Rough Turning Operations

The information in this section will help you to create and edit Rough Turning operations in your Manufacturing Program.

The Rough Turning operation allows you to specify:

• Longitudinal, Face, and Parallel Contour roughing modes
• external, internal, or frontal machining according to the type of area to machine
• relimitation of the area to machine
• various approach and retract path types
• various lead-in and lift-off options with specific feedrates
• recess machining
• various contouring options with specific feedrates.

The following topics are dealt with in the paragraphs below:

• Tooling
• Geometry including Part and Stock Offsets
• Location and Limits
• Machining Strategy Parameters
• Feeds and Speeds
• Tool Compensation
• Macros.

Tooling for Rough Turning

The following tooling may be used:

• External and Internal insert-holders with all insert types except groove and thread.
• External and Internal 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.

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.

Note that the Insert-Holder Constraints setting does not influence the Leading and Trailing Safety Angles defined in the operation editor.

Geometry for Rough 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.

Multiple areas are not managed. If a profile with multi-domains is selected manually or by means of the automatic stock selection capability, only a single area is taken into account for machining.

The Start Limit option allows you to specify a point, line, curve or face as the start element of the Stock profile. If a face is specified, the start element is the intersection of the face and the working plane. The position of the start of machining is also defined with respect to this element by one of the following settings: None / In / On / Out. The Start Limit relimits input stock only and does not affect the part profile.

With the Selection of a valid Start Element (under Geometry tab) in one of its mode IN/ON and OUT mode, the Input Stock can be limited or varied in its length. The Machined area is calculated based on the Stock modified by this Start Limit. ToolPath begins from this Start element or Start limit based on the Limit mode chosen.

The following is explained for the Machining Strategies, Back Location External Rough Turning. Same is applicable for other options of Location and Orientation.

The Default Behavior without Start Limit definition for input stock (or Start Limit mode is None): Part is extended upto stock (which could be held in a chuck) and toolpath is calculated.




This shows the Highlight Behavior for Start Limit selected, for modes IN, ON and OUT. 
Start Limit Mode IN:



Start Limit Mode ON:

Start Limit Mode OUT:


The End Limit option allows you to specify a point, line, curve, or face to relimit or extrapolate the selected part profile. This also relimits the input stock. 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. The part profile is relimited or extrapolated in this direction. The input stock is also relimited by end element in this direction.

Note that location of start/end limit is based on the direction of machining as shown in the below image of Strategy tab. The following image displays the machining direction for Longitudinal Roughing mode, External Orientation, and Front Location Strategy.

The Stock Extension distance allows you to extend the stock in the machining direction and, to any desired length. This can be useful in Rough turning scenarios, where you want to machine beyond the stock profile. This extension is taken into account for tool path computation when an End Limit element is defined and used on the operation (when End Limit mode is different from None).

The extension distance defines the extended domain for tool path computation. Note that the End Limit is respected only when it is specified (according to the In / On / Out mode) inside the extended domain.

The figures below show that an End Limit is defined (selected and mode different from None) and a Stock Extension distance is defined (greater than 0).

The tool moves beyond the stock (extension distance). This distance defines the machining domain extension for tool path computation.

Note that in this particular case, the limit is not reached (In / On / Out) because it is outside the extended machining domain.

In the following examples, the following key is used to illustrate various cases of stock extension:

Example 1: End Limit beyond stock with no stock extension

Example 2: End Limit beyond stock but inside stock extension

Example 3: End Limit beyond stock and stock extension

Example 4: Stock extension with no End Limit

Example 5: End Limit inside stock and no stock extension

Relimiting the area to machine by means of limit elements

If you specify a point, it is projected onto the part profile.
A line through the projected point parallel to the radial axis delimits the area to machine.

If you specify a line, its intersection with the part profile is calculated (if necessary, the line is extrapolated).
A line through the intersection point parallel to the radial axis delimits the area to machine.

If you specify a curve, its intersection with the part profile is calculated (if necessary, the curve is extrapolated using the tangent at the curve extremity).
A line through the intersection point parallel to the radial axis delimits the area to machine.

Orientation for Rough Turning

The following Orientations are proposed: Internal, External, and Frontal (for Face and Parallel Contour Rough Turning only).

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. Selected part and stock profiles do not need to be joined (see the following figures).

External Rough Turning

Internal Rough Turning

Frontal Rough Turning

Frontal machining is proposed for face Rough Turning. In that case, the minimum and maximum diameters of the area to machine are determined by the stock profile dimensions.

For example, in the following figure the area to machine is relimited by the spindle axis because the stock profile is also relimited by the spindle axis.

Part and Stock Offsets for Rough Turning

• Stock offset: specifies a virtual displacement of the stock profile.
• Part offset: specifies a virtual displacement of the part profile.

  

• Axial part offset: specifies a virtual displacement of the part profile along the spindle axis direction.

  

  The following image shows offset of a part (located initially at Zero offset) due positive and negative Axial part offset value. This is applicable in general for any Orientation Strategy parameter .i.e. External, Internal etc.

  

• Radial part offset: specifies a virtual displacement of the part profile in the radial axis direction.

  

  The following image shows offset of a part (located initially at Zero offset) due positive and negative Radial part offset value. This is applicable in general for any Orientation Strategy parameter .i.e. External, Internal etc.

  

• Start Limit Offset: distance with respect to the start element (only if start element is a line or a curve, and when In or Out  is set for start element positioning).
• 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).

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.

Location and Limits for Rough Turning

The following machining Locations are proposed:

• Front, the part is machined toward the head stock
• Back, the part is machined from the head stock.

Orientation and Location settings determine the way the program closes the area to machine using radial, axial, axial-radial or radial-axial relimitation.

The following options allow you to restrict the area to machine that is pre-defined by the stock and part. You may want to restrict this area due to the physical characteristics of the tool and the type of machining to be done.

Minimum Machining Radius

Maximum Machining Radius (for internal machining)

Note that Max Boring Depth is defined on the tool.

Axial Limit for Chuck Jaws (for external or frontal machining): Offset defined from the machining axis system.

Machining Strategy Parameters for Rough Turning

Path Definition for Rough Turning

• Machining tolerance
• Max Depth of Cut
  This option is used to specify the maximum distance between passes.
  It is replaced by Radial Depth of Cut and Axial Depth of Cut for Parallel Contour Rough Turning.
• Leading and Trailing Safety Angles
  The insert geometry is taken into account to avoid collision by reducing the maximum slope on which the tool can machine. The Leading Safety Angle and Trailing Safety Angle allow you to further reduce the area to machine.
  Note that Trailing Safety Angle can be used only when Recess Machining is set.
  
  Leading and trailing angles can also be defined on the insert-holder to define the maximum slope on which machining can be done. In this case and if the Insert-Holder Constraints setting is applied (see above), the angles that reduce the slope the most will be taken into account.
• Part Contouring
  You can specify a contouring type for longitudinal and face Rough Turning in order to clear the part profile by means of the following settings:
  • No: no contouring
  • Each path: profile following at each roughing pass
  • Last path only: profile following at last roughing pass only.
• Under Spindle Axis Machining
  For Face and Parallel Contour Rough Turning with Frontal machining, this option allows you to request machining under the spindle axis.
• Machining Direction (only for Parallel Contour and Face Rough Turning with Frontal machining)
  You can specify the machining direction with respect to the spindle axis by means of the To/From Spindle Axis choice.
• Recess Machining (if Contouring Type is Each Pass or Last Path Only)
  If you require recess machining, activate this check box.
  When recess machining is active in Parallel Contour Rough Turning, Axial and Radial Depth of Cut must have suitable values to ensure a collision free tool path. See Recommendations below.

The following options are proposed for recess machining:

• Plunge Distance and Plunge Angle (for longitudinal and face Rough Turning)
  Define the plunge vector before each new pass with respect to the cutting direction.

Example of Recess with External Longitudinal Rough Turning

In the figure above the tool motion is as follows:

• approach in RAPID mode
• lead-in at the first recess pass and plunge approach for other passes
• plunge at plunge feedrate
• machine at machining feedrate
• contouring at contouring feedrate
• lift-off at last recess pass at lift-off feedrate.

Note that Trailing angle is defined on the tool.

Recommendations for Collision Free Recess Machining in Parallel Contour Rough Turning

Machining in Parallel Contour Rough Turning is done by means of successive offsets of the tool path: the offset depends on the axial and radial depth of cut values.
The following recommendations describe how to set the axial and radial depth of cuts to ensure a collision free tool path.

Parallel contour principle:
The parallel contours of the tool path are obtained by first shifting the last pass then shifting each successive pass depending on the axial and radial depth of cut values.

Then the passes are relimited taking into account the stock definition.

Correct combination of axial and radial depth of cuts
Compared with the left and right angles on the insert, the axial and radial depth of cut values define a shift direction that must be compatible with the insert.

The shift direction must be inside the limit angles defined on the tool insert otherwise a collision may occur. In collision cases, the collision is on the first pass, not on the last passes of the tool path.

Example of a correct combination

Example of an incorrect combination (right of tool)

The parallel contour tool path is in collision because the shift does not respect the tool insert angle on the right side.

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

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.

• Lead-in Distance and Lead-in Angle
  These parameters define the lead-in vector at the start of each pass with respect to the normal to the cutting direction.

Lead-in distance takes the stock profile and stock clearance into account. The tool is in RAPID mode before this distance.

If no lead-in angle is requested, the lead-in path is normal to the cutting direction.
For Longitudinal and Face Rough Turning the lead-in angle can be applied as follows:

• no angle applied to lead-in path
• lead-in angle applied to each path
• lead-in angle applied to last path only.

For Parallel Contour Rough Turning, the Lead-in angle is applied to each path.

• Attack Distance
  Defined with respect to the cutting direction and takes the stock profile and stock clearance into account.

• 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.

For Longitudinal or Face Rough Turning, lift-off occurs:

• at the end of each pass when Contouring Type is set to None or Last Path Only.
• At the end of the last pass of the operation when the contouring type is set to Each Path. This prevents the tool from damaging the part when returning to the end point in RAPID mode.
• at the end of each pass that ends on the stock profile.

For Parallel Contour Rough Turning, lift-off occurs when the end of the pass has already been machined by a previous pass.

Feeds and Speeds for Rough 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.

The value of the Maximum Spindle Speedparameter would initially be populated from the Max spindle speed parameter set in the Part Operation.

By default, the Maximum Spindle Speed is the same as the value set on the machine referenced by the Part Operation (via the Machine Editor > Machine Spindle tab). Default value is 6000.

If the Spindle Output option in checked, the maximum spindle speed value can be automatically output in the APT file at the beginning of the machining operation by defining the NC Command NC_SPINDLE_MAXSPEED in the pptable.

Example: *START_NC_COMMAND NC_SPINDLE_MAXSPEED MAXSPNDL/%MFG_MAX_SPNDL_SPEED, & MFG_MAX_SPNDL_UNIT, & MFG_SPNDL_WAY*END

NOTE: If the option Spindle Output is not checked, syntax corresponding to NC_SPINDLE_MAXSPEED would not be output but you still have the option to output the maximum spindle speed value by using the parameter %MFG_MAX_SPNDL_SPEED in other machining operation related instructions.

This value is also visible within the Process Table. You can change the value in Process Table  and tool path needs to be recomputed. The unit for Maximum Spindle Speed is always Angular. The maximum value you can enter in machining operation dialog box /Process Table is the value set in the Part Operation. The minimum value you can enter is 1.

• Compute tool path for machining operation.

• Right-click Maximum Spindle Speed parameter for machining operation and select Edit Maximum Spindle Speed from the contextual menu.

• Change value in Edit Parameter dialog box.

• Open machining operation dialog box, the Maximum Spindle Speed parameter value in Feeds and Speed tab is similar to the changed value.
  If you have not re-compute tool path than Maximum Spindle Speed changed value in Process Table and Maximum Spindle Speed parameter value in Feeds and Speed tab will not be same.

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

• Machining Feedrate
• Lead-in Feedrate which is applied during the lead-in and attack distance
• Lift-off Feedrate
• Contouring Feedrate (if contouring type is Each Path or Last Path Only)
• Plunge Feedrate (for longitudinal and face Rough Turning)
• 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 check box 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 machining operation 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 each path 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 Rough 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.

Approach, Retract and Linking Macros for Rough 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).

Linking macros, which comprise retract and approach motion can also be used on Rough Turning operations. Approach and retract motions of linking macros are interruptible. It can be useful to interrupt an operation when the foreseeable lifetime of the insert is not long enough to complete the machining.

See Define Macros on a Turning Operation for more information.