4. Program Settings

Program Settings panel permits to sets the Control Software behavior.
The following images represent the settings captured from the default machine just as after a clean installation and are only for samples.

Units Mode

Permits to define the Units Mode used in the Control Software UI between Metric (mm) and Imperial (in).

It ONLY sets the measures representation in the UI so, in the G-Code, the Units Mode can be defined with a G20 or G21 and can be different than UI.

During the G-Code Program/Macro/MDI execution, G20 and G21 commands can be freely mixed but UI representation will be fixed to this setting.

All fields and settings of the UI are affected by the Units Mode except for Board Settings which are always expressed in the Metric System.

Enable Automatic Update Check

If enabled actives automatic check, at Control Software start and every 3 minutes, of online updates.

If an update is available a blinking advice message will be shown in Control Software Status Bar.

If disabled you can manually check if an update is available with the main menu Help → Check for Updates.

Update Manager checks for online updates regarding only the current version, eg: 1.9.x search only for 1.9 branches.

The update Check feature can be locked, to the end-user, using Access Levels settings.

PS: During the Update phase, if Windows UWF Status is found Enabled, the update procedure will be stopped because is not possible to update permanently files in a UWF protected disk.

Enable Automatic Connection with the CNC Board

If enabled it actives automatic connection with CNC Board at Control Software starts.

Enable Overwrite of CNC Board Settings at Connection

When Control Software opens a connection with CNC Board it checks if Board Settings in CNC Board are the same as Board Settings stored on Control Software.

If settings are different, and this option is enabled, the Control Software automatically sent Board settings on Control Software to CNC Board.

If this option is disabled, a prompt user dialog will show the state and will ask the end-user to Download Control Software Board Settings to CNC Board or Upload CNC Board settings to Control Software.

This feature is very useful when the same CNC Board is used in a CNC machine that uses more than one configuration, such as a 3-Axis vertical spindle or a 4-Axis horizontal spindle.

Enable the Opening of the Default Folder on Request of the “Open File…” Dialog

If enabled it permits to define the default folder open on Request of the main menu File → Open File… dialog or pressing the F12 key.

Special Windows folder shortcuts can be used here (for eg. %APPDATA%, to reach the user application data folder).

Enable Checking if the Loaded G-Code File Content is Modified by Another Program

If enabled it permits to define how to update the loaded G-Code file when a new version is available.

This happens, for eg., when a user asks CAM to create a new G-Code output file or when the G-Code file is modified by the user with a text editor.

Four different actions could be chosen:

• Ask user what to do if the system is ready

When the loaded G-Code program changes externally, and the CNC is in IDLE, a prompt dialog asks the user what to do.

• Ask user what to do when the system will be ready

When the loaded G-Code program changes externally, and the CNC is not in IDLE the check system waits for CNC IDLE, then a prompt dialog asks the user what to do.

• Load automatically newer file content if the system is ready

When the loaded G-Code program changes externally, and the CNC is in IDLE, the G-Code program will be automatically reloaded.

• Load automatically newer file content when the system will be ready

When the loaded G-Code program changes externally, and the CNC is not in IDLE the check system waits for CNC IDLE, then the G-Code program will be automatically reloaded.

Start Visible

Defines if the Start button will be visible, or not, in the CNC Board Control Bar.

Pause Visible

Defines if the Pause button will be visible, or not, in the CNC Board Control Bar.

Stop Visible

Defines if the Stop button will be visible, or not, in the CNC Board Control Bar.

Resume Visible

Defines if the Resume button will be visible, or not, in the CNC Board Control Bar.

Enable Jog With Keyboard

Enables the Jog control with the keyboard.

With the Keyboard is possible to control X-Axis (Left/Right keys), Y-Axis (Up/Down keys), and Z-Axis (Page Up/Page Down keys).

To do Jog with the keyboard the Jog Controls panel axis control must be visible and focused.

To focus it click the mouse in the near zone or press the F1 key one or two times till the blue focus rectangle is shown.

Auto Disable Jog Space Mode

Enables the auto-disable of Jog Space Mode.

When Jog movements are made with the Jog Controls panel and the Jog Space field is checked, with Auto Disable Jog Space Mode active, at end of the movement the Jog Space field will be automatically disabled.

Fixed Distance with CTRL + Fast Click

Defines the fixed distance used when with the CTLR key pressed a fast key/left-mouse click is done in the desired axis movement.

When the CTRL key is pressed a fast click, below 500 ms of duration, moves the selected axis of programmed distance.

