Define Macros on a Milling Operation

task target This task shows you how to define macros on a milling operation.

This is done using the Macros tab page of the machining operation editor. In this example you will add circular approach, circular retract, and linking macros to a Profile Contouring operation.

For more general information about macros, see NC Macros.

task target

Predefined Macros

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. You can then adjust parameters of the macro (such as path length and feedrate).

User-Built Macros

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.

In addition, the following icons allow you to:

remove all macro paths
remove current macro paths
copy the paths defined on the Approach macro on to the approach paths of other macros or copy the paths defined on the Retract macro on to the retract paths of other macros.

Macro Edition

A sensitive icon representing the elementary paths of the macro will help you to build or edit your macro. The current macro path is colored violet. Right-clicking a macro path gives you access to a contextual menu.


  • Deactivate: Deactivates the selected macro path.

  • Activate: Activates a path that was previously deactivated.

  • Feedrate: Allows you to modify the feedrate type associated to the selected macro path by making a selection in the sub-menu. If local is selected, you can assign a local feedrate value.

  • Parameter: Gives access to parameters of the selected macro path.

  • Delete: Deletes the selected macro path.

  • Insert: Inserts a macro path depending on the type chosen in the sub-menu.


Inherited Macros

If you create a machining operation and there are other operations of the same type in the program, the new operation will inherit the macros used in the most-recently edited operation of the same type. An operation is considered edited when you click OK to quit the operation definition dialog box.

Create a Profile Contouring operation as described in the Prismatic Machining User's Guide.
scenario 1. Double-click the Profile Contouring operation in the specification tree to edit that operation.
2. Select the Macros tab page in the operation definition dialog box. The initial status of all the macros in the Macro Management list is Inactive.
3. Right-click the Approach macro line and activate the macro by means of Activate.

In the Current Macro Toolbox select the Circular horizontal axial mode.

A sensitive icon representing the 3 elementary paths of this macro appears.

4. Double-click each elementary path to display a dialog box that allows you to specify the exact characteristics the path.

The following dialog box allows you to specify the exact characteristics of the circular path.

Set the values of the circular approach paths so as to have a 10mm vertical path followed by a 15mm radius circular path.

5. You can then click Replay to check the circular approach. The status of the macro becomes Up to date.
6. Activate the Retract macro in the Macro Management list and create a circular retract macro in the same way.
7. Select the Linking Retract macro line in the Macro Management list, then in the Current macro Toolbox select the Axial mode.
8. Double-click the displayed value, then assign a 20mm value to the retract path.

9. Select the Linking Approach line in the Macro Management list, then select the Axial mode. Assign a 20mm value to the approach path.
10. In the Options tab, select the Cornerized clearance with radius check box, then enter a corner radius value of 3mm.


Click Replay to validate the tool path. Make sure that the Different colors mode is activated by selecting this icon in the Tool Path Replay dialog box.

  In the Replay dialog box select the By colors mode in order to visualize feedrate changes. The tool path is displayed with the following colors:
  • Yellow: approach feedrate
  • Green: machining feedrate
  • Blue: retract feedrate
  • Red: Rapid feedrate
  • White: user-defined feedrate.

Please note that  transition paths are represented by dashed white lines.

    The status of the macros are now Up to date.

12. Click OK to accept the modifications made to the operation.

The operation is updated with the specified macros.

task target

PP Words in Macros

You can insert PP words in macros by double-clicking the green X symbols in the sensitive icons.

The PP Words Selection dialog box is displayed. You can enter the syntax in the following ways:

  • enter one or more PP word syntaxes directly in the text field
  • click to access the PP words table that is referenced in the current part operation. You can then select predefined syntaxes from this table using the dialog box that appears.

For Pocketing and Profile Contouring operations, you should select the NC_CUTCOM_ON instruction in the list of available syntaxes if you want the program to interpret cutter compensation automatically (that is, by a CUTCOM/LEFT or CUTCOM/RIGHT instruction). If you choose different syntax in the list, it will be used as selected.
The methodology for this is described in the section "How to Generate CUTCOM Syntaxes" in  the Prismatic Machining User's Guide.

Default Linking Macros in Case of Collision

If a user-defined linking macro is not collision free, a default linking macro is applied.

Macro Motion Tangent to Tool Path and Parallel to Tool Axis

When the tangent to the tool path is parallel to the tool axis, the following macro motions are replaced by an axial motion:

  • tangent motion
  • normal motion
  • circular motion
  • ramping motion.

Helix Approach Macro

For Pocketing, Profile Contouring, Multi-axis Curve Machining and Multi-Axis Flank Contouring operations, a Helix approach macro can be used rather than a Ramping approach macro when a cutter approaches raw material.

The helix is specified by defining radius, height and angle values.

The figure below illustrates a helix approach macro when the Direction of cut is Climb and the tool's Way of rotation is Right:

The figure below illustrates a helix approach macro when the Direction of cut is Conventional and the tool's Way of rotation is Right:

end of task