Pocketing

Related Topics
Creating a Pocketing Operation for Closed Pockets
Creating a Pocketing Operation for Open Pockets

The Pocketing dialog box appears when you select Pocketing. This dialog box contains controls for:



Machining Strategy Parameters



Tool Axis
See Defining the Tool Axis
Tool path style
Specifies tool path style.

The options in the Tool path style dropdown combo box are as follows:

  • Inward helical: the tool starts from a point inside the pocket and follows inward paths parallel to the boundary.
  • Outward helical: the tool starts from a point inside the pocket and follows outward paths parallel to the boundary.
  • Back and forth: the machining direction is reversed from one path to the next.

Machining Parameters



Direction of cut
Specifies how machining is to be done.

The options in the Direction of cut dropdown combo box are as follows:

  • Climb milling: the front of the advancing tool (in the machining direction) cuts into the material first

  • Conventional milling: 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.
Fixture accuracy
Specifies a tolerance applied to the fixture thickness. If the distance between the tool and fixture is less than fixture thickness minus fixture accuracy, the position is eliminated from the trajectory. If the distance is greater, the position is not eliminated.
Limit machining area with fixture
Select this check box to re-limits the area to machine for computing the tool path without jump motions around the check elements.
  • Limit machining area with fixture is not selected: there is a jump motion around the check element.

  • Limit machining area with fixture is selected, there is a contouring around the check, and no jump motion.

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.

Radial Parameters



Mode

The options in the Mode dropdown combo box specifies how the distance between two consecutive paths is computed, and are as follows:

  • Maximum distance between paths
  • Tool diameter ratio
  • Stepover ratio

Distance between paths
Defines the maximum distance between two consecutive tool paths in a radial strategy.
Percentage of tool diameter
Defines the maximum distance between two consecutive tool paths in a radial strategy as a percentage of the nominal tool diameter. Depending on the selected radial mode, this value is used as:
  • Tool diameter ratio:

  • Stepover ratio:

Overhang
Allows a shift in the tool position with respect to the soft boundary of the machining domain.

Avoid scallops on all levels
Select this check box to adjusts the distance between paths to avoid scallops on all level.
  • Avoid scallops on all levels is not selected:

  • Avoid scallops on all levels is selected:

Truncated transition paths

  • Available for Back and Forth tool path style.
  • When selected, truncates the transition portion of the trajectory to follow the external profile more exactly.
  • Truncated transition paths is not selected:

  • Truncated transition paths is selected:

Contouring pass
Select this check box to allows a final machining pass around the exterior of the trajectory and islands for removing scallops. This is available for Back and Forth tool path style.
Contouring ratio
Specifies the contouring ratio to adjust the position of the final contouring pass for removing scallops. This is done by entering a percentage of the tool diameter (0 to 50). This is available for Back and Forth tool path style.
Always stay on bottom
When machining a multi-domain pocket using a Helical tool path style, this parameter forces the tool to remain in contact with the pocket bottom when moving from one domain to another. This avoids unnecessary linking transitions.

Axial Parameters



Mode

The options in the Mode dropdown combo box specifies how the distance between two consecutive levels is computed, and are as follows:

  • Maximum depth of cut
  • Number of levels
  • Number of levels without top

Maximum depth of cut
Defines the maximum depth of cut in an axial strategy.
Number of levels
Defines the number of levels to be machined in an axial strategy.
Automatic draft angle
Specifies the draft angle to be applied on the sides of the pocket.
Breakthrough
Specifies the distance in the tool axis direction that the tool must go completely through the part. Breakthrough is applied on the bottom element, which must be specified as soft.

Finishing Parameters



Mode

The options in the Mode dropdown combo box specifies whether or not finish passes are generated on the sides and bottom of the area to machine, and are as follows:

  • No finish pass
  • Side finish last level
  • Side finish each level
  • Finish bottom only
  • Side finish at each level & bottom
  • Side finish at last level & bottom

In short:

  • Side finishing can be done at each level or only at the last level of the operation.
  • Bottom finishing can be done without any side finishing or with different combinations of side finishing.

Side finish thickness


Specifies the thickness of material that can be machined by the side finish pass.
Number of side finish paths by level
Specifies the number of side finish paths for each level in a multi-level operation. This can help you to reduce the number of operations in the program.

Bottom thickness on side finish
Specifies the bottom thickness used for last side finish pass, if side finishing is requested on the operation.

Side thickness on bottom


Specifies the thickness of material left on the side by the bottom finish pass.
Bottom finish thickness
Specifies the thickness of material that will be machined by the bottom finish pass.

Spring pass
Select this check box to indicate whether or not a spring pass is to be generated on the sides in the same condition as the previous side finish pass. The spring pass is used to compensate the natural spring of the tool.
Avoid scallops on bottom
Select this check box to adjusts the distance between paths to avoid scallops on the bottom. This is available for single-level and multi-level operations with bottom finish pass.
Compensation output
The options in the Compensation output dropdown combo box manage the generation of Cutter compensation (CUTCOM) instructions for the pocketing operation side finish pass, and are as follows:


  • If 2D Radial profile is selected, both the tool tip and cutter profile can 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.

    Note: A negative Offset on contour (parameter in Geometry tab) is possible for 2D radial profile output.

