Multi-Axis Flank Contouring Operations

The information in this section will help you create and edit Multi-Axis Flank Contouring operations in your manufacturing program.

Select the Multi-Axis Flank Contouring operation icon then select the geometry to be machined.

A number of strategy parameters are available for defining:

• machining criteria
• axial and radial stepover conditions
• finishing
• tool axis guidance
• high-speed milling
• cutter compensation.

Specify the tool to be used , feeds and speeds , and NC macros as needed.

The following user tasks illustrate some of this operation's capabilities:

• Tanto Fan tool axis mode
• Combin Tanto tool axis mode
• Local modifications
• Non-contiguous drives.

Multi-Axis Flank Contouring: Strategy Parameters

Multi-Axis Flank Contouring: Machining Parameters

Multi-Axis Flank Contouring: Stepover Parameters

Multi-Axis Flank Contouring: Finishing Parameters

Multi-Axis Flank Contouring: Tool Axis Parameters

Tool axis guidance Specifies how the tool axis is to be guided.
Tanto Fan: The tool is tangent to the drive surface at a given contact height, and the tool axis is interpolated between the start and end positions.
Combin Tanto: This strategy combines three phases: tool fans over a given Leave distance tool is tangent to the drive surface at a given Contact height and is contained in a plane normal to forward direction tool fans over a given Approach distance.
Combin Parelm: This strategy combines three phases: tool fans over a given Leave distance tool is tangent to the drive surface at a given Contact height and follows the surface isoparametrics tool fans over a given Approach distance.
Mixed Combin: Either Combin Parelm or Combin Tanto is applied depending on the drive surface geometry. Combin Tanto is applied for cylindrical and planar drives. Combin Parelm is applied for other drive surface geometry.
Fixed: The orientation of the tool axis is fixed.
Normal to Part: The tool axis remains normal to the Part Surface while the tool remains in contact with the drive surface.
Tanto: This mode can only be assigned locally to a drive and not globally to the operation. The tool is tangent to the drive surface at a given contact height, and the tool axis is contained in a plane normal to forward direction.
Contact height Determines a point on the drive surface where the tool must respect tangency conditions. The Contact height is measured from the tool tip along the tool axis. The point on the drive is computed such that its projection normal to the drive onto the tool axis respects the Contact height value.
Leave fanning distance Specifies a distance at the start of a motion over which tool fanning takes place.
Approach fanning distance Specifies a distance at the end of a motion over which tool fanning takes place.
Disable fanning For operations with Combin Tanto, Combin Parelm and Mixed Combin tool axis guidance, it is possible to disable fanning at Start element, at Stop element, or at both these limiting elements.
Control fanning using tool parameter When this option is selected, a Useful cutting length can be defined on the current tool. This parameter is helpful for controlling tool fanning or the offset distance when approaching drive surfaces with negative draft angles, without needing to modify the tool chosen in the database. Otherwise, the default standard cutting length value (Lc) of the tool will be used.
An auxiliary guide curve can be selected in order to modify the tool axis strategy. It is mainly used to avoid collisions at the top of drive elements or to keep a safety distance on these elements. The following parameters can be used if a guide curve is selected the guide curve. Position on guide curve Tool positioning with respect to the guide curve: Auto/Right/Left/On. Auto lets the program determine the best position regarding the curve. Offset on guide curve Offset to be applied to the guide curve. Use of guide curve Tool can be made to respect the guide curve either Always or If needed (that is, only where there is a risk of collision with the drive element). For example, for the following geometry:
A collision occurs if top auxiliary guide curve is not defined:		Collision is avoided if top auxiliary guide curve is defined:

Multi-Axis Flank Contouring: High Speed Milling (HSM) Parameters

In a Multi-Axis Flank Contouring, cornering for HSM applies to all corners for machining or finishing passes. It does not apply to macros or default linking and return motions.

Cornering Specifies whether or not cornering is to be done on the trajectory for HSM.

Corner radius Specifies the radius used for rounding the corners along the trajectory of a HSM operation. Value must be smaller than the tool radius.

Cornering on side finish path Specifies whether or not tool path cornering is to be done on side finish paths.

Corner radius on side finish path Specifies the corner radius used for rounding the corners along the side finish path of a HSM operation. Value must be smaller than the tool radius.