When the CTRL key is pressed a long long click, over 500 ms of duration, executes a normal Jog axis movement but with an initial delay of 500 ms required to detect if in the fixed distance mode.

Dynamic Offsets permit to add positive/negative offset to X/Y/Z-Axis during CNC working using the related floating panel.
A change of Dynamic Offsets is possible only with CNC in RUN State and in a range of +3/-3mm.
Don't use Dynamic Offsets during RTCP enabled movements (G43.4 or G43.7).

Enable Dynamic Offset X

Enables the Dynamic Offset feature for X-Axis.

Enable Dynamic Offset Y

Enables the Dynamic Offset feature for Y-Axis.

Enable Dynamic Offset Z

Enables the Dynamic Offset feature for Z-Axis.

Dynamic Offsets Step

Defines the minimum step (+ or -) of Dynamic Offsets value change.

Modal Macro Motion Mode

Define the default motion mode used to perform the movements between two custom macro repetitions (Look at Modal Macro calls):

• In Fast - G0

A fast movement with the G0 command will be performed.

• In Feed - G1

A feed movement with the G1 command will be performed.

In the G-Code Program/Macro/MDI, with the G10 L100 P5800 V<value> command is possible to specify a different value from the default (#5800 = 0 → G0; #5800 = 1 → G1).

At the start of the G-Code Program/Macro/MDI, the default motion mode value will be always restored.

Cutter Compensation Option

Defines how the CNC Board will manage the Tool Cutter Compensation enabled with G41/G41.1 and G42/G42.1 commands.

The available options are:

• NIST

The default NIST mode.

• Easy Lead-In

Delays the first movement of the entry move until the following line or arc is specified.

When the second entry motion is specified it performs the entry move to a position tangent to the beginning of the second line or arc.

This option works well with some CADs such as Fusion360 indeed no gouging errors are generated.

• Normal

It is the only option that can handle concave corners and concave arcs.

PS: For more info look at Tool Compensation Entry Options.

Cutter Compensation Gouging Threshold

Defines the cutter compensation gouging threshold applied to G41/G41.1 or G42/G42.1 commands when Cutter Compensation Option is set to Normal.

Arc Radius Tolerance

Defines the maximum accepted difference of the distance between the start point and the center of an arc and that between the end-point and the center of the arc before generating a compilation error.

The value should be also equal to or higher than the greatest axes quantum movement (Axis Quantum = CNC Board axis Measure / Pulses).

Infinite Loop Threshold

Defines how to manage a possible infinite loop in WHILE commands.

When the value is set to 0 means: Continue till the WHILE expression is satisfied or the user press the ESC key to abort the current compilation.

When the value is set > 1 means: Continue till the WHILE expression is satisfied or the user press the ESC key to abort the current compilation or the n-value loops are reached.

Esample of an infinite loop:

  #1=0
  WHILE [#1 LT 10] DO 01
    G91 G01 X5
  END01  

In this case the coder missed to increment #1 value (eg: #1=[#1+1]) so the loop with Infinite Loop Threshold = 0 will continue to infinite.

For example with Infinite Loop Threshold = 10000, after 10000 loops the compiler will notice an error and stop compiling automatically.

Block Delete

Enables Block Delete management.

Block delete is used in a program by placing a forward slash (/) at the beginning of the line.

It is a useful function that allows the operator to skip the blocks within the program.

When the Block Delete option is enabled, and G-Code Editor Block Delete icon is active, all G-Code lines with / will be disabled and not executed.

The G-Code located to the right of an enabled Block Delete is still subject to syntactic check even if the code execution will be skipped:

G43 Persistent

Defines if G43 compensation is persistent in CNC Board at end of a G-Code Program/Macro/MDI execution.

G52 Independent

Defines if G52 is independent between changes of active WCS in a G-Code Program/Macro/MDI execution.

G92 Persistent

Defines if G92 offsets are persistent in the CNC Board at end of a G-Code Program/Macro/MDI execution.

Origin Offset Persistent

Defines if the changing of the selected World Coordinate System (WCS) made in the G-Code Program/Macro/MDI is kept at end of code execution:

• Checked

At the start of the program execution, the current active WCS is used.

At the end of the program execution, any changing of selected WCS with the G54/G55/G56/G57/G58/G59.1/G59.2/G59.3 commands will be kept.

In the case of the program stop, the current selected WCS is kept.

• Unchecked

At the start of the program execution, the current active WCS is used.

At the end of the program execution, any changing of selected WCS with the G54/G55/G56/G57/G58/G59.1/G59.2/G59.3 commands will be lost and WCS 1 (G54) is applied.

