ZLevel

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

This dialog box contains controls for:

This page discusses:

See Also
Creating a ZLevel 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
End mill tools , conical tools , TSlotter tools and Barrel tools are available for these operations.
Notes:
  • Barrel tools are not supported by circular interpolation.
  • The TSlotter tool is defined with one corner radius only, the upper corner radius being equal to the corner radius.
  • The TSlotter takes into account a 2D projection of the limiting contour: The limit is considered to be a prism parallel to the tool axis and passing through the limiting contour

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
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 Defines the start point.
Imposed Defines the imposed point.
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.
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 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.

Pass Overlap Specifies pass overlap.
Offset on Tool Path Specify the offset on tool path.
Axial
Parameter Description
Stepover Mode

Specifies how the distance between two consecutive paths is computed:

  • Constant
  • Via scallop Height

Distance Between Paths Defines the maximum distance between two consecutive tool paths in a radial strategy.
Scallop Height Defines scallop height.
Guiding Strategy Helix Reduces motions.
Zone Parameters
Table 1.
Parameter Description
Maximum Horizontal Slope Specifies maximum horizontal slope.
Remove portions of pass in undercut Removes portions of pass in undercut
High Speed Milling (HSM) Strategy Parameters
Table 2.
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.
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.
Approximate passes to optimize circular interpol Approximates the tool passes to optimize a circular interpolation. Specifies the radius used for rounding the corners along the trajectory of an HSM operation. Value must be smaller than the tooltip radius.

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.
See 3/5-Axis Converter
Parameter Description
Remove Motions in Collisions The tool axis is not modified: the tool path stops before the collision point, and the corresponding portion af the tool path is removed.
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).
Automatic The tool axis is automatically computed to avoid collisions.
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.

Lift Tool

Solves the interferences by a minimum lift of the tool along the tool 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.
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
Optimize Machine Rotary Axis If selected, minimizes the variations of rotary degree of freedom, as well as tool axis variations.
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
  • Between Passes
  • Between Passes Link

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.