Groove Turning Operations

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

The Groove Turning operation allows you to machine a groove by a series of plunging cuts. You can specify:

• external, internal, frontal or inclined machining according to the type of area to machine
• various approach and retract path types
• various lead-in and lift-off options with specific feedrates
• various plunge locations
• tool output point change.

The following topics are dealt with in the paragraphs below:

• Tooling
• Geometry
• Machining Strategy Parameters
• Feeds and Speeds
• Tool Compensation
• Macros.

Tooling for Groove Turning

The following tooling may be used:

• Internal, External and Frontal Groove insert-holders with groove and trigon inserts.
  Refer to Trigon Insert Used on a Groove Insert-holder for more information about this tooling configuration.
• External and Internal insert-holders with round inserts.

Note that the following attributes may influence machining (they are located on the Insert-holder's Technology tab):

• Gouging angle
• Trailing angle
• Leading angle
• Max Recessing Depth
• Max Cutting Depth
• Max Boring Depth.

These attributes take tooling accessibility into account and may reduce the machined area.
However, you can use the Insert-Holder Constraints option on the operation editor to either ignore or apply these tooling attributes. You can replay the operation to verify the influence of these attributes on the generated tool path.

Notes:

• Insert-Holder Constraints are applied if the sum of tool setup angle and angle of groove incline (if defined) is less than 45 degrees.
• The Insert-Holder Constraints setting does not influence the Gouging Safety Angle or Max Depth of Cut defined in the operation editor.

Geometry for Groove Turning

Part and Stock profiles are required. They can be specified as follows:

• select edges either directly or after selecting the By Curve contextual command. In this case the Edge 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.

Orientation for Groove Turning

The following Orientations are proposed: internal, external, frontal and inclined. The selected Orientation defines the type of geometric relimitation to be done between the stock and part geometry in order to determine the area to machine. For an inclined orientation you must specify the Angle of Incline.

Part and Stock Offsets for Groove Turning

• Stock offset, which is defined perpendicular to the stock profile
• Part offset, which is defined perpendicular to the part profile.
• Axial part offset
• Radial part offset.

Offsets can be positive or negative with any absolute value. The global offset applied to the part profile is the resulting value of the normal, axial and radial offsets.

End Limit for Groove Turning

In grooving, the part profile usually needs to have flanks at the both ends of the profile. But in some cases you can define geometry with single flank. Such a geometric selection is referred as an open-ended groove.

In case of a Groove Turning operation for an open-ended groove, one end is limited by flank and the second end limit of the profile geometry is considered till the selected geometric end element. If you need to restrict the end to a different location, then the selected geometry for this purpose is referred to as End Relimiting Elements. The option that is used to select this element is called as End Limit.

End Limit option allows you to specify a point, line, curve or face to relimit or extrapolate the selected part profile. If a face is specified, the end element is the intersection of the face and the working plane. The position of the end of machining is defined with respect to this element by one of the following settings: None / In / On / Out.

End limit offset: distance with respect to the end element (only if end element is a line or a curve, and when In or Out  is set for end element positioning).

If you wants to limit the path at the open end, the End Limit Offset option helps in defining end limit element. When you select the End Limit, a message comes Click to select an End Re-limiting Element.

Once End Relimiting element is selected it is highlighted and the tool path is computed till the end limit element. The new tool path will be as shown below.

The End Limit has an influence on the specified Strategy tab settings.

Case 1: With reference to the above geometry, if the selected strategy options are:

• Orientation: External
• First plunge position: Centre
• Next plunges position: To head stock.

In this case the tool path will be defined from centre to flank, then from centre to end element.

Case 2: With reference to the above geometry, if the selected strategy options are:

• Orientation: External
• First plunge position: Centre
• Next plunges position: From head stock.

In this case the tool path will be defined from flank to centre, then from end element to centre.

Machining Strategy Parameters for Groove Turning

Path Definition for Groove Turning

• Max Depth of Cut
  This option is used to specify the maximum distance between plunges.
• First Plunge Position
  Depending on the groove orientation, you must specify a first plunge position by means of the following choice: Left/Down - Center - Right/Up - Automatic.
  Automatic is only available for frontal machining. In this case, the position of the first plunge is deduced from the tool's minimum and maximum cut diameters. The position is at a distance:
  (Minimum cut radius + Maximum cut radius)/2.

• Next Plunges Position (if First Plunge Position is set to Center).
  You can specify the position of the plunges that follow the first plunge with respect to:
  • the spindle axis by means of To/From Spindle for frontal machining
  • the head stock by means of To/From Head Stock for internal or external machining
  • the groove by means of Left/Right of Groove for inclined machining.

  If First Plunge Position is set to Center, the Single plunge option is available. This is suitable for machining a narrow groove, possibly using the Grooving by level and Chip break options. Note that in this case Part Contouring is not available.

• Part Contouring
  You can specify if contouring is required by means of the proposed checkbox.
  The part profile is followed at the end of grooving. This is done by machining down the sides of the groove in order to clear the profile.
  
  Part Contouring is done based on collision checking between the tool insert and stock/part profiles.
  This means the contouring path which is collision free, may lead to incomplete part contouring based on the geometry of the stock and part profile selected during Geometry definition.
  
