Power Machining

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

This dialog box contains controls for:

This page discusses:

See Also
Creating a Power Machining on the Center
Creating a Power Machining on the Side
Optimizing a Power Machining 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.
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.

Strategy Parameters

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

Machining
Parameter Description
Machining Strategy Two machining strategies are available.

Center(1) only Provides a roughing of the center of the part.
Center(1) and Side(2) Provides a ZLevel finishing of the sides in addition to the roughing of the centers.

Machining Mode Specifies the machining mode.

By Plane The whole part is machined plane by plane.
By Area The whole part is machined area by area.

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.

Optimize Machining Direction Optimizes machining direction.
Machining Direction Sets machining direction.
Center Parameters
Parameter Description
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.

Helical Movement Only available with Helical Movement. Sets one of the following helical movement options:
  • Both
  • Inward
  • Outward
Stay on Bottom Forces the tool to remain in contact with the pocket bottom when moving from one domain to another.
Part Contouring Lets the tool machine the outside contour of the part.
Movement Only available with Concentric. Sets one of the following concentric movement options:
  • One-Way
  • Zig-Zag
Contouring Style 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.
Pass Overlap Mode Specifies one of the following parameters.

Overlap Ratio The overlap between two passes, given as a percentage of the tool diameter.
Overlap Length The overlap between two passes, given as a distance.
Step Over Ratio The step over between two passes, given as a percentage of the tool diameter.
Step Over Length The step over between two passes, given as the maximum distance between passes.

Tool Diameter Ratio Specifies the tool diameter ratio. This is available when Overlap ratio is selected as Step over.
Side Parameters
Parameter Description
Bottom Finish Thickness on Side Specifies the bottom finish thickness on side.
Compensation Output Specifies the compensation output.
Maximum Cut Depth on Side Specifies depth of the cut done by the tool at each pass.
Zone Parameters
Parameter Description
Remaining Thickeness For Side Specifies remaining thickness for side.
Important: Be very careful when using the Remaining thickness for sides. Refer to About Power Machining on 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 Enables pocket filter.
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.

Table 1. 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
Table 2. Spindle Speed
Parameter Description
Spindle Unit Angular or linear.
Machining Spindle Defines the speed of the spindle linear/angular advancement.