Interface & commands

Loading a file: Notepad++ plugin

After installation is successful, the NCnetic plugin shows up in the Notepad++ plugin toolbar. By hitting the Plot/Refresh function, the 3D plot window appears, and the currently selected G-code file is simulated. To switch files or after editing the current file, you need to hit the Plot/refresh function again in order to plot the new or modified file.

If no “Languages” (also called lexer) have been applied to the currently displayed G-code file, the plugin will apply its own syntax highlighting.

Loading a file: Gcode viewer stand-alone application

After launching the application, click on the ‘Import’ button in the toolbar and select the file you want to plot.

Alternatively, drag and drop files from the Windows File Explorer.

You can also launch the standalone portable application via the command line by calling the .exe file and passing the file to plot as an argument:

Example: C:\NCneticPlayer.exe “C:\Users\MyUser\mill_pgm.nc”

Interface

If a .STL file is present in the same folder as the NC file and shares the same name (for example: mill_pgm.nc and mill_pgm.stl), the 3D model is plotted in the 3D view alongside the NC file. Alternatively, you can drag and drop an .STL file into the 3D view to plot it.

Selecting a move in the 3D view will jump to the corresponding line within the G-code file. Selecting a text line within the G-code file will select the corresponding move in the 3D interface. Additional information about the selected file and the selected move, such as coordinates, feeds, lengths, etc., are displayed in the right panel.

By dragging its handle left or right, you can show/hide the right-side panel, which provides additional details about the selected move, including length, coordinates, feed, spindle speed, and more Below the right-side panel, you’ll find buttons to execute various commands:

Below the 3D view control, you’ll find a toolbar with buttons for executing various commands:

• Import (stand alone only)
• Export
• Kill file processing
• Start simulation
• Stop simulation
• Previous
• Next
• Tool database
• Options & settings

In addition, a track bar allows you to navigate through the entire file line by line.

Interaction with the 3D interface is performed through commands:

• Selection (mouse left-click by default)
• Pan (mouse middle button by default)
• Rotate (mouse right button by default)
• Go back to default view and re-center view(double-click any mouse)

In addition to mouse commands, views can be adjusted by clicking on the corresponding face on the compass (XYZ axis display) located in the bottom-right corner of the 3D view.

Supported functions

Adresses

• N: Block number.
• x, Y, Z: Linear axis values (or macro inputs).
• A, B, C: Angular axis values.
• I, J, K: Arc center axis values.
• F: Feed rate.
• S: Spindle speed.
• R: Arc radius or rotation angle or drill cycle retraction value.
• L: Sub repetition or drill cylce repetition
• P: Sub number or scale factor
• T: Tool number

Gcodes

• G0: Rapid move.
• G1: Linear move.
• G2: Counter-clockwise arc.
• G3: Clockwise arc.
• G4: Dwell.
• G90/G91: Absolute/relative coordinates. 91.0 and G91.1 to for absolute / relative arc center.
• G17/G18/G19: Work plane selection (XY/XZ/YZ).
• G40/G41/G42: Tool radius compensations (None/Left/Right)
• G28: Home.
• G92: Set new reference.
• G52: Work offset / Reference shift.
• G53: Machine coordinate system.
• G54/G55/G56/G57/G58/G59: Work offset.
• G80/G81/G82/G83/G84/G85/G86/G87/G88/G89: Drill cycles.
• G50/G51: Scale program/Reset scale.
• G68/G69: Rotate program/Reset rotation

Comments

Any text following the character ; or ’ is considered a comment, as well as any text enclosed in parentheses.

Sub-programs

• Sub start: The character O followed by digits is considered a program or routine declaration.
• Sub end: M99 signals a return from a sub-program or routine, while M02 or M30 return from the main program.
• Sub call: To call a sub-program from the main program, use M98 P1234, where 1234 corresponds to the sub-program name (e.g., O1234).

Macro B

• Variables: The character # followed by digits is considered a variable. Variables can be assigned and then used for formulas and/or logic operations.
• GOTO: Jump to the target block number.
• IF: If/then logic operator.
• WHILE: While logic operator
• G65: Call a macro with input parameters.

Options & Settings

View

Inputs

Machines

Machine type

File type

Remap adresses

The default addresses [X, Y, Z, I, J, K, A, B, C, F, S, R] may not be suitable for all G-code files. For instance, while A typically represents rotation around the X-axis, B represents rotation around the Y-axis, and C represents rotation around the Z-axis, some CNC manufacturers may not adhere to this standard convention. In such cases, remapping the addresses can be useful.

Example:

We have G1 X100 Y50 Z20 U15 V30, where U represents the first rotation axis and V represents the second rotation axis of a 5-axis head-head machine. Addresses X, Y, and Z are standard, while U and V are specific to the machine we aim to simulate.

-> Remapping the addresses from A to U and B to V results in the correct G-code interpretation.

Export

Tool database

The interface is divided into three sections:

• Tool List: Displays the tool name, color, and station number where the tool is mounted. Use the ‘Add’, ‘Remove’, or ‘Copy’ commands to manage the tool list. Additionally, ‘Set Position’ buttons are available to quickly mount the selected tool in a station defined in the current NC file. Use ‘Set Position X’ to remove any assigned station number.
• Tool Settings: Allows configuration of all parameters for the tool selected in the tool list.
• Tool Geometry Representation: Shows a visual representation of the tool’s geometry.

