Isoparametric Machining

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

This page discusses:

See Also
Creating Isoparametric Machining Operations

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
For Multi-Axis Tube Machining operations, the following tools are available:
  • End Mill tools
  • Conical tools
  • Lens Mill tools
  • Face Mill tools
  • TSlotter tools
  • Barrel tools
Note: When you use barrel cutter tools, you can define the end flat diamater of the tool with the DFLAT parameter.

Geometry

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

Mandatory Parameters
Mandatory Parameter Description
Parts Selects the parts 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).

Strategy Parameters

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

Machining
Parameter Description
Tool Path Style Defines the tool path style during machining.

Zig-zag The tool path alternates directions during successive passes.
One-way The same machining direction is used from one path to the next.

Machining Tolerance Specifies the maximum allowed distance between the theoretical and computed tool path.
Note: The machining tolerance influences the distance between two consecutive paths. When the machining tolerance value is increased, the distance between two consecutive paths is decreased according to the specified maximum scallop height value.
Maximum Discretization Step Ensures linearity between points that are far apart.
Maximum Discretization Angle Specifies the maximum angular change of tool axis between tool positions.
Notes:
  • Maximum discretization step and Maximum discretization angle influence the number of points on the tool path.
  • Choose their value carefully to avoid a high concentration of points along the tool trajectory.
  • These parameters also apply to macro paths that are defined in machining feedrate. They do not apply to macro paths that do not have machining feedrate (RAPID, Approach, Retract, User, and so on).
Radial Parameters
Parameter Description
Stepover

Specifies how the distance between two consecutive paths is computed:

  • Via scallop Height
  • Distance on Part
  • Number of Paths

Scallop Height Defines scallop height.
Maximum Distance Between Paths Defines the maximum distance between two consecutive tool paths in a radial strategy.
Number of Paths Defines the number of tool paths when the Number of Pathsstepover strategy is defined.
Skip Path Defines skip path. You can select one of the following options:
  • None
  • First
  • Last
  • First and Last
Start Extension Specifies the length of an additional machined area located before the first path on part.
End Extension Specifies the length of an additional machined area located after the last path on part.
Tool Axis Strategy Parameters
Important: Modifications of the tool axis generated by the mode you have selected apply only to the machining passes, not to the between paths passes.
Parameter Description
Tool Axis Mode

Fixed Axis The tool axis arrow proposes a context menu:
  • Select: Defines the tool axis.
  • Analyze: Starts the Geometry Analyzer.
Interpolation The tool axis is interpolated between two selected axes.
Lead and Tilt The tool axis is normal to the part surface with respect to a given lead angle (alpha) in the forward tool motion and with respect to a given tilt angle (beta) in the perpendicular direction to this forward motion.
Optimized Tilt The tool axis is allowed to vary from the specified Lead angle within an allowed range.
4 Axis Lead/Lag The tool axis is normal to the part surface with respect to a given lead angle in the forward direction and constrained to a specified plane.
4 Axis Tilt The tool axis is normal to the part surface with respect to a given Tilt angle and is constrained to a specified plane.
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.
Normal to Line The tool axis passes through a specified curve, and is normal to this curve at all points.
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 Drive Surface The tool axis remains normal to the drive surface with respect of a lead angle.
Rolling Drives the contact point position along the side radius of the tool. You can select one of the following option:
  • Fixed: the contact position is kept fixed along the side radius.
  • Fixed and Tool Retract: the contact point is fixed and linking motions are created when this contact point position generates collisions.

Tool Axis Parameters

Collisions Checking
Parameter Description
Activate collisions checking Activates or deactivates collisions checking.
Collision checking strategy Defines the strategy: Automatic or Removes Motions on Collisions.
Part, Check Enables collision checking on one or multiple elements.
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.
Maximum Angle Defines the maximum angle range within which the tool axis can vary.
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
  • Return in a Level Retract
  • Return in a Level 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.
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 Defines the speed of linear/angular advancement of the tool during finishing.
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.