Multi-Axis Flank Contouring: 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.

Multi-Axis Flank Contouring: Geometry

You can specify the following Geometry:

• Part with possible Offset on Part
  See note below about negative part offset and collision checking on checks.
• Drives surfaces with possible Offset on Drive.
• Start and Stop limiting elements with possible Offset on Start and Offset on Stop.
  The tool can be positioned with respect to the start and Stop elements by selecting one of the proposed options: On, In, Out, or Tangent to Drive.
• Fixture or check elements with possible Offset on Check.
• Offset along Tool Axis.

Drive Elements

Surfaces or planes can be selected and they are taken into account according to their order of selection. The tool path starts on the first drive and ends on the last drive, except when Close tool path is set (in this case, the first drive is also used as the last drive).

The Face Selection toolbar appears to help you select faces or belts of faces.

Please refer to Face Selection for a description of these commands.

For some parts, you may need to select the same face as a drive element more than once. For this, you can use Multi-selection of Contours , which allows multi-selection of faces when selecting drive elements.

In this case, the same drive has more than one annotation. To improve visualization of selected drives, the annotation is positioned at the edge (and not in the middle) of the drive.

Note that, when selecting drives, a warning message may appear about the possible creation of a second belt of faces if you forget to select a face.

Drives can be adjusted using the Local Modifications contextual command. For example, this allows you to make the following local modifications to a drive:

• use a different guiding strategy
• set different offsets
• imposed a 4-axis constraint.

The program automatically determines the stopping and restarting conditions between contiguous drives. If drives are not adjacent, those values must be set manually with the Local Modifications capability. The program automatically detects fillets and joggles (features comprising 3 contiguous drives) to manage the choice of suitable elements for stopping.

Use Curves as Part

You can select edges that are boundaries of the drive elements as part elements. To do this, right click the part surface area in the sensitive icon and select the Use Curves as Part contextual command.

Start and Stop Elements

You can select vertices, edges, planes and faces as limiting elements. If a vertex or edge is selected, a virtual plane is computed on the vertex or at the middle of the edge perpendicular to the current drive and part.

You can right click the start or stop element in the sensitive icon and select the Switch contextual command to swap the Start and Stop labels on the selected elements. This does not reverse the direction of the tool path.

Start Position and Optional Reference Point

A typical start element is a plane/almost planar surface that is normal to the drive, and normal to the part. This allows the program to use an automatic reference point.

It is recommended to select an edge or vertex that will automatically simulate a correct plane.

In the case of a manually selected reference point, you have to imagine that the tool makes a virtual move from a Reference position to the Start position, which is the end position of that move. The Reference position is defined by the reference point and the tool axis at that point.

The tool move moves from the Reference position to an intermediate position then on to the Start position when Part, Drive and Check surfaces are specified.

The intermediate position is defined as being the normal projection of the Reference point on the Drive surface.

Reference position is not taken into account for tool path computation of the machining operation. It is only a reference location that helps to specify the Start position related to the Part, Drive and potentially Check surfaces that are specified by the user.

Expected results are obtained by respecting a reference position close to this end location (but at a distance greater than the tool radius value).

Selecting the fillet of the joggle as starting element is not a good choice. Because the elements are always seen as infinite, the extension of this fillet is parallel to the first drive. If these two elements do not have a common boundary, select a starting element whose extensions are not parallel to the drive (drive also seen as infinite).

Local Drive Surface Conditions

Local Restarting direction: Auto / Left / Right / Forward. This is a relative direction, seen from a cutter point of view. You should set the value according to the direction of the cutter at the end of the previous motion. In Auto mode, the program applies either Left, Right or Forward according to local geometry conditions.

Local Stopping condition: Auto / To / On / Past / Tangent DS. You should set the value according to how you want the cutter to reach the next drive. In Auto mode, the program applies either To, Past or Tangent DS according to local geometry conditions. In some cases, the stopping condition may be ignored (for example, if the drive to reach is located after the Past position of the current drive).

Local Tool side on drive: Same as first / Swap / On. You should keep in mind that the reference side is the one set on the first drive as indicated by the displayed arrow. This parameter is predominant compared the local Stopping condition.

Stopping and Restarting conditions must be defined on non contiguous drives.

