Sweep Roughing

The Sweep Roughing dialog box appears when you select Sweep Roughing from the Surface Machining section.

This dialog box contains controls for:

This page discusses:

See Also
Creating a Sweep Roughing 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 End Mill tools are available for these operations.

Geometry

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

Mandatory Parameters
Mandatory Parameter Description
Part Selects the part to machine.
Tool Axis Defines the tool axis.
Optional Parameters
Optional 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.
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.

Strategy Parameters

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

Machining
Parameter Description
Machining Direction Defines the tool path direction during machining.
Roughing Type Specifies the rouhng type.

ZOffset The tool path is offset from the part.
ZPlane The part is machined plane by plane. The planes are perpendicular to the tool axis.
ZProgressive The part is machined by interpolating the tool path between the part and the top of a theoretical rough stock.

Tool Path Style Defines the tool path style duting machining.

Zig-zag The tool path alternates directions during successive passes.
One-way Next The tool path always has the same direction during successive passes. The tool goes diagonally from the end of one tool path to the beginning of the next.
One-way Same The tool path always has the same direction during successive passes. The tools returns to the first point in each pass before moving on to the first point in the next pass.

Machining Tolerance Specifies the maximum allowed distance between the theoretical and computed tool path.
Radial Defines the radial strategy parameters:

Distance Between Pass Defines the maximum distance between two consecutive tool paths in a radial strategy.
Step-Over Side Defines step-over side with respect to the machining direction. Can be either to the left or the right of the tool path.

Axial Lets you specify maximum cut depth.

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
  • Between Passes
  • Between Passes Link

When the Activate the intermediate stock check box is selected in the Part Operation, it is processed in approach and retract motions as described in Using Intermediate Stock.

Note: Any Machining Process created in V6R2012x or earlier, and containing at least one Sweep Roughing operation, must be recomputed to take advantage of this capability.

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