The information in this section will help you create and edit Multi-Axis Helix Machining operations in your manufacturing program.
Click the icon, then select the geometry to be machined . A number of collision checking parameters can be set on the Geometry tab page.
A number of strategy parameters are available for defining:
Specify the tool to be used , feeds and speeds , and NC macros as needed.
For more information about how to specify this type of operation please refer to:
Direction of cut
Specifies how machining is to be done.
Specifies the maximum allowed distance between the theoretical and computed tool path.
Maximum discretization step
Defines the maximum allowed distance between two points on the tool path. It is used to ensure linearity between points that are far apart. Default value is 100 m.
Maximum discretization angle
Specifies the maximum angular change of tool axis between tool positions. It is used to add more tool positions (points and axis) if value is exceeded. Default value is 180 degrees.
Note: The Maximum discretization step and Maximum discretization
angle influence the number of points on the tool path. The values
should be chosen carefully if you want to avoid having 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).
Defines the criteria to be used for distributing the turns of the generated helix: by scallop height, distance between turns, or number of turns.
Note that the machining tolerance influences the distance between two consecutive turns.
For example, when the machining tolerance value is increased, the distance between two consecutive turns is decreased according to the specified scallop height value.
Specifies the maximum scallop height between consecutive turns of the generated helix in the radial strategy.
Distance between turns
Defines the maximum distance between consecutive turns of the generated helix in the radial strategy.
Number of turns
Defines the number of turns of the generated helix in the radial strategy.
Gives the possibility of not machining the path on the first contour, the path on the last contour, or both these paths.
Tool axis mode
Specifies how the tool axis is to be guided: Lead and Tilt, 4-axis Tilt or Interpolation.
In this mode the tool axis is normal to the part surface with respect to a given lead angle (a) in the forward tool motion and with respect to a given tilt angle (B) in the perpendicular direction to this forward motion.
There are several types of lead and tilt modes as follows:
The tool axis is normal to the part surface with respect to a given tilt angle and is constrained to a specified plane. This mode has the same behavior as Lead and Tilt except that the local normal to the part is replaced by a normal to plane constraint. You can specify a Lead Angle and a Tilt angle.
For example, this mode is dedicated to milling parts with tool axis nearly parallel to the part itself (near flank milling). It is primary intended for NC machines whose configuration is A+C, but it can be used on any other multi-axis machine.
In this mode the tool axis is interpolated between selected axes. Four default interpolation axes are proposed initially. The orientation of these axes can be adjusted by the user. Additional axes can be inserted anywhere on the area to machine to ensure that the tool can be positioned at each point on the trajectory and that the trajectory is collision-free.
In the Machine Editor, the Compensation tab contains options for:
If the options are set as follows, compensation can be managed at machining operation level.
In this case a Compensation tab appears in the Strategy page of the machining operation editor, and the following options are available.
Allows you to manage the generation of Cutter compensation (CUTCOM) instructions in the NC data output:
The following options are proposed:
The tool contact point will be visualized during tool path
replay. Cutter compensation instructions are automatically generated
in the NC data output. An approach macro must be defined to
allow the compensation to be applied.
Cutter compensation instructions are not automatically generated in the NC data output. However, CUTCOM instructions can be inserted manually. For more information, please refer to How to generate CUTCOM syntaxes.
You can specify the following Geometry:
This section shows how collision checking is managed in Multi-axis Helix Machining operations. The Collision Checking parameters are accessed in the Geometry tab page of the operation's dialog box.
Collision checking can be performed on check and part elements with the tool assembly (that is, the complete shape of the cutter plus its holder) or the cutting part of the tool (red part of following tools):
To save computation time, you should use the tool assembly only if the geometry to be checked can interfere with the upper part of the cutter.
The parameters involved for check elements (such as fixtures) are described below.
Check (or Fixture) accuracy
Defines the maximum error to be accepted with respect to the fixture with its offset. Setting this parameter to a correct value avoids spending too much computation time to achieve unnecessary precision.
Offset on check
Defines the minimum distance between the cutter and the fixture, used to limit the tool path.
Defines the maximum cutter interference with the fixture during "linking passes" (including approach and retract motion).
The illustration below shows return motion with no macro or jump.
The illustration below shows return motion with macro between path and fixture.
To activate collision checking on part elements, you must select the Active checkbox.
Defines the maximum error to be accepted with respect to the part with its offset. This parameter is set to the machining tolerance value. It can be only be changed by modifying the machining tolerance.
Defines the maximum cutter interference with the part during "linking passes" (including approach and retract motion).
In Multi-axis Helix Machining, collision checking with part elements is useful in the following case.
Note that Allowed gouging must be set to a non zero value, otherwise a "Nothing to Mill" message may be issued.
In Multi-axis Helix Machining, collision checking on part elements is not useful in the following cases.
A "Nothing to Mill" message may be issued.
Recommended tools for Multi-Axis Helix Machining are End Mills, Face Mills, Conical Mills and T-Slotters.
In the Feeds and Speeds tab page, you can specify feedrates for approach, retract and machining as well as a machining spindle speed.
Feedrates and spindle speed can be defined in linear or angular units.
A Spindle output checkbox is available for managing output the SPINDL instruction in the generated NC data file. If the checkbox is selected, the instruction is generated. Otherwise, it is not generated.
Feeds and speeds of the operation can be updated automatically according to tooling data and the Rough or Finish quality of the operation. This is described in Update of Feeds and Speeds on Machining Operation.
You can define transition paths in your machining operations by means of NC Macros. These transition paths are useful for providing approach, retract and linking motion in the tool path.
An Approach macro is used to approach the operation start point.
A Retract macro is used to retract from the operation end point.
A Linking macro may be used in various cases (for example, to link two non consecutive paths).
A Clearance macro can be used in a machining operation to avoid a fixture, for example.