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

< 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.

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.

< 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:

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

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

< Use advanced toolpath transformation >- this parameter converts the NC toolpath from machine to geometric. Which, in turn, makes it possible to correct the toolpath using the robot axes map. If the setting is disabled, then the final toolpath is formed (as closely as possible repeating the one specified in the NC program), without the possibility of changing it.

< Step of physic movements dividing > - available only when using Use advanced toolpath transformation (see above). In this mode, at the first stage, the tool path is converted into a geometric curve. At the next stage, machine movements are rasterized with the step specified in the current parameter to ensure maximum similarity with the original toolpath. The smaller the value of the rasterization step, the higher the accuracy of construction and, accordingly, the similarity with the original toolpath.

< Add unrecognized commands in the trajectory > - this parameter adds all commands of the control program not recognized by the interpreter to the toolpath. Unrecognized commands are added to the tool path description as a technology command parameter < INSERT > before the recognized commands.

< Radius compensation mode > - A bility to disable or set an arbitrary compensation value on the tool radius.

< 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.

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