Cavities Roughing

The Cavities roughing dialog box appears when you select Cavities roughing from the Surface Machining section.

This dialog box contains controls for:

This page discusses:

See Also
Creating a Cavities 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
Parameter Description
Part Selects the part to machine.
Rough Stock Defines the block of raw material to be machined to produce the part.
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.
Start Points Defines the start point.
Imposed Plane Defines the plane that the tool must obligatorily pass through.
Imposed Plane 2 Defines the second plane that the tool must obligatorily pass through.
Zone Order Sets the order in which the zones on the part are machined.
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.
Start Points
There are specific conditions for start points:
  • They must be outside the machining limit. Examples of machining limits are the rough stock contour, a limit line, an offset on the rough stock, an offset on the limit line, etc.
  • They must not be positioned so as to cause collisions with either the part or the check element. If a start point for a given zone causes a collision, the tool will automatically adopt ramping approach mode.
  • The distance between the start point and the machining limit must be greater than the tool radius plus the machining tolerance. If the distance between the start point and the machining limit is greater than the tool radius plus the safety distance, the start point will only serve to define the engagement direction.
  • If there are several start points for a given area, the one that is used is the first valid one (in the order in which they were selected) for that area. If there are several possible valid points, the nearest one is taken into account.
  • One start point may be valid and for more than one area.
  • If a limit line is used, the tool will approach outer areas of the part and pockets in ramping mode. towards the outside of the contour. The tool moves from the outside towards the inside of this type of area. In this case, you must define the start point.
  • When Tool path style is set to Concentric, start points are automatically defined. In this case, the start point is the center of the largest circle that can be described in the area to machine. Lateral approach modes cannot be used.
  • When Tool path style is set to Helical, whenever possible, the end of the engagement associated to the start point corresponds to the beginning of the sweeping path.
  • If this is not possible, the path will be cut to respect the constraint imposed by the start point.
Note: If you use a limit line or if you use an inner offset on the rough stock, the start point may be defined inside the initial rough stock. The rules concerning the domain of the contour line or the offset on the rough stock contour line above must be applied.

Strategy Parameters

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

Machining
Parameter Description
Machining Mode Specifies the machining mode.

By Plane The whole part is machined plane by plane.
Pockets Only Only pockets on the part are machined.
Outer Part Only the outside of the part is machined.
Outer part & Pockets The whole part is machined external area by external area and pocket by pocket.

Machining Tolerance Specifies the maximum allowed distance between the theoretical and computed tool path.
Cutting Mode Specifies the position of the tool regarding the surface to be machined.

Climb The front of the tool (advancing in the machining direction) cuts into the material first.
Conventional The back of the tool (advancing in the machining direction) cuts into the material first.
Either Either of the two possibilities may be used depending on which is most suitable to the current cutting action.

Machining Direction Defines the tool path direction during machining.
Tool Path Style

Helical Moves the tool in successive concentric passes from the boundary of the area to machine towards the interior.
Concentrics 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.
Back and Forth Alternates between one direction and its opposite.

Contouring Pass Only available with Back and Forth. Sets one of the following contouring style options:
  • After Back and Forth
  • Prior to Back and Forth
Contouring Pass Ratio Only available with Back and Forth. Specifies contouring pass ratio.
Radial Strategy Parameters
Parameter Description
Pass Overlap Specifies pass overlap.
Tool Diameter Ratio Specifies the tool diameter ratio.
Axial
Parameter Description
Maximum Cut Depth Specifies the maximum cut depth the tool can realize during machining.
Variable Cuth Depth Defines variable cut depth.
Zone Parameters
Parameter Description
Remaining Thickeness For Side Specifies remaining tickness for side.
Minimum Thickness on Horizontal Areas Specifies the minimum thickness on horizontal areas.
Machine Horizontal Areas Until Minimum Thickness Enables machining of horizontal areas until minimum thickness.
Pocket Filter Activates the filter for small passes.
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.
  • The Smallest area to machine is taken into account only if the area detected has no impact on larger areas beneath.
High Speed Milling (HSM) Strategy Parameters
Parameter Description
High Speed Milling Specifies whether or not cornering for HSM is to be done on the trajectory.
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.
Cornering on Part Contouring Pass Enables cornering on part contouring pass.
Corner Radius on Part Contouring Pass Specifies the radius used for rounding the corners along the part contouring pass of an HSM operation.
Output Parameters
Parameter Description
Circular Interpolation Activates the arc interpolation output, when possible:
  • When the tool is in contact with a revolution surface with its axis parallel to the tool axis.
  • In the cornerization circular path.
  • And in circular motions of the macro.

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.
Finishing Feedrate Specifies the finishing feedrate.
Transition Activates the transition.
Feedrate Transition Transition options:
  • Machining
  • Approach
  • Retract
  • RAPID
  • Local
Slowdown Rate Reduces the current feedrate by a given percentage.
Spiral Start Rate Specifies the spiral start rate.
Feedrate Reduction in Corners Reduces 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
Parameter Description
Spindle Unit Angular or linear.
Machining Spindle Defines the speed of the spindle linear/angular advancement.