine.
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.
Spindle Speed
Parameter Description
Spindle Unit Angular or linear.
Machining Spindle Defines the speed of the spindle linear/angular advancement.