Groove Milling Operations

The information in this section will help you create and edit 2.5 axis Groove Milling operations in your manufacturing program.

Select Groove Milling then select the geometry to be machined . 

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

A number of strategy parameters are available for defining:

• machining criteria

• axial and radial stepover conditions

• finishing.

The Machining direction (Top/Bottom, Bottom/Top) and Axial strategy (Standard, Middle, Middle alternate) parameters determine the tool path ordering for machining the groove as follows:

• The roughing pass ordering respects the Machining direction definition
• If Side finish pass is defined: a side finish pass is done for each roughing level
• If Top and/or Bottom finish passes are defined, Top and/or Bottom finish pass are done in order to minimize tool motion between levels.

  For example, in Top/Bottom machining with Top and Bottom finish passes, top finishing is done just after the first machining level and just before the second machining level.

  In Bottom/top machining with Top and Bottom finish passes, bottom finishing is done just after the first machining level and just before the second machining level.

• The tool compensation point is taken into account for each pass. This point is switched automatically during a Return between levels macro whenever the next level to machine requires a different compensation point.

Groove Milling Strategy Parameters

Groove Milling: Machining Parameters

	Tool path style Indicates the cutting mode of the operation: Zig Zag: the machining direction is reversed from one path to the next One way: the same machining direction is used from one path to the next.
	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.
	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.
	Close tool path Specifies whether or not the program must close the tool path.
	Percentage overlap Specifies the amount that the tool must go beyond the end point of a closed tool path according to a percentage of the tool diameter.
	Compensation output Allows you to manage the generation of Cutter compensation (CUTCOM) instructions. The following options are proposed: If 2D Radial profile is selected, both the tool tip and cutter profile 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. If 2D Radial tip is selected, the tool tip 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. If None is selected, cutter compensation instructions are not generated in the NC data output. In this case, please refer to How to generate CUTCOM syntaxes.  Any user-defined PP words in macros are added to the cutter compensation instructions generated in the NC data output. Therefore you should be careful when specifying CUTCOM instructions in macros. A negative Offset on contour (parameter in Geometry tab page) is possible for 2D radial profile output.
	Compensation on top / Compensation on bottom Specifies the tool corrector identifiers to be used in the operation. This point is switched automatically during a Return between levels macro whenever the next level to machine requires a different compensation point. 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.

Groove Milling: Axial/Radial Stepover Parameters

	Machining direction Defines how the distance between two consecutive levels is to be computed: Top/Bottom Bottom/Top.
	Axial strategy Defines how the tool path is to be ordered for machining the groove: Standard Middle Example: Middle axial strategy with Bottom/Top machining Example: Middle axial strategy with Top/Bottom machining Middle alternate Example: Middle alternate axial strategy with Top/Bottom machining
	Axial mode Defines how the distance between two consecutive levels is to be 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.
	Distance between paths Defines the maximum distance between two consecutive tool paths in a radial strategy.
	Number of paths Defines the number of tool paths in a radial strategy.

Groove Milling Finishing Parameters

	Finishing mode Indicates whether or not finish passes are to be generated on the sides, top and bottom of the area to machine. There are several possible combinations:     For example, Top/Bottom machining with side, top and bottom finish passes:
	Side finish thickness Specifies the thickness of material that will be machined when finishing the flank of the groove.
	Bottom finish thickness Specifies the thickness of material that will be machined when finishing the bottom of the groove.
	Bottom thickness on side finish Specifies the bottom thickness used for last side finish pass, if side finishing is requested on the operation.
	Top finish thickness Specifies the thickness of material that will be machined when finishing the top of the groove.
	Top/bottom finish path style Defines the finish path style for the top and bottom finish passes: Zig zag or One way.
	Spring pass Indicates 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.

Groove Milling Geometry

Tool follows a guiding contour between top and bottom of the groove while respecting user-defined geometry limitations and machining strategy parameters.

You can specify the following Geometry:

• Bottom (planar face or surface) with possible Offset on Bottom. Bottom may be Hard or Soft. 

• Top plane with possible Offset on Top. Top may be Hard or Soft.
• Open or closed guiding contour (edges or sketch) with possible Offset on Contour.
• Start and Stop Relimiting elements with possible Offsets. 
• Fixture or check elements with possible Offset on Check.

Specifying Guiding Contours

Guiding contours can be specified in several ways:

• if the Contour Detection contextual command is set, select the bottom element. The boundary of the selected face will be proposed as guiding contour.

• select edges. In this case the Edge Selection toolbar appears to help you specify the guiding contour.

• select the By Belt of Faces or By Boundary of Faces contextual command. In this case the Face Selection toolbar appears to help you specify the guiding contour.

• select the Sectioning contextual command. Please refer to Sectioning for details of how to use this capability.
  Please note that the sectioning selection method is not associative.

Specifying Relimiting Elements

The guiding contour can be restricted by means of Start and Stop relimiting elements. The tool can be positioned In, On or Out with respect to a relimiting element. You can select a point or a curve as relimiting element.

A fast way to specify relimiting points is to right-click the guiding contour area in the sensitive icon of the dialog box and set the Relimitation point detection contextual command.  When you select a guiding contour, its extremities will be used as relimiting elements.

Note that a relimiting point can be created anywhere along the guiding contour by means of the Add relimiting point contextual command. Just right-click the relimiting element area in the sensitive icon of the dialog box and select any position along the guiding contour.

Checking for Collisions between Tool and Guide Elements during Macro Motions

Collision checking is done during macro motion. All guiding elements defined on the operation are taken into account during this verification. However, in some cases, it can be useful to deactivate collision checking with the guides (see example below).

The Collision Avoidance capability allows you to manage this collision checking.

When you select Collision checking on the Geometry tab page, the following dialog box appears.

When the Include guiding elements checkbox is selected, guides are checked for collisions during macro motion. By default the checkbox is selected.

When the checkbox is not selected, no collision verification is done with the guides during macro motions.

By default the checkbox is selected.

Groove Milling Tools

A Groove Milling operation uses a T-Slotter.

Groove Milling Feeds and Speeds

In the Feeds and Speeds tab page, you can specify feedrates for approach, retract, machining and finishing 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 Groove Milling, feedrate reduction applies to inside corners for machining or finishing passes. It does not apply for macros or default linking and return motions.

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

Groove Milling 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.

Groove Milling P1/P2 Considerations

Note that P2 functionalities for Groove Milling include all Finishing parameters, and Sectioning for guiding element selection.
To edit in P1 a Groove Milling operation that was created in P2, the following parameter values must be set:

• Finishing Mode = No finish path
• Side finish thickness = 0.0 mm
• Top finish thickness = 0.0 mm
• Bottom finish thickness = 0.0 mm
• Spring pass = no.