Multi-Axis Helix Machining

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:

Multi-Axis Helix Machining: Strategy Parameters

Multi-Axis Helix Machining: Machining Parameters

	Direction of cut Specifies how machining is to be done.
	In Climb milling, the front of the advancing tool (in the machining direction) cuts into the material first. In Conventional, the rear of the advancing tool (in the machining direction) cuts into the material first.
	Machining tolerance 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).

Multi-Axis Helix Machining: Radial Parameters

	Stepover 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.
	Scallop height 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.
	Skip path Gives the possibility of not machining the path on the first contour, the path on the last contour, or both these paths.

Multi-Axis Helix Machining: Tool Axis Parameters

Tool axis mode
Specifies how the tool axis is to be guided: Lead and Tilt, 4-axis Tilt or Interpolation.

Lead and Tilt

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:

Fixed lead and tilt: Here both the lead and tilt angles are constant.

Variable lead and fixed tilt: Here the tool axis is allowed to move from the specified lead angle within a specified range, the tilt angle remaining constant.

Fixed lead and variable tilt: Here the tool axis is allowed to move from the specified tilt angle within a specified range, the lead angle remaining constant.

Lead angle
Specifies a user-defined incline of the tool axis in a plane defined by the direction of motion and the normal to the part surface. The lead angle is with respect to the part surface normal.

Maximum lead angle
Specifies a maximum lead angle.

Minimum lead angle
Specifies a minimum lead angle.

Tilt angle
Specifies a user-defined incline of the tool axis in a plane normal to the direction of motion. The tilt angle is with respect to the part surface normal.

Allowed tilt
Specifies the range of allowed tilt variation.

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. 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.

Interpolation

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.

The orientation of an axis is adjusted by means of the Axis Definition dialog box.

Manual. Choose one of the following:
- Components to define the orientation by means of I, J and K components.
- Angles to define the orientation by means of a rotation of the X, Y or Z axis. The rotation is specified by means of one or two angles.
  
  When the Angles option is selected, the drop down list proposes by default an item specific to interpolation axes: Lead (Angle1) & Tilt (Angle 2).
  
  The tilt angle is the angle between the interpolation axis and the normal to the part (N) in the plane (N,NxM).
  The lead angle is the angle between the interpolation axis and the normal to the part (N) in the plane (N,M).
  
  Other proposed angle options are:
  - Angle 1 about X, Angle 2 about Y
  - Angle 1 about Z, Angle 2 about X
  - Angle 1 about Y, Angle 2 about Z
  Key in the desired angle values in the Angle 1 and Angle 2 fields.
Selection. If you select a line or linear edge, the tool axis will have the same orientation as that element. If you select a planar element, the tool axis will be normal to that element.
Points in the View. Just select two points to define the orientation.

The tool axis is visualized by means of an arrow. The direction can be reversed by clicking Reverse Direction in the dialog box.

You can select the Display tool checkbox to display the tool and check that the tool is correctly orientated. Note that the tool will be displayed according to the tool tip point (and not the contact point).

Once Display tool is selected, Check Interferences becomes available. Click it to start checking interferences between the complete tool assembly and the part and check, if any.

If no interferences are found, the status light on the left turns green.
If interferences are found it turns red. They are displayed in red by the intersection of the tool with the surface in collision.

Check Interferences is available only when the operation parameters are coherent.

Just click OK to accept the specified tool axis orientation.

Multi-Axis Helix Machining: Cutter Compensation Parameters

In the Machine Editor, the Compensation tab contains options for:

globally defining the 3D contact cutter compensation mode: None/Contact/Tip and Contact
imposing the compensation mode to all operations supporting the selected mode whatever the choice defined at machining operation level.

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.

Compensation output
Allows you to manage the generation of Cutter compensation (CUTCOM) instructions in the NC data output:

The following options are proposed:

3D Contact (G29/CAT3Dxx)
None.

3D Contact (G29/CAT3Dxx)

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.
Example of generated APT source:

$$ Start generation of : Multi-Axis Helix Machining.1 FEDRAT/ 1000.0000,MMPM SPINDL/ 70.0000,RPM,CLW CUTCOM/NORMPS $$ START CUTCOM NORMPS XC, YC, ZC, XN, YN, ZN, I, J, K .../... CUTCOM/OFF $$ END CUTCOM NORMPS XC, YC, ZC, XN, YN, ZN, I, J, K $$ End of generation of : Multi-Axis Helix Machining.1

None

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.

Multi-Axis Helix Machining: Geometry

You can specify the following Geometry:

Part elements (faces) with possible Offset on Part.
Faces must be continuous in tangency in order to ensure good quality tool paths.
Four limiting curves comprising:
- Upper and lower contours, which must be closed contours. The selected curves must lie on faces.
- Leading and trailing edges, which must intersect the upper and lower contours. The selected curves must lie on faces.
A Start or a Stop point, which specifies the entry or the exit point of the helix. When one point is selected, the other point is automatically deduced.
Optionally, check elements with possible Offset on Check.

Multi-Axis Helix Machining: Collision Checking

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.

Collisions with Check Elements

The parameters involved for check elements (such as fixtures) are described below.

Check (or Fixture) accuracyDefines 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.

Allowed gouging
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.

Collisions with Part Elements

To activate collision checking on part elements, you must select the Active checkbox.

Part accuracyDefines 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.

Allowed gouging
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.

Concave and non smooth part milled with 0 degree Lead angle

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.

Convex part machined with ball, flat or filleted ended tool or with a Fixed or Variable tool axis mode.

Concave part milled with 0 degree Lead angle.

A "Nothing to Mill" message may be issued.

Multi-Axis Helix Machining: Tools

Recommended tools for Multi-Axis Helix Machining are End Mills, Face Mills, Conical Mills and T-Slotters.

Multi-Axis Helix Machining: Feeds and Speeds

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.

Multi-Axis Helix Machining: NC Macros

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.