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.
You build the macros using the interface provided under the Macros tab page in the Machining Operation Definition dialog box.
You can use predefined macros. These are made up from one or more paths in a specific order. Just select the desired mode in the Current Macro Toolbox of the Macros page. You can then adjust parameters of the macro (such as path length and feedrate).
You can also build your own macros using the Build by user mode.
Depending on the context, you can use the following icons to specify macro paths:
tangent motion
normal motion
axial motion
circular motion
ramping motion
helix motion
PP word
motion perpendicular to a plane
axial motion to a plane
motion perpendicular to a line
distance along a given direction
tool axis motion
motion to a point.
If the current macro ends with a PP word, PP word
becomes inactive and so you cannot add another successive PP word. For example
in the following sequence of macro paths ending with PPword.2:
...-TangentMotion-PPWord.1-CircularMotion-PPWord.2
you cannot add another PP word directly after PPword.2. However, you can edit and complete PPWord.2.
If the current macro ends with an axial path (Axial, Axial to a plane, Axial
perpendicular to a plane), the following icons become inactive:
Tangent motion,
Circular motion,
Normal motion,
Ramping motion.
This is because there is insufficient information about conditions such as tangency
or normal to the axial path.
Note that this behavior is not applied to 3-axis surface machining operations
(the icons remain active).
This type of motion is available for most prismatic and axial machining operations.
Select Motion perpendicular to a line
.
The motion is symbolized in the Current Macro Tool box by a linear path going to a Line symbol.
Select the Line symbol to display the following dialog box.
Select the desired method to specify the line orientation from the proposed list:
Just click OK to accept the specified orientation.
Example:
Motion starts and ends at the same linear location for each machining level.
For a ball-end tool, the tool axis motion in the macro is achieved by a rotation around the center point of the tool. In this case, a small circular arc tool path is created.
For other tool types, the tool axis motion comprises a rotation around the tip point of the tool.
An Approach macro is used to approach the operation start point. It is available for all machining operation types.
A Retract macro is used to retract from the operation end point. It is available for all machining operation types.
A Linking macro may be used in several cases, for example:
You could specify a Linking macro to do the following:
A Return on Same Level macro is used in a multi-path operation to link two consecutive paths in a given level.
For example, you could define a Return on Same Level macro on a Profile Contouring operation in One Way mode to do the following :
Note that no Return on Same Level macro is needed on a Profile Contouring operation in Zig Zag mode. The motion between two paths is done at machining feedrate by following the profile of the boundary.
A Return between Levels macro is used in a multi-level machining operation to go to the next level.
You could define a Return between Levels macro to do the following:
A Return to Finish Pass macro is used in a machining operation to go to the finish pass.
For example, you could define a Return to Finish Pass macro to do the following:
A Clearance macro can be used in a machining operation to avoid a fixture, for example.
You could define a Clearance macro to do the following:
These conventions concern both Circular and Tangent motions.
For Circular motions
,
position of the circle is defined by the Angular orientation parameter.
For Tangent motion
,
direction of the motion is defined by the Horizontal angle parameter.
The following types of operation are concerned.
This concerns the following operations:
Profile Contouring
Pocketing
Multi Axis Flank Contouring
Multi Axis Curve Machining in Side or Tip mode (between two curves or between
curve and surface).
For Circular motion:
Angular Orientation = 0.0 deg => Circle on the free side of the flank
Angular Orientation = 90 deg => Vertical Circle
Angular Orientation = 180 deg => Circle on side to the flank
For Tangent motion:
Horizontal Angle = -90 deg => Motion on the free side of the flank.
Horizontal Angle = 0.0 deg => Motion along Tangent
Horizontal Angle = 90 deg => Motion on side to the flank
This concerns the following operations:
Isoparametric Machining
Multi Axis Sweeping
Multi Axis Contour Driven
Multi Axis Curve Machining in Contact mode.
For Circular motion:
Angular Orientation = 0.0 deg => Circle on the free side of the bottom
Angular Orientation = 90 deg => Vertical Circle
Angular Orientation = 180 deg => Circle on side to the bottom
For Tangent motion:
Horizontal Angle = 90 deg => Motion on the free side of the bottom.
Horizontal Angle = 0.0 deg => Motion along Tangent
Horizontal Angle = -90 deg => Motion on side to the bottom.
For some machining operations, the Compensation output option can be activated to manage the generation of cutter compensation instructions in the NC data output.
However, note that a CIRCLE syntax may not be generated for a circular macro: the circle may be discretized and GOTO instructions generated instead. To obtain a CIRCLE syntax:
