Sequential Axial and Sequential Groove Operations

The Sequential Axial dialog box appears when you select Sequential Axial and the Sequential Groove dialog box appears when you select Sequential Groove. This dialog box contains controls for:

Related Topics
Creating a Sequential Groove Operation
Creating a Sequential Axial Operation



Motions Parameters



Properties
Edits the motion selected in the dialog box.
Delete
Deletes the motion selected in the dialog box.
and
Changes the rank of the motion selected in the dialog box.
Spindle Speed
Inserts a tool motion defined by a spindle speed.



Spindle mode
Specifies spindle mode as Machining / Local spindle speed.
Local Spindle
Specifies the value and unit of local spindle speed.

Note:

The spindle speed can be defined in linear (length per minute) or angular (length per revolution) units.

  • : length in revolutions per minute and unit is set to mm_turn.
  • Linear: length in feed per minute and unit is set to mm_mn.

Way of rotation
Specifies way of rotation as CLW/CCLW

NC_SPINDLE NC command is generated in output file. Example:

SPINDL/500,RPM

Spindle Stop
Inserts a tool motion defined by a spindle stop or lock.

Spindle stop: NC_SPINDL_STOP NC command is generated in output file

Spindle lock: NC_SPINDL_LOCK NC command is generated in output file.

Delay
Inserts a tool motion defined by a delay (in spindle revolutions or time).

Spindle Dwell mode
Specifies spindle dwell mode as By time units / By revolutions.

NC_DELAY NC command is generated in output file. Example: 

DELAY/2,REV

PP Word
Inserts a tool motion defined by PP word statements (access to a PP word table is available if one is defined on the machine of Part Operation).
Go to Plane
Inserts a tool motion defined by an axial motion to a plane defined and numbered 1 to 5 in the Geometry tab. The motion is done normal to the plane.

Plane number
Specifies plane number between 1 to 5.
Offset on plane
This offset is added to the offset that can be set on the geometric element selected in the Geometry tab.

Note:

  • Offset is positive along the tool axis direction and negative on the opposite direction.
  • Offset defined on the selected element (plane) and the offset defined on the motion are both taken into account to compute the tool position.

Feedrate mode
Allows definition of Machining, Approach, Retract, RAPID, or Local feedrate (including feedrate unit when local feedrate is defined).
Compensation
Allows definition of the compensation point for this motion. The compensation is activated at the start of the motion.

NC_COMPENSATION syntax is generated in the output file when the compensation point is different from previous motion. Example: 

LOADTL/2,5

Go Delta
Inserts a tool motion defined by a displacement specified by DX, DY, DZ values. Positive DZ value is defined along the machining hole axis.

See Feedrate Mode and Compensation.

Go to Clearance
Inserts a tool motion defined by an axial motion up to clearance plane (defined by the Approach clearance). The tool tip can reach the plane defined by the approach clearance displayed on the Strategy tab .

See Feedrate Mode and Compensation.

By default, If no Go to Clearance motion is defined in the motion list, an automatic motion is done from the last position reached by the tool motion (last sequential motion) up to the clearance plane (defined by the Approach clearance). This automatic motion is done at RAPID feedrate.

Circular
Inserts a tool motion defined by approach, retract and complete circular motions, which are defined in the icon of the dialog box.

Available in Sequential Groove only.

Tool path is generated as follows.

  • Approach motions, full circular motion (on the selected diameter + offset), and retract motions.
  • Approach and retract motions can be activated or deactivated (the complete circular motion cannot be deactivated).
  • Feedrate type or local value (including feedrate unit) can be set on each motion.
  • Circular approach and retract motion parameters can be set.

Offset on diameter
Offset taken into account for tool path computation (positive value defines offset inside the circle and negative value defines offset outside the circle).
Direction of cut
Specifies how machining is to be done.

Yopu can specify: Climb / Conventional (direction of motion is done to respect cutting condition).

Spring pass
Select this check box to define an optional circular motion before retract motion.

By default, the check box is not selected.

Helical
Inserts a tool motion defined by approach, retract, and complete helical motions, which are defined in the icon of the dialog box. Available in Sequential Groove only.



Tool path is generated as follows.

  • Approach and retract motions can be activated or deactivated (the helical motion cannot be deactivated).
  • Feedrate type or local value (including feedrate unit) can be set on each motion.
  • Circular approach and retract motions parameters can be set.

Offset on diameter
Offset taken into account for tool path computation (positive value defines offset inside the contour and negative value defines offset outside the contour).
Plane
Defines the plane to reach (can be plane 1 or plane 2 of the level).
Offset on plane
This offset is added to the offset that can be set on the geometric element selected in Geometry tab.
Helix mode
Specifies helix mode as By angle/By pitch. Angle or pitch value is displayed in Angle(Ang) or Pitch (P).
Direction of cut
Specifies the direction of cut for tool as Climb / Conventional

Note:

  • The up/down helical motion direction is defined with the plane to reach. Up or down helical motion is defined with the difference between the current position and the plane to reach.
  • Helical interpolation instructions can be generated in the output file (APT source and Clfile) for helical tool motions.
  • Approach and retract motions are not done with a helical tool path.

Strategy Parameters



Power
See Power
Approach clearance
Defines a safety distance along the tool axis for approaching the hole reference.
Machining tolerance
Specifies the maximum allowed distance between the theoretical and computed tool path.
Compensation output
Defines automatic activation/deactivation of CUTCOM statements for all circular and helical trajectories

You can specify:

  • None
  • 2D Radial profile
  • 2D Radial tip

First compensation
Specifies the tool corrector identifier to be used in the operation. The corrector type (P1, P2, P3, for example), corrector identifier, and corrector number are defined on the tool. When the NC data source is generated, the corrector number can be generated using specific parameters.
Compensation application mode
Specifies how the corrector type specified on the tool (P1, P2, P3, for example) is used to define the position of the tool:

You can specify:

  • Output point: the tool compensation point is generated in the output file. The tool path computation is done according to the tool tip.
  • Guiding point: the tool motion is computed according to the tool compensation point and the tool compensation point is generated in the output file.

Automatic ROTABL
Select this check box to allow the generation of rotation motions between drilling points that have different tool axes. This capability works with a 3-axis milling machine with rotary table when ROTABL/ output is requested.

User Parameters

See Adding a User Parameter

Geometry

Sequential Axial and Sequential Groove operations inherit options and behavior available on axial operations: Check element selection, Offset on check, Top element selection, Top element/Projection, Origin offset, Jump distance, machining points to select (selection and management of machining points), ordering capability (Closest, Manual, By Band, Reverse Ordering), machining pattern selection, and so on. Refer to 2.5 to 5-Axis Drilling Operations for more information.

For both operations, the geometry () (hole to machine) is managed in the Global tab. The additional geometry (planes or depth and offsets) is managed in the Local tab. However, there are some differences concerning geometry selection.

Sequential Axial operation

  • Geometry selection is dedicated to hole machining. You define planes (and offset) or depth value to manage axial tool path between planes.
  • Any number of planes can be selected and used for the tool motions.
Sequential Groove operation

  • Geometry selection is dedicated to groove machining. You define planes, diameters (and offsets), or values to manage axial and circular motions.
  • Up to 10 machining levels can be defined: two planes and one diameter can be defined on each level.
  • The sequential motions defined in the list are applied to each groove level: the list of motions is defined for a single level. At tool path generation, the motions are applied to each groove level.

Selection of Geometry

Geometry can be defined by selection of geometrical elements or by valuation of depth or diameter values.

When selecting a geometrical element to define the plane or diameter, the depth or diameter value is automatically displayed in the dialog box.

The depth or diameter value can be modified. In this case the link with the corresponding geometry (plane, diameter) is lost: the corresponding plane (and offset) is reset.

In case of modified geometry (not up to date), a yellow status light is displayed in the Status column of Activities Process Tree.

In case of lost geometry (geometry not found), a red status light is displayed in the Status column of Activities Process Tree.

For a sequential motion on which geometry is not found, the character (?) is displayed in the Status column of Activities Process Tree.

Global and Local Geometry for Sequential Axial Operations

Global tab:

Hole diameter and depth
Initialized from point selection, these values are not used for tool path computation but are displayed for information. They can be can be used by f(x) formula.
Inverse pattern ordering
Select this check box to reverses the order of machining holes.
Relimit hole origin
Select this check box to determine the hole origin according to tool axis (when design hole is selected).

For more details, See Geometry.