User defined settings may lead to bad tool paths. So you should ensure the consistency of the chosen collection of drive surfaces. For example, a gap between the end of a motion and the beginning of the next motion would generate a simple straight-line path, which is generally not suitable.

In order to machine some gaps, you may have to create extra geometry. A typical example is two drive elements that are tangent but not contiguous, lying on the same surface.

Geometry and Tool

Keep in mind that a geometric element is always extended to infinity, vertically and horizontally.

The cutting length of the tool should not be too great compared to the height of the drives. This can lead to bad results or failure in corners.

For negative draft angles the top of the cutting part of the tool is taken into account to define the fanning areas, if necessary along the vertical extension of the drive.

It is preferable to specify the cutting length of the tool in the Useful cutting length parameter.

Geometry Recommendations

Do not set the Close tool path option if the first drive is not to be machined as the last drive also.

Do not use a manual reference point if its use is not clearly defined. Prefer an automatic reference point, using a plane/planar surface as start element, normal to the drive1 and normal to the part (select an edge or a vertex that will simulate this plane without geometry creation).

Use a cutter whose cutting length (Lc) is nearly the height of the drive elements (use the Useful cutting length parameter, do not modify the tool).

Always keep in mind that all geometrical elements are seen as infinite elements, extended in all directions: horizontal and vertical. Also drive elements are machined in the order of selection, one after another.

Select the OUT condition to end after a joggle, or use a plane/edge/vertex as end element.

If a negative part offset is used and its absolute value is bigger than the tool body radius,
this is not compatible with collision checking on checks.
If you really want to perform collision checking on checks you must use a smaller negative offset on parts.
Otherwise unselect check elements.

Multi-Axis Flank Contouring: Tool

Recommended tools for Multi-Axis Flank Contouring are End Mills and Conical Mills.

Multi-Axis Flank Contouring: 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 of 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.

Feedrate Reduction in Corners

You can reduce 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, and distances before and after the corner.

Feed reduction is applied to corners along the tool path whose radius is less than the Maximum radius value and whose arc angle is greater than the Minimum angle value. Corners can be angled or rounded.

For Multi-Axis Flank Contouring, feedrate reduction applies to inside corners for machining or finishing passes. It does not apply to macros or default linking and return motions.

If a cornering is defined with a radius of 5mm and the Feedrate reduction in corners is set with a smaller radius value, the feedrate will not be reduced.

Feedrate Reduction in Corners Combined with Local Slowdown Rate

If the Feedrate reduction in corners option is selected and local Slowdown rates are applied to drives, the general rule is that the corner feedrate Reduction rate is applied after the local Slowdown rate on the current feedrate. For a machining feedrate the feedrate will be equal to (machining feedrate * local Slowdown rate * corner Reduction rate).

For example if the local Slowdown rate is 80% on the first drive, 40% on the second drive and the corner feedrate Reduction rate is 50%, the feedrate sequence is:

• 80% then 40% along the first drive
• 20% then 40% along the second drive.

Feedrate reduction in corners with no Local Slowdown on drives:

Feedrate reduction in corners combined with Local Slowdown on drives:
 

Multi-Axis Flank Contouring: 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 several cases, for example:

• to link two non consecutive paths
• to access finish and spring passes.

A Return on Same Level macro is used in a multi-path operation to link two consecutive paths in a given level.

A Return between Levels macro is used in a multi-level machining operation to go to the next level.

A Return to Finish Pass macro is used in a machining operation to go to the finish pass.

A Clearance macro can be used in a machining operation to avoid a fixture, for example.

Editing Parameters of Several Multi-Axis Flank Contouring Operations

You can modify the parameters of several Multi-Axis Flank Contouring operations in one shot as follows:

• Select two or more Multi-Axis Flank Contouring operations either in the Specification tree or in the Process table.
• Right-click the highlighted operations and select Selected Objects > Definition... 
  The Multi-Axis Flank Contouring dialog box appears.
• Modify any of the parameters that are available for edition.
  Note: Geometry and macro definitions can be edited if all the selected operations already have identical values.
  Some parameters may not be available for edition. Tool parameters cannot be edited and the Replay icon is disabled.
• Click OK to apply the modified parameters of all the selected operations.