  To get complete Part Contouring, geometry of the stock and part profile selected during Geometry definition must account for any collisions between tool insert and geometry.
• Grooving by Level mode
  This option allows you to machine the groove in one or more levels.
  Multiple-levels mode is particularly useful when the groove is too deep to machine in one level. In this case Max depth of level defines the maximum depth of each level. If it is greater than the Maximum depth of cut defined on the tool, the value on the tool is taken into account.
  
  During return motion at the end of a level, the tool returns at Rapid or Air-cutting feedrate to the first pass of a new grooving level up to a Max approach distance. The feedrate then reduces to lead-in feedrate for this approach distance.
  
  See also Behavior of Linking Macro when Grooving by Level.
• Under Spindle Axis Machining
  When Groove Turning in frontal mode, this option allows you to request machining under the spindle axis.
• Chip Break
  You can specify if chip clearing is to be done during machining by setting the check box. In this case you must specify Plunge, Retract and Clear distances.
• Gouging Safety Angle
  Angle attributes on the grooving insert are taken into account to avoid collision by reducing the maximum slope on which the tool can machine. The Gouging Safety Angle allows you to further reduce this slope.
  
  Note that a gouging angle can also be defined on the insert-holder to define the maximum slope on which the tool can machine. In this case and if the Insert-Holder Constraints setting is applied (see above), the angle that reduces the slope the most will be taken into account.
• Machining Tolerance.

Lead-in, Lift-off and Attack for Groove Turning

• Lead-in Distance
  Defined with respect to the cutting direction. It takes the stock profile and stock clearance into account. The tool is in RAPID mode before this distance.
• Attack Distance
  Defined with respect to the cutting direction and the stock profile with a stock clearance.

These options allow penetration into the workpiece at a reduced feedrate in order to prevent tool damage. Once the attack distance has been run through, the tool moves at machining feedrate.

When tool motion between two passes is in contact with the part profile, in order to avoid collisions the corresponding feed is the lift-off feedrate and not RAPID.

• Lift-off Distance and Lift-off Angle
  These parameters define the lift-off vector at the end of each pass with respect to the cutting direction. The figure below shows the effect of a positive lift-off angle (external machining is assumed).

Feeds and Speeds for Groove Turning

Speed unit can be set to:

• Angular: spindle speed in revolutions per minute
• Linear: constant cutting speed in units per minute

then you can give a Machining Speed value.

You can also set a Maximum spindle speed value for the operation (by default, this value is the same as the Maximum spindle speed set on the Part Operation).

The following feedrates can be set to either Angular units (length per revolution) or Linear units (length per minute):

• Contouring feedrate
• Lead-in feedrate, which is applied during lead-in and attack distances
• Lift-off feedrate
• First Plunge feedrate and Next Plunges feedrate.
  Different feedrates can be assigned to the first plunge and the following plunges
• Air cutting feedrate.

Feedrates are also available for air cutting trajectories such as macro motions and path transitions.
Note that RAPID feedrate can be replaced by Air cutting feedrate in tool trajectories (except in macros) by selecting the checkbox in the Feed and Speeds tab page .

You can select Air Cutting feed-rate as Linear (feed per minute) or Angular (feed per revolution). When you select it as Angular the unit is set to mm_turn, the unit is set to mm_mn for Linear.

The changes in unit of Air cutting feed-rate, are also reflected in APT file output. Calculated cycle time in Properties dialog box of MO also get changed. There are changes in total time and machining time on tool path replay dialog box.

Dwell setting indicates whether the tool dwell at the end of a path or a plunge is to be set in seconds or a number of spindle revolutions.

Please note that decimal values can be used for the number of revolutions. For example, when machining big parts that have a large volume, it can be useful to specify a dwell using a value of less than one revolution (0.25, for example).

Tool Compensation for Groove Turning

You can select a tool compensation number corresponding to the desired tool output point. Note that the usable compensation numbers are defined on the tool assembly linked to the machining operation. If you do not select a tool compensation number, the output point corresponding to type P9 will be used by default.

Note that the change of output point is managed automatically if you set the Change Output Point option.
If the output point is consistent with the flank of the groove to be machined, the output point is changed when the other flank of the groove is machined.
At the end of the operation, the output point is the same as it was at the start of the operation. See Changing the Output Point for more information.

Approach, Retract and Linking Macros for Groove Turning

The following Approach and Retract macro modes are proposed: Direct, Axial-radial, Radial-axial, and Build by user.
The selected macro type (Approach or Retract) defines the tool motion before or after machining.

Various feedrates are available for the approach and retract motions (RAPID, lead-in, lift-off, and so on). Local feedrates can be set to either Angular units (length per revolution) or Linear units (length per minute).

See Define Macros on a Turning Operation for more information.

Linking Macros

Linking macros, which comprise retract and approach motion can also be used on Groove Turning operations.
Approach and retract motions of linking macros are interruptible. For Groove Turning only, you can interrupt the macro at the end of the number of specified levels. See Interruptible Macros for more information.

It can be useful to interrupt an operation when the foreseeable lifetime of the insert is not long enough to complete the machining.

 Behavior of Linking Macro when Grooving by Level

Groove turning can be done in one or more levels using the Grooving by Level mode. Also, you can define Linking macros and define interrupt modes of these macros.

Prior to Release 18, if the Linking macro is interrupted at the end of a level, the macro returns to the previous tool path and not to the next cutting motion.

As from Release 18, the macro returns to the next cutting position in the toolpath after retract from interruption at the end of a level.

A Linking macro returning to previous tool position and then moving to the next cutting position is considered a redundant move. As from Release 18, such redundant moves are avoided.