4 Axis Pocketing

The 4 Axis Pocketing dialog box appears when you select 4 Axis Pocketing.

This page discusses:

See Also
Creating a 4 Axis Pocketing Operation

Resource Parameters

The Resource tab allows you to select a tool.

Resource Tab
Parameter Description
Select a Tool from Session Selects a tool in Resource Configuration View.
Select from Catalog Selects a tool from a reference tool file or PLM catalog.
Select from Database Selects a tool from the database.
Display Tool Properties Accesses tool parameters.
Define Tool Axis Defines the tool axis.
Tool Number Defines the number of tools.
Display Tool Displays the tool position.
Default Displays the tool at default position.
User Defined Displays the tool at a position defined by the user.
Note: You can define the tool position using Select a Tool from Session .
Tools
End Mill tools , Face Mill tools , Conical tools and TSlotter tools are available for these operations.

Geometry

the Geometry allows you to define the geometric parameters that are machined.

Mandatory Parameters
Mandatory Description
Bottom Defines the lowest plane machined on the part.
Contour Specifies the guide of the machining operation.
Note: This parameter is mandatory only in Finishing mode.
Optional Parameters
Optional Parameter Description
Contour Specifies the guide of the machining operation.
Note: This parameter is optional only in Roughing mode.
Start Point Selects preferential start position on the operation.Available for Inward Helical tool path style only.
Cutting Point Provides a cutting point to the Manufacturing Operation
First Relimiting Element Defines the starting point of the relimiting element.
Second Relimiting Element Defines the ending point of the relimiting element.
Machining Side Specifies the machining side.
Reverse Machining Side Specifies the reverse machining side.
Top Defines the highest plane machined on the part.
Check Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Island Specifies islands that are defined by hard boundaries with an optional offset on each island..
Pocketing Style Specifies the pocketing style.
Bottom Specifies the bottom type on planar faces or on a surface: Hard or Soft.
Other Parameters
Parameter Description
Start Specify that the start point is to be located Inside or Outside the pocket.
Notes:
  • If it is outside the pocket, you must specify a clearance with respect to the pocket boundary.
  • Like in Pocketing Operation, for internal Start Point, check the Always stay on bottom check box (in the Radial tab) to avoid any plunge in the material.
  • For a start point outside the pocket, if the projection of the start point is not on a soft boundary, it is ignored. A default start point is defined, according to the tool path style chosen.
Offset on Contour Specifies the distance between the tool and the guide contour at the beginning of the operation.
Offset on Hard Boundary Specifies the hard boundary offset.
Offset on Soft Boundary Specifies the soft boundary offset.

Strategy Parameters

The Strategy tab allows you to specify the strategy and user parameters.

Machining
Parameter Description
Computation Specifies the Roughing or Finishing computation mode.
Pocketing Tool Path Style

Specifies tool path style.

The Tool path style options are as follows:

  • Outward helical: The tool starts from a point inside the pocket and follows outward paths parallel to the boundary.
  • Inward helical: The tool starts from a point inside the pocket and follows inward paths parallel to the boundary.
  • Back and forth: The machining direction is reversed from one path to the next.
  • Offset on part One-Way: The machining direction is offset on the part one way.
  • Offset on part Zigzag: The machining direction is offset on the part zigzagging.
  • Concentric: The tool follows successive arc motions. For more information, see the section below.
  • Outward and Inward Spiral Morphing: The tool follows a true spiral motion evolving smoothly to match the boundary of the pocket. For more information, see the section below.
Direction of Cut

Specifies how machining is to be done:

  • Climb: The front of the advancing tool (in the machining direction) cuts into the material first.
  • 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.
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.
Compensation Specifies the tool corrector identifier to be used in the operation. The corrector type, corrector identifier, and corrector number are defined on the tool. When the NC data source is generated, the corrector number is generated using specific parameters.
Roughing Removes material before the bottom finishing paths.

  • Limits are defined with points along the revolution axis of the bottom or plane perpendicular to this axis.
  • Only cylindrical or conical bottoms are accepted.
  • If selected:
Finishing See Strategy Parameters > Finishing Strategy Parameters
Concentric Tool Path Style Parameters
The trajectory created by the Concentric strategy adapts itself dynamically to ensure a safe cutting at nominal speed. The engagement of the tool is controlled to never exceed a maximum value, even in corner areas.
This style is most suitable for hard-material milling, such as milling titanium, stainless steel, and ceramic materials where the tool needs to be protected. Other tool path styles, which are based on a constant distance between passes, are not appropriate because the tool load increases significantly when milling the inside of a radius.
The Concentric style controls the tool load by modifying, for each motion, the distance between passes. As a result, the tool lifetime is increased and the machining time is optimized.
Outward and Inward Spiral Morphing Tool Path Style Parameters

Outward and Inward Spiral Morphing tool paths give priority to a continuous machining motion (the goal is to avoid retract and linking motions as much as possible) and ensures that the step over does not exceed a maximum defined.

This strategy is more appropriate for a small step over between passes and a regularly shaped contour Otherwise, a small step over is generated by the morphing algorithm.

The High Speed Milling (HSM) feature guide cornerization is available for this strategy, as it relies already on a spiral and adapted offset motion.

