G-code based operation, G-code based lathe operation


NC program


the interpreter




the toolpath

G-code based operation >  and < G-code based lathe operation>  operations located in <Auxiliary> list. It can be also used for indexed and continuous processing at 4 and 5 coordinate machining centers. All available simulation types are supported, including additive manufacturing to simulate material layer buildup. G-code based lathe operation supports only turning tool. G-code based operation does not support the turning tool. The use of Wire EDM machining is not supported. These operations allow you to perform:

  • direct control of the machine simulation using G-codes;

  • check and optimize the NC program;

  • convert the text of the NC from one controller to another (for machines with identical kinematic scheme);

  • debug your own interpreter during its creation.

The toolpath is formed on the basis of the following operation parameters:

  • Specified NC text on the  < Job assignment > parameters panel;
  • Selected interpreter on the  < Strategy > parameters panel;

  • Assigned tool on the  < Tool > parameters panel.

The NC text > can be written manually or can be loaded from an external file and edited, if necessary. The built-in text editor supports syntax highlighting of the main key structures of the CNC programming language, as well as a wide range of keyboard shortcuts for working with text.

More detailed information about the possibilities of working with the NC text is described in the section < Job assignment for G-code based operation >

 < Interpreter file (*.snci) > defines the format of recognition of the controller commands in blocks of the NC program. The corresponding parameter specifies the full path to the selected interpreter. The parameter value can be entered manually as well as by using the file selection dialogue, which is accessed by using the  entered button. During the selection process, selection process, a preview of the interpreter information is available (description, purpose, CNC system, authors, etc.):

The ability to select an interpreter from the container is supported.

Currently, interpreters of the following CNC systems are available for use:

Machine groupCNC systemComment


MillingAPTImport toolpath only
Apt_Simplify_3DImport toolpath only
ISOImport toolpath only
Fanuc 30iTo simulate and import a toolpath
Haas VF-2To simulate and import a toolpath
Heidenhain iTNC 530To simulate and import a toolpath
NC210To simulate and import a toolpathAn additional license is required
Sinumerik 840DTo simulate and import a toolpath
Tormach PCNC Mach3To simulate and import a toolpath
Tormach PCNC PathPilotTo simulate and import a toolpath
Global controlImport toolpath onlyAn additional license is required
Turn-millingSinumerik 840DTo simulate and import a toolpath
Okuma OSP-P300To simulate and import a toolpathAn additional license is required
RobotFanuc robot (R-30iB controller)To simulate and import a toolpath
Kuka robotTo simulate and import a toolpath
Motoman robotTo simulate and import a toolpath
ABB robotTo simulate and import a toolpath

Note: All interpreters support command list generated by postprocessors in SprutCAM distribution kit only.

"Import toolpath only" interpreters are not supported matching line NC code - trajectory of tool movement.

When you select an interpreter, pay attention to its purpose (the Purpose field in the Preview pane)

The selected interpreter should be intended for simulation. Otherwise, the trajectory of the tool may be incorrect (shifted relative to the coordinate system of the workpiece, duplicated approaches/retracts, incorrect starting position, etc.).

 < Use advanced toolpath transformation >- the setting involves converting the NC trajectory into a geometric one, allowing you to modify it with a robot map and/or copying operation. If the setting is disabled, the final trajectory is formed without the possibility of changing it (the most accurately repeating the control program).

 < Step of physic movements dividing > - setting up is only available when using Use advanced toolpath transformation (see above). In this mode, at the first stage, the NC trajectory is transformed into a geometric curve. For maximum repetition of the original trajectory, machine movements are splintered. The routing step is set by this setting. The smaller the step, the more accurate the original trajectory will be.

 < Add unrecognized commands in the trajectory > - this parameter enables adding all unrecognized commands of the NC-program to the toolpath. Unrecognized commands will be added to the toolpath as the INSERT command text before the recognized commands.

Example of how the parameter "Add unrecognized commands in the trajectory" works

NC programThis parameter is disabledThis parameter is enabled

Commands M107, E - are not recognized by the interpreter

<The tool > that will be processed is determined on the corresponding tab of the operation parameters window. When creating G-code based operations, it is assigned a default tool for appropriate processing (milling or turning).

Note: Currently, the tool number indicated in the NC text is not taken into account when selecting from the list of project or library tools. Due to the above feature, only the NC text in which the processing is carried out by one tool can be assigned as a job assignment for each such operation.

G-code based operation demo video

 Watch demo video

See also:

Job assignment for G-code based operation, G-code based lathe operation

Keyboard shortcuts for working with NC text

Creating your own interpreter