In the case of the program stop, the current selected WCS is kept.

The changes to any WCS origin offset values made with the G10 L2 Pp Xx Yy Zz Aa Bb Cc command are not affected by this parameter.

Enable User M Code Arguments

Define if the user-defined M macros will accept arguments, eg: M201 A10 J-1.3.

Enable the Creation of Simulator Data

Defines if the creation of Simulator Data is enabled.

Disabling Simulator Data will improve G-Code program compilation time and will reduce the memory used by the PC.

In the 32-bit version of the control software, when the estimated execution time of the G-code exceeds 5 hours, the simulator data is automatically disabled.

User Macro Path Mode

Two types of macros are available in the G-Code language: Machine Macros and User Macros.

The Machine Macros are stored in the folder %APPDATA%\RosettaCNC-1-\<machine>\macros.

To quickly reach the actual Machine Macros folder, you can use the “File → Open Macro Folder” menu.

Machine Macros can be used to create new G & M commands, provide well-defined CNC functions such as tool change, or subroutines that can be called up by number/name using the M98/G65/G66/CALL commands.

User Macros can be ONLY used to create subprogram callables by name.

User Macro Path is used ONLY if the subprogram is called with the prefix /, eg: G65 P“/square_pocket.ngc” W100. H100. Z-40. R-5. T2.

The User Macro Path Mode allows this by choosing from the following options:

• Disabled

The User Macro feature is disabled.

• GCode File Path

The User Macros are searched in the same path as the currently opened G-Code Program.

• User Defined Path

The User Macros are searched in the below-defined path.

Path

Defines the path where the User Macros are stored when the User Defined Path option was chosen.

Machine Axes Positions when CNC is Disconnected - MAPD

Defines the machine axes positions used in Control software when not connected with a CNC Board.

Typically these values are used how axes start points during G-Code simulation with internal software Simulator and without a CNC Board connected.

The System Macro restart.ngc manages all the activities necessary to START machining from a specific program line or to RESUME machining stopped with a STOP command from the last executed line or from one of your choice. However, when the macro is not available, a series of minimal operations are performed.
The following parameters allow you to configure these operations.

Default Movement Mode

Defines how the CNC make the default movements to start Start/Restart from a line from:

• In Feed - G1:
  default movements will use the G1 command (feed movement).
• In Fast - G0:
  default movements will use the G0 command (fast movement).
• Handheld by the PLC:
  default movements are managed by PLC internal strategy.

First Movement Speed

Defines the default movement speed when Default Movement Mode is set to In Feed - G1.

Max Distance

Defines the maximum accepted distance between the actual CNC position and the first CNC target position described in the G code.

If the distance is greater than Maximum Distance, an error message will be displayed in the dialog box and no movement will be made.

Force Tool Measurement

If enabled, if the currently loaded tool is different from the required tool, the Tool Change procedure will be forced otherwise an error message will signal the case and no movement will be performed.

PS: This is a very poor way to manage a START/RESTART from a line. The use of the restart.ngc macro is the right way to get better management of that.

Select Language to Use

Permits to define the UI language to use choosing from available languages.

Any change of current language requires a Control Software re-start to be fully applied.

PS: The Default item means “Use current computer default language, if present in the list, otherwise use the English language”.

Through the API Server, the Control Software exports a part of its API which can be used with external client applications.
The API server is a TCP/IP Server listening on localhost with a communication protocol based on JSON Request/Response packets.

The API Server, if enabled, will be activated automatically when the Control Software is started.
If, when starting the Control Software, the API Server Listening Port is found to be already in use, the following dialog will be displayed:

Enable API Server

Enabled the Control Software API Server.

Listen Port

Localhost Listening Port of the API Server.

It can be any localhost port not already used in the range 0 to 65535.

Enable “Cmd” Commands Group

Enable the API Server “Cmd” commands group.

Enable “Set” Commands Group

Enable the API Server “Set” commands group.

Enable “TLS” (Transport Layer Security)

NOT YET IMPLEMENTED!

PS: The changes to the API Server will take effect the next time the Software Control is started.

This panel displays all the Network Adapters for the Internet Protocol version 4 that can be reached by the Control Software.
For each adapter in the list, the IP address, the NET MASK and the NET NAME are available.

Update List

Updates the list of Network Adapters.

This is necessary if you change the Network configuration, eg: enabling a new LAN/WIFI connection.

IP

Defines the IP of the CNC Board to connect with.

Change IP

Permits to discovery and change the IP Settings of the CNC Boards connected in the Network.

For more information, see the “How To: Change Board IP” page.

Grid Size

Defines the size of the Grid used to represent the XY-Axis area in the machine coordinates.

Grid Z Position

Defines the Z machine coordinate where the Grid will be placed.

Is usual to place this value at the same Z-Axis Min Limit value.

Initial View

Defines the initial 3D view mode used as default when the Control Software is executed.

The graphical engine will automatically fit the 3D scene objects to be all shown in the display.

Choose one of the following values:

• Front

  The initial view will be on the front of the CNC.

• Back

  The initial view will be on the back of the CNC.

• Top

  The initial view will be at the top of the CNC.

• Bottom

  The initial view will be at the bottom of the CNC.

• Left

  The initial view will be on the left of the CNC.

• Right

  The initial view will be on the right of the CNC.

• ISO 1..9

  The initial view will be one of the ISO perspective modes.

• Custom View 1..4

  The initial view will be one of the ISO perspective custom modes.

Scene AntiAliasing

Defines the strength of Antialiasing filter applied by the graphical engine to 3D scene:

• Default

  Antialiasing disabled (will take the first available pixel format).

• None

  Antialiasing disabled (will take the first available pixel format).

• (MSAA): 2x

  Multisampled Antialiasing (MSAA): 2x.

• (MSAA): 2xHQ

  Multisample Antialiasing (MSAA): 2x High Quality.

• (MSAA): 4x

  Multisampled Antialiasing (MSAA): 4x.

• (MSAA): 4xHQ

  Multisampled Antialiasing (MSAA): 4x High Quality.

• (MSAA): 6x

  Multisampled Antialiasing (MSAA): 6x.

• (MSAA): 8x

  Multisampled Antialiasing (MSAA): 8x.

• (MSAA): 16x

  Multisampled Antialiasing (MSAA): 16x.

• (CSAA): 8x

  Coverage Sampled Antialiasing (CSAA): 8x.

• (CSAA): 8xHQ

  Coverage Sampled Antialiasing (CSAA): 8x High Quality.

• (CSAA): 16x

  Coverage Sampled Antialiasing (CSAA): 16x.

• (CSAA): 16xHQ

  Coverage Sampled Antialiasing (CSAA): 16x High Quality.

Default and None are similar but not the same.
Default does not touch the settings related to sample buffers of the OpenGL context from what defined in GPU Windows Settings.
None disables WGL_SAMPLE_BUFFERS_ARB and therefore the Anti-Aliasing management completely.

MSAA stays for Multi Sampled Antialiasing.
CSAA stays for Coverage Sampled Antialiasing.

Coverage Sampled Antialiasing (CSAA) is supported by NVIDIA cards (CSAA Tutorial)

Scene Nuance Mode

Xxx…

Scan Points Colors

Xxx…

Scan Mesh Colors

Xxx…

Hide Tool

Xxx…

Path Line Size

Xxx…

Tool Tip Size

Xxx…

Resolution

Xxx…

Set Number of Points per Block

Xxx…

Points per Block

Xxx…

Load

Permits to load a saved theme from a file.

Save

Permits to save the current theme in a file.

Tool xx0..xx9

Defines the colors assigned to Tools.

The color assigned to the Tool depends on the last Tool digit number.

Eg: Tool 1, 11, 21, .. share the same Tool color as 2, 22, 92, and so on.

Model

Defines the color of the G-Code program Model geometry.

The G-Code program model is an STL file with the same G-Code program name, but extension STL, loaded when a G-Code program is loaded.

Background

Defines the 3D scene background color.

This color is used when in the machine customize path is not available the background.png background image.

If in machine customize path is available the background.png image the system will use the image instead of background color.

Rapid Move

Defines the color for toolpath G00 (rapid) movements.

Grid

Defines the color of the working area Grid.

Tool

Defines the color of the Tool Body.

Tool Tip

Defines the color of the Tool Tip Body.

Scan Points

Defines the color of Scan Points during Scanning 3D/Scanning Surface features.

Scan Mesh

Defines the

Axis Text

Defines the color of the Axis text in MCS origin.

User Message Text

Define the color of the User Message for the M109 command.

Float Panels Border

Defines the Float Panels border color for Jog/MDI/etc.