  • If 2D Radial tip is selected, the tool tip can 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.
  • If None is selected, cutter compensation instructions are not automatically generated in the NC data output. However, CUTCOM instructions can be inserted manually. In this case, refer to Procedure for Generating CUTCOM Syntaxes.

Note: The PP words in macros you define are added to the cutter compensation instructions generated in the NC data output. Therefore be careful when specifying CUTCOM instructions in macros.

HSM Parameters



High Speed Milling
Specifies whether or not cornering for HSM is to be done on the trajectory.
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.

Limit angle
Specifies the minimum angle for rounding corners in the tool path for a HSM operation.

Extra segment overlap
Specifies the overlap for the extra segments that are generated for cornering in a HSM operation. This is to ensure that there is no leftover material in the corners of the trajectory.

Cornering on side finish path
Specifies whether or not tool path cornering is to be done on side finish path.
Corner radius on side finish path
Specifies the radius used for rounding the corners of the side finish path in a HSM operation. Value must be smaller than the tool radius.
Limit angle on side finish path
Specifies the minimum angle for rounding the corners of the side finish path in a HSM operation.
Transition radius
Specifies the radius at the start and end of the transition path when moving from one path to the next in a HSM operation.

Transition angle
Specifies the angle of the transition path that allows the tool to move smoothly from one path to the next in a HSM operation.

Transition length
Specifies a minimum length for the straight segment of the transition between paths in a HSM operation.

User Parameters

See Adding an User Parameter

Geometry



You can specify the following geometry:

  • Pocket Bottom (planar face or surface) with possible Offset on Bottom. Bottom may be Hard or Soft.
  • Pocket Boundary (edges or sketch) with possible:
    • Offset on Hard Boundary,
    • Offset on Soft Boundary,
    • Offset on Contour. If you specify an Offset on Contour, it is added to any defined Offset on Hard Boundary,Offset on Soft Boundary, and Offset on Island.
  • Pocket Top plane with possible Offset on Top.
  • Islands (defined by hard boundaries) with possible offset on each island.
  • Check elements with possible Offset on Check.
  • Start point and End point as preferential start and end positions for the operation. This allows a better control for optimizing the program according to the previous and following operations.

    Note: The Start point can be located outside an open pocket. In this case, you must specify a clearance with respect to the pocket boundary.

See also Selecting Guiding and Relimiting Elements

Tools

Recommended tools for Pocketing are:

  • End Mills ,
  • Face Mills ,
  • Conical Mills , and
  • T-Slotters .

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
  • Finishing

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.

Slowdown Rate
Reduces the current feedrate by a given percentage. The reduction is applied to the first channel cut and to the transitions between passes.
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
  • Distance before corner
  • Distance after 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.

For Pocketing, feedrate reduction applies to machining and finishing passes:


  • for all corners in Back and forth mode
  • for inside corners in Inward and Outward Helical mode.
  • The figure below shows that feedrate reduction is not applied in Inward Helical for most of the corners, as these are not inside corners.

  • The figure below shows that feedrate reduction is applied in each corner in Outward Helical, as these are inside corners.

Feedrate reduction does not apply for macros or default linking and return motions.

Corners can be angled or rounded, and may include extra segments for HSM operations.



Combining Slowdown Rate and Feedrate Reduction in Corners

If a corner is included in a slowdown path, the general rule is that the lowest percentage value is taken into account. For example:

  • if the Slowdown rate is set to 70 % and Feedrate reduction rate in corners is set to 50%, the feedrate sequence is: 100%, 70% (entry in slowdown), 50% (entry in corner), 70% (end of corner, still in slowdown), 100% (end of slowdown).
  • If feedrate Reduction rate in corners is then set to 75%, the feedrate sequence is: 100%, 70% (entry in slowdown), 70% (entry in corner: 75% ignored), 70% (end of corner, still in slowdown), 100% (end of slowdown).

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:

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.

Quality
The feed and speed values are computed according to the Quality setting on the operation.
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 transition paths in your machining operations by means of NC macros:

  • Approach: to approach the operation start point,
  • Retract: to retract from the operation end point,
  • Linking: to link motions in the tool path,
  • Return between Levels to go to the next level in a multi-level machining operation,
  • Return to Finish Pass to go to the finish pass
  • Clearance to avoid a fixture, for example.

When a collision is detected between the tool and the part or a check element, a clearance macro is applied automatically. If applying a clearance macro would also result in a collision, then a linking macro is applied. In this case, the top plane defined in the operation is used in the linking macro.

The proposed macro mode are:

  • None
  • Build by user
  • Horizontal horizontal axial
  • Axial
  • Ramping

For more information, please refer to the Defining Macros.

Intermediate Levels

Right-click Parameters in the contextual menu of a Ramping approach macro mode.

The following dialog box appears:

When Intermediate levels check box is selected, the approach macro is divided in three parts:

  • A ramping approach from the top of the pocket to the intermediate level
  • A horizontal path, which is the same as the first path if the machining mode is Back and Forth or the first closed path if the machining mode is Helical
  • A ramping approach from the intermediate level to the machining level.

The yellow path in the figure below illustrates an intermediate level for a ramping approach macro in a Back and Forth Pocketing operation.