The end point is not supported and is silently ignored.

The start point management: Start point is supported for Outward only.

If a start point is provided, the system verifies the reachability of this point. Nonreachable points are silently ignored. If points are reachable, the spiral motion starts from this point.

Island management: If an island is selected, the tool path starts (or finish depending on inward/outward flavor) around the island. If more than one island is selected or a reachable start point is given, the tool path contains a retract and linking motion.

If start point and island with Outward flavor is specified, the spiral starts at the start point and progresses toward the external contour. It then returns to the start point (after a linking motion) and progresses toward the island (with respect to the cutting mode).

Radial Strategy Parameters
Parameter Description
Radial Strategy Specifies how the distance between two consecutive paths is computed. Select one of the following options:
  • Maximum Distance
  • Tool Diameter Ratio
  • Stepover Ratio
Distance Between Path Defines the maximum distance between two consecutive tool paths in a radial strategy.
Tool Diameter Ratio Defines the maximum distance between two consecutive tool paths in a radial strategy as a percentage of the nominal tool diameter.
Overhang Ratio Allows a shift in the tool position with respect to the soft boundary of the machining domain.
Contouring Pass Allows a final machining pass around the exterior of the trajectory for removing scallops. This is available for 4 Axis Pocketing using a Back and Forth or Concentric tool path style.
Contouring Ratio Adjusts 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 4 Axis Pocketing using a Back and Forth or Concentric tool path style.
Always Stay on Bottom Forces the tool to remain in contact with the pocket bottom when moving from one machining domain to another.By default, deactivated.
Axial Strategy Parameters
Parameter Description
Mode

Specifies how the distance between two consecutive levels is computed:

  • 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.
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 Strategy Parameters
Parameter Description
Mode

Specifies whether or not finish passes are generated on the sides and bottom of the area to machine:

  • 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

Side Finish Thickness Specifies the thickness of material that is machined by the side finish pass.
Bottom Thickness on Side Finish Specifies the bottom thickness used for a 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 is machined by the bottom finish pass.
Spring Path Indicates whether or not a spring pass is 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.
High Speed Milling (HSM) Strategy Parameters
These parameters are disabled if a Concentric tool path style is selected.
Parameter Description
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 an HSM operation. Value must be smaller than the tooltip radius.
Corner Radius on Side Finish Path Specifies the corner radius used for rounding the corners along the side finish path of an HSM operation.
Note: Value must be smaller than the tool radius.
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.
Tool Axis Strategy Parameters
Parameter Description
Tool Axis Mode

Constant Lead The normal direction to surface first defines the fourth axis.
4 Axis Constant Lead The normal direction to surface first defines the 4th axis.

Lead Angle Value Specifies the lead angle value.
Axis Offset Specifies the axis offset.

Tool Axis Parameters

Tool Axis Parameters
Parameter Description
Activate Collision Checking Activates the collision checking option.
Part, Check, Design Part Enables collision checking on one or multiple elements.
Note: For collision checking with design parts, make sure that you have selected a valid Design Part in the Part Operation.
Fixtures on Part Operation Takes into account Check defined with the Part Operation
Additional Surface Selects additional surface to be checked.
Offset on Tool Defines the tolerance distance specific to the tool radius and tool length.
Offset on Tool Assembly Defines the tolerance distance specific to the tool assembly radius and tool length.

Macros Parameters

The Macros tab allows you to define transition paths in your machining operations by means of NC macros.

  • Approach
  • Retract
  • Clearance
  • Linking Retract
  • Linking Approach
  • Returnn in Level Retract
  • Returnn in Level Approach
  • Return Finish Pass Retract
  • Return Finish Pass Approach
  • Return Between Levels Retract
  • Return Between Levels Approach

For more information, see NC Machining Apps Common Services: Using the Working Area: Creating Machining Operations: Defining Macros: NC Macros.

Feedrate and Spindle Speed Parameters

The Feeds and Speeds tab allows you to define the following feeds and speeds parameters.

For more information, see About Feeds and Speeds.

Feedrate Parameters
Parameter Description
Feedrate Unit Defines the feedrate unit: Angular or Linear.
Approach Feedrate Defines the speed of linear/angular advancement of the tool during its approach, before cutting.
Machining Feedrate Defines the speed of linear/angular advancement of the tool during machining.
Retract Feedrate Defines the speed of linear/angular advancement of the tool during its retract, after cutting.
Finishing Feedrate Defines the speed of linear/angular advancement of the tool during finish machining.
Transition

You can locally define the feedrate for a transition path to a machining operation B from a machining operation A or from a tool change activity.

For more information, see Setting a Transition Feedrate.

Local Value Specifies the local feedrate value.
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.
RTCP ON When selected, activates RTCP mode on transition paths between the previous and current operations.
Spiral Start Rate

Is defined as a percentage of the machining feedrate. By default, it is defined as 70% and can vary from 20% to 100%.

Available with the Concentric tool path style.
Spindle Speed Parameters
Parameter Description
Spindle Unit Specifies the spindle unit: Angular or Linear.
Spindle Output Activates or deactivates the NC output of the spindle speed.
Machining Spindle Defines the speed of the spindle advancement.