Name

Xxx…

Size

Xxx…

Tab Size

Xxx…

Color

Xxx…

Threshold on the Feed

Xxx…

Lower Threshold

Xxx…

Equal

Xxx…

Upper Threshold

Xxx…

Velocity Color Mode

Xxx…

Min

Xxx…

Max

Xxx…

Min

Xxx…

Max

Xxx…

Feed Z Level Color Mode

Xxx…

Min

Xxx…

Max

Xxx…

Min

Xxx…

Max

Xxx…

Through this panel and related sheets, it is possible to set the visibility of buttons in the top toolbar.

Through this sheet, it is possible to show and define the top toolbar macro button's actions.

Through this panel, it is possible to set the visibility of some button in the left toolbar, also know as Machine Toolbar.

Show Jog Controls Visible

Defines the visibility of the left toolbar Show Jog Controls button.

When the button is not visible the Jog Controls panel can be yet shown/hidden pressing the F1 key or using the related main menu item.

When the UI central area view is not in Main View, showing or hiding the Jog Controls panel will automatically switch the view to Main View.

Show MDI Commands Visible

Defines the visibility of the left toolbar Show MDI Commands button.

When the button is not visible the MDI Commands panel can be yet shown/hidden pressing the F4 key or using the related main menu item.

When the UI central area view is not in Main View, showing or hiding the MDI Controls panel will automatically switch the view to Main View.

Camera Type

Defines the type of connected camera between “USB Camera” and “IP Camera”.

At the moment ONLY IP cameras are supported.

USB Camera

Sets the Vision Engine to work with a USB Camera.

IP Camera

Sets the Vision Engine to work with an IP Camera.

Host & Port

Defines the Host & Port of the IP Camera.

Username

Defines the Username necessary to connect to the IP Camera internal server.

Password

Defines the Password necessary to connect to the IP Camera internal server.

Camera Brand

Defines the brand of IP Camera from one of supported brands:

• Undefined
• Foscam
• Panasonic
• Aviosys
• Smartec
• ACTi
• ArcVision
• Axis
• DLink
• Beward
• Genius
• Planet
• Samsung
• Trendnet
• Vivotek

Video Format

The Vision Engine support the following video formats:

• MJPEG
• H264

Through this panel, it is possible to restrict write access or disable access to some settings menus by binding everything to a password.

The system allows three access levels: L1, L2, and L3.

Level 1 is linked to the operations carried out by the machine operator.
This level does not have an associated password as it is active by default when the Control Software is started.

Level 2 could be associated with the maintenance technician of the machine who periodically may need to intervene in some aspects of the same.

Level 3 is usually the level associated with the manufacturer who is the only one who can intervene on delicate parts such as axis settings, or the firmware and software update functions.

Access Levels Table

The table shows the functions of the Control Software that can be bound by an access level.

The orange DOT symbol indicates to which access level every single function is associated.

Set Master Password

In order to activate the system of access levels, the manufacturer of the machine must introduce a Master Key which is necessary so that it is possible to associate the functions to the various levels.

By default, after installation, the master access key is not set and the functions are available to anyone as the access level management is not configured.

The master key must be brought back and kept in order to be able to configure the access levels at any time.

If the master password has never been entered, a double confirmation will be requested before accepting it:

If a master password has already been entered and you want to change it, you must first enter the old password followed by the double-entry of the new one:

A new password consisting of an empty string means that you want to disable the level access system.

Password L2

Defines the password for access level L2.

The password can be numeric or alphanumeric.

The password must be different from the master password or other level passwords.

Password L3

Defines the password for access level L3.

The password can be numeric or alphanumeric.

The password must be different from the master password or other level passwords.

A practical example of a typical configuration:

Custom Alarm 01..08

Xxx…

Custom Warning 01..08

Xxx…

Custom Alarm 01..08

Xxx…

Custom Warning 01..08

Xxx…

Through this panel and related sheets, it is possible to define the custom descriptions for user inputs/outputs and analog inputs/outputs.
For the custom descriptions, only chars from the ANSI chars set are usable.

Every language supported by Control Software will have its messages so if the English language is active the showed/entered messages in the grid will be for English.
To Enter the descriptions for a different language select what in the Language panel then enter related text in the grid.
All messages are stored in the external file rosettacnc.ini, of the current machine, and they could be also edited with an external editor in the ANSI char format.

The custom descriptions will be used and shown in the Board Monitor panel reachable with the menu Setup→Board Monitor.. when the Control Software is connected with a CNC Board:

The Board Monitor is enabled to permits direct editing of the description fields in the currently active language.

This sheet permits editing of the user inputs custom descriptions.
The field Nr corresponds to the user input number (eg: 1 = user input 1).
The field Description will contain the custom description text in the currently active language.