Strategy Parameters
- Tool Axis
-
The Tool Axis command in the Turning
Operations dialog box is represented by an arrow when
creating a part operation.
See Defining the Tool Axis
- Max Depth of Cut
- Specifies the maximum distance between passes.
- Min Depth of Cut
- Specifies the minimum distance between passes.
- Recessing Strategy
- Specifies recessing strategy as:
A Mill turn operation which
allows machining a Recess in a One Way or Zig Zag Tool motion. This is
basically suitable for machining hard materials using round ceramic
inserts, thereby minimizing wear and cutting stress. Here you have
the flexibility to define Minimum depth of a cut. This results in a
behavior where machining is progressive with passes of different
thickness varying between Maximum
depth of cut and Minimum depth of cut.
Following is the
progressive Machining behavior by defining Maximum depth of cut and
Minimum depth of cut:
- Orientation
- Specifies the orientation.
You can specify:
- Internal
- External
- Frontal
- Other: Specifies the
Angle of Incline, for an
Other orientation.
The selected orientation defines the type of geometric
relimitation to be done between the rough stock and part geometry in
order to determine the area to machine.
The following
- Machining Direction
- Specifies the machining direction.
You can specify:
- To Head rough stock or
From Head rough stock for
Internal and
External orientation.
- To Spindle or From
Spindle for Frontal
orientation
- Right of Groove or Left
of Groove for Other
orientation.
When a part profile has multiple recesses (that is, a non-convex
profile along the cutting direction), only the first recess along
the specified direction is machined.
- Part Contouring
- Select this check box to specify part contouring, if contouring is
required.
The part profile is followed at the end of recessing.
This is done by machining down the sides of the recess in order to
clear the profile (1 - Lift-off distance, 2 - Part Clearance, 3 -
Part Geometry).
- Under Spindle Axis Machining
- Select this check box to request machining under the spindle axis. This
option is available for Frontal
orientation.
- Change Output Point
- Select the Change Output Point check box to
automatically manage the change of output point. Change Output
Point.
If the output point is consistent with the
flank of the recess to be machined, the output point is changed when
the other flank of the recess is machined. At the end of the
Machining Operation, the output point is the same as it was at the start of the
Machining Operation. For more information, please refer to the Tool Output Point Change.
- Tool Compensation
- Select a tool compensation number corresponding
to the desired tool output point.
The usable compensation numbers are defined on the tool assembly
linked to the Machining Operation.
By default, the output point corresponding to type
P9 is used, if you do not select a tool
compensation number.
- Tool Axis Flip
- This flips the Tool Axis.
- Initial Depth of Cut
- This enables more flexibility in machining by entering the Initial and
final depth of the cut. This gives you more control over machining
through a variable depth of the cutting behavior. The Maximum depth of
the cut is ignored in this case.
- Final Depth of Cut
- This enables more flexibility in machining by entering the Initial and
final depth of the cut. This gives you more control over machining
through a variable depth of the cutting behavior. The Maximum depth of
the cut is ignored in this case.
Option
- Angle and Distance before Plunge
- Specifies the plunge vector before each new pass
with respect to the cutting direction.
- Entry and Exit Flank Angles
- Specifies the entry and exit flank angles for Zig
Zag mode only.
The insert geometry is taken into
account to avoid collision by reducing the maximum slope on which
machining is done. Defining Entry and Exit Flank
Angles on the Machining Operation allow you to further reduce the area to machine.
Leading and trailing angles can also be defined on the insert-holder
to define the maximum slope on which machining is done. In this case
and if the Insert-Holder Constraints setting
is applied, the angles that reduce the slope most are taken into
account.
- Flank Gouging Angle
- Specifies the flank gouging angle.
Flank gouging angle are for
Zig Zag mode only. Angles of the insert
are taken into account to avoid collision by reducing the maximum
slope on which machining is done. Defining a flank gouging angle
allows you to further reduce the area to machine.
A gouging angle can also be defined on the insert-holder to define
the maximum slope on which machining is done. In this case and if
the Insert-Holder Constraints setting is
applied, the angle that reduces the slope most are taken into
account.
- Plunge distance for 1st flank
- Specifies the plunge vector before each first pass with respect to the
cutting direction.
- Plunge distance for 2nd flank
- Specifies the plunge vector before each second pass with respect to the
cutting direction.
- Machining Tolerance
- Specifies the maximum allowed distance between the theoretical and
computed tool
path.
- Insert-Holder Constraints
- Specifies insert-holder constraints as:
The following attributes (located on the Insert-holder
Technology tab) may influence machining:
See Creating and Editing Milling, Drilling, and Probing Tools:
- Trailing angle
- Leading angle
- Maximum recessing depth
- Maximum boring depth
These attributes take tooling accessibility into account and may
reduce the machined area.
However, you can use the Insert-Holder
Constraints option to either ignore or apply these
tooling attributes. You can replay the Machining Operation to verify the influence of these attributes on the generated tool
path.
The Insert-Holder Constraints setting does not
influence the leading and trailing safety angles.
Rework
- Lift-off Distance and Lift-off Angle
- Specifies the lift-off vector at the end of the last pass with respect
to the cutting direction.
The figure below shows the effect of a
positive lift-off angle for external machining (1- Lift-off vector,
2 - Positive lift-off angle, 3 - Cutting direction).
- Rework Mode
- Select this check box to make the following options available:
- Distance before Rework Plunge
- Angle before Rework Plunge