Main

Geometry

4-axis and 5-axis

NCnetic includes all the essential tools to easily set up and simulate 4-axis and 5-axis NC files. This section covers the basic settings required to configure NCnetic for accurate simulations.

By convention, the addresses in the NC file are as follows:

• A: rotation around the X-axis
• B: rotation around the Y-axis
• C: rotation around the Z-axis

You can customize these by remapping the addresses in the options.

4-axis Rotary Tables

The most common type of 4-axis CNC machine has a part holder mounted on a rotary table to perform rotational machining, multi-side milling, or simply to change parts fixed on different sides of the table.

The origin of the Z-axis (Z=0) may coincide with the rotation axis (‘Rotary Z offset radius’=0, the default setting), or be on the surface of the part. In the latter case, the radius of the cylindrical part must be entered in ‘Rotary Z offset radius’.

4-Axis Tool tilting

This configuration often corresponds to a choice of toolpath representation rather than an actual hardware feature (although such machines do exist). In this case, the rotation values represent a tilt of the tool rather than the rotation of the part. The advantage of this notation is that the XYZ values for the tool position remain unaffected by the rotations.

“Tangential” tools

The ‘XYZ_C_HEAD’ configuration of a 4-axis machine is used when the rotation of the tool around its own axis is critical. A common example is tangential knife or blade cutting, where the cutter must be oriented in the direction of tool travel to cut the material accurately.

5-axis

5-axis CNC machines are designed so that, in addition to the three translational movements, two rotational movements allow the tool to be oriented in any direction. These rotations may affect either the part being machined, as in the table-table configuration; the tool, as in the head-head configuration; or one on each, as in the table-head configuration.

For a quick setup, set the ‘Machine Type’ option in the options to match your configuration. Use the ‘Include Sample’ flag to add a simplified 3D model of the kinematic chain for the current machine type. The ‘Inverted Rot’ option allows you to reverse the direction of a rotation axis, so that a positive angle results in a counterclockwise movement, or vice versa.

TCP mode

TCP mode is a special representation of tool orientation that can be activated with the ‘File Type’ option. In this mode, the content of the NC file is interpreted as though the machine operates in a head-head AC configuration, using azimuth and inclination angles, regardless of the machine’s actual kinematic chain. The advantage of this notation is that the XYZ values for tool position remain unaffected by the rotations.

Export & post-processor

Within CAM software, all the information needed to create a toolpath is stored in as standardized a format as possible. A CAM toolpath object contains a list of coordinates and direction vectors that the tool should follow, along with process inputs at each point such as movement type (rapid/feed), feed rates, spindle speeds, and tool properties like diameter and length, as well as any other relevant information for the machining task.

When it’s time to generate the NC file for a specific machine, the post-processor loops through all of this information and writes the correct sequence of commands into the NC file, which the machine will read, interpret, and execute.

Illustrating the concept with C#:

We have a (very) simplified toolpath structure:

class ArrayOfMove
{
    List<Move> Moves; // List of moves
}

Where each move has the following structure:

class Move
{
    string Type; // "Rapid"/"Linear"/...
    double TargetX; // X target position 
    double TargetY; // Y target position 
    double TargetZ; // Z target position 
}

The post-processor can be constructed as a function that takes such a Toolpath as input and prints the corresponding G-code into the NC file:

void PostProcess(ArrayOfMove toolPath)
{
    // Initialize file content variable
    string fileContent = "";

    // Loop through each move in the toolpath
    foreach (Move move in toolPath.Moves)
    {
        // Check the move type: G1 for linear feed, G0 for rapid
        if (move.Type == "Linear")
            fileContent += "G1"; // Feed move
        else
            fileContent += "G0"; // Rapid move

        // Add the X, Y, and Z coordinates to the file content
        fileContent += " X" + move.X.ToString();
        fileContent += " Y" + move.Y.ToString();
        fileContent += " Z" + move.Z.ToString();

        // Add a new line after each move command
        fileContent += "\r\n";
    }

    // Write the complete file content to a .nc file
    File.WriteAllText("C:\\myNCFile.nc", fileContent);
}

Building custom post-processor with NCnetic.

When NCnetic or any backplotter reads an NC file, it performs the reverse operation of a post-processor. The NC file is translated back into its standard native structure.

It is then possible to reprocess the file and output a new file format.

To do this, an ’export’ function is available, supporting XML, JSON, or CSV formats. In the ‘Options & Settings’ window, go to the ‘EXPORT’ section and select the ‘EXPORT FILE TYPE’. You can enable the ‘FILE DIALOG’ property (set it to true) to open a file-saving dialog window.

The output file can then be processed by a custom application by checking the ‘RUN EXE’ property and specifying an *.exe file in the ‘EXE PATH’ property.

When the ’export’ is performed, the executable is called with the exported file as an argument, which is equivalent to performing this action in a command prompt:

c:\MyCustomExe.exe "c:\ExportedFile.xml"

Additionally, it is possible to call a script by enabling the ‘INCLUDE SCRIPT’ property and specifying a script file in the ‘SCRIPT PATH’ property. For example, running Python with a *.py script during ’export’ is equivalent to performing this action in a command prompt:

python c:\MyPythonScript.py "c:\ExportedFile.xml"

The executable should read the exported file, extract relevant informations, and write (post-process) a new output file.

Practical code sample: DXF post-processor

The following code is the Program.cs content of a .Net console application. It will convert the XML export into a DXF file in the XY view (Use ‘EXPORT=XML’ & ‘FILE DIALOG=true’).

Download link: https://www.ncnetic.com/Program.cs.txt