Local tab:

Number of planes
Any number of machining planes can be defined. They are presented in groups of five maximum in the sensitive icon of the Local tab.

The distance to each machining plane is defined by entering a value or by selecting a geometrical element (plane, planar surfaces, planar edge, or point). These values are defined for the first machining hole and the same values are used to machine all the machining holes.

Global and Local Geometry for Sequential Groove Operations

Global tab:

Hole diameter and depth
Initialized from point selection, these values are not used for tool path computation but are displayed for information. They can be can be used by f(x) formula.
Number of levels
A maximum of 10 levels can be specified.
Machining strategy
Defines how the different levels are taken into account:
  • For Top/Bottom strategy, the first level to machine depends on the Plane 1 axial position. The level to machine is determined according to the distance from hole origin to the Plane 1 of a level. The first level to machine is the level on which Plane 1 is the upper one.
  • For Bottom/Top strategy, the first level to machine depends on the Plane 2 axial position. The level to machine is determined according to the distance from hole origin to the Plane 1 of a level. The first level to machine is the level on which Plane 2 is the lower one.
Inverse pattern ordering
Reverses the order of machining holes.
Relimit hole origin
Determines the hole origin according to tool axis (when design hole is selected).

Local tab:

Level number
The geometry linked to the selected level number is displayed.
Machining diameter
Defines a diameter value or select an element (circular edge).
Offset on diameter
Defines the offset to be used on the defined diameter (or selected circular element). A positive value defines an offset inside the diameter. A negative value defines an offset outside the diameter.

Tools

All

  • milling tools and
  • drilling tools

(except Barrel Mills ) can be used in this type of operation.

See Specifying a Tool Element in a Machining Operation

Feedrates and Speeds Parameters



Feedrate: Automatic compute from tooling Feeds and Speeds
This check box allow an operation's feeds and speeds values to be updated automatically when the tool's feeds and speeds values are modified.

You can specify the following feedrates:

  • Approach
  • Machining
  • Retract
  • Rapid: In Point to Point operations, a local feedrate can be defined for all tool motions (except the first motion, which must be either RAPID or a specific feedrate). The local feedrate is applied instead of the machining feedrate during the tool motion to reach the tool position. For the operation start point, machining feedrate is taken into account.

Note:

The above feedrates can be defined in linear (feed per minute) or angular (feed per revolution) units.

  • Angular: feedrate in revolutions per minute and unit is set to mm_turn.
  • Linear: feedrate in feed per minute and unit is set to mm_mn.

Transition
You can locally set the feedrate for a transition path to a machining operation B from a machining operation A or from a tool change activity. This is done by selecting the Transition check box in the Machining Operation dialog box for operation B.

For more information, please refer to the Setting a Transition Feedrate.

Spindle Speed: Automatic compute from tooling Feeds and Speeds

This check box allow an operation's feeds and speeds values to be updated automatically when the tool's feeds and speeds values are modified.

If the Feedrate Automatic compute check box is selected and the Spindle Speed: Automatic compute from tooling Feeds and Speeds check box is not selected, then only the feedrate values can be computed. If both are not selected then automatic updating is not done.

When you modify a tool's feeds and speeds, all existing operations with the Automatic compute check boxes selected that use this tool (or an assembly using this tool) can be recomputed.

Spindle output
This check box manage output of the SPINDL instruction in the generated NC data file:
  • If the check box is selected, the instruction is generated.
  • Otherwise, it is not generated.

Note:

Spindle speed is applied on the different motions of the operations (including approach, retract, linking macros). Spindle can be re-defined with Spindle tool motion.

The spindle speed can be defined in linear (length per minute) or angular (length per revolution) units.

  • Angular: length in revolutions per minute and unit is set to mm_turn.
  • Linear: length in feed per minute and unit is set to mm_mn.

Compute
Feeds and speeds of the operation can be updated according to tooling feeds and speeds by clicking the Compute button located in the Feeds and Speeds tab of the operation

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 About Feeds and Speeds.

NC Macros



You can define transitions paths for:


  • Approach: to approach the operation start point.
  • Retract: to retract from the operation end point.
  • Linking: Linking between machining holes of the same pattern
  • Clearance: Used to define the feedrate on the horizontal path between two machining positions.

The proposed macro mode are:

  • None
  • Build by user

For more information, please refer to the Defining Macros.