GCode Sender

WARNING: This feature is in development. It is not ready for production. Test it with the spindle off and the tool away from the work.

Not available in this version: the plugin does not open. Its menu entry shows the message Cancelled. This tool is not ready yet. The sections below describe the tool as it works when it is enabled.

The GCode Sender connects to a GRBL 1.1 controller over a serial port. It streams a CNCJob G-code to the controller. It also jogs the axes, sets the work zero, controls the spindle and the feed, probes the surface, and can level the G-code with a height map. A virtual controller runs a job on screen, and the Plot 3D tab shows the toolpath. The same tool also controls an E-Cut USB motion board. See E-Cut.

Where to find it

• Menu: Plugins menu, entry GCode sender. There is no keyboard shortcut.
• The tool opens in the Plugin tab. The tab has three sub-tabs: Connect, Control and Sender. The Control and Sender sub-tabs are enabled only when a controller is connected.
• The GRBL console is a dock. Show it with the Show console check box.

Screenshot placeholder: images/GCode-Sender-1.png - the GCode Sender tab with the three sub-tabs, the Source Object and the Job group.

Quick start

1. Create a CNCJob object. Select it in Source Object.
2. Open the Connect sub-tab. Select the port in COM list. Select the baud rate in Baud rates. The default is 115200.
3. Click Disconnected. The button turns green and shows Connected when GRBL answers.
4. Open the Control sub-tab. Click Zero Axes for the position where the work starts.
5. Use the jog arrows to check the movement. Start with a small Step.
6. Open the Sender sub-tab. Check the status with Get Report if needed.
7. Click Check mode in the Job group if you want GRBL to read the program without motion.
8. Click Start. The tool streams the CNCJob. Use Hold, Resume or Stop when needed.

Screenshot placeholder: images/GCode-Sender-2.png - the Connect sub-tab with the COM list, the baud rate list and the connect button.

Screenshot placeholder: images/GCode-Sender-3.png - the Control sub-tab with the jog arrows, the Zero Axes group and the Pause/Resume button.

Parameters

Header

Parameter	Description	Default
Source Object	The CNCJob object to send.	Active CNCJob, if any
Fit View	Fits the bounds of the G-code in the isometric view after the source object is loaded.	Checked
Show console	Shows or hides the GCode Console dock.	Unchecked
Beginner / Advanced button	Beginner hides many parameters. Advanced shows all parameters.	From global_app_level (Beginner)
Reset Tool	Resets the parameters of the tool.	-

Connect sub-tab

Parameter	Description	Default
COM list	The serial ports found. The E-Cut board appears as SH-9001 E-Cut USB when it is connected.	First port found
Search	Searches again for serial ports.	-
Baud rates	The baud rates in the list. The list has 9600 to 2000000.	115200
New	A custom baud rate. Range 40 to 9999999.	-
Add	Adds the custom baud rate to the list.	-
Delete selected baudrate	Removes the selected baud rate from the list.	-
Reset	Software reset of the controller. Enabled only when connected.	Disabled
Disconnected / Connected	Connects to the selected port, or disconnects when the port is open.	Disconnected

Control sub-tab

Parameter	Description	Default
Jog arrows (X+, X-, Y+, Y-, Z+, Z-)	Moves the axis by Step in the arrow direction, at the Feedrate. A press and hold moves continuously when Continuous is checked.	-
Origin (jog)	Raises Z to the safe Z (tools_grbl_travelz), then moves to X0 Y0.	15.0
Step	The distance of one jog move.	5
Feedrate	The feedrate of a jog move.	1500
Continuous	Hold a jog arrow to move. Release the arrow to stop. Shown only when the controller supports it.	Unchecked, hidden
Pause/Resume	Toggles feed hold (!) and cycle start (~). Blocked while a recovery is needed.	Off
Zero Axes: X, Y, Z, All	Sets the current position as zero of the active work coordinate system (G10 L20). All sets X, Y and Z.	-
Homing button	Sends $H (home cycle). If a reset is pending, the tool asks for a reset first.	-
E-Cut settings	Opens the E-Cut machine settings. Shown only with the E-Cut board.	Hidden

Sender sub-tab

Parameter	Description	Default
Send Command and Send	Sends one line to GRBL, for example $$. The answer goes to the console. Press Enter in the field to send.	-
Get Config parameter and Get	Reads one GRBL setting ($n) and shows the value.	-
Get Report	Prints the GRBL status report in the console.	-
Probe	Probes the points in the Probe Points Table and builds the height map.	-
Stop (probing)	Stops the running operation. GRBL goes into feed hold. Recovery is needed (see Advanced).	-
Save icon	Saves the GRBL height map to a file.	-

Job group

Parameter	Description	Default
Start	Streams the G-code of the selected CNCJob to GRBL. A dialog asks to start from the Beginning or from a Line. If the Level the G-code check box is on and a height map exists, a dialog asks: Generate New, Use Existing or Cancel.	-
Hold	Feed hold (!). Resume continues the job.	-
Resume	Cycle start (~). Blocked while a recovery is needed or a previous job was abandoned.	-
Stop	Stops the job: feed hold, then a soft reset. Recovery is needed.	-
Unlock	Sends $X to clear the alarm lock.	-
Sim	Opens the simulation dialog with a virtual controller. No serial port is used.	-
Check mode	GRBL reads the G-code of the next Start without motion. It is valid for one job.	Unchecked
Spindle	Toggle. ON sends M3 S<RPM>. OFF sends M5. The button shows the state that the controller reports.	Off
RPM	The spindle speed for Spindle. Range 0 to 100000.	10000
Progress bar	Shows the progress of the job, in percent.	0
Status label	Shows the state, for example Idle.	Idle
Overrides: Feed	Feed override: -10, -1, 100 %, +1, +10.	100 %
Overrides: Rapid	Rapid override: 25 %, 50 %, 100 %.	100 %
Overrides: Spindle	Spindle override: -10, -1, 100 %, +1, +10.	100 %
Override values label	Shows the current values, for example F: 100% R: 100% S: 100%.	-
Save levelled G-code	Saves the G-code that the sender streams, after the levelling.	-
Show in Plot 3D	Shows the toolpath, the tool and the height map in the Plot 3D tab.	-

Autolevelling group

Parameter	Description	Default
Level the G-code	Applies the height map to the G-code before streaming.	Unchecked
Probe Points Table, Show	Shows or hides the probe points table. Same as in Levelling.	Checked
Plot probing points	Draws the probe points on the canvas.	From the Preferences
Plot height map	Shows or hides the height map surface in Plot 3D. Hiding the surface does not change the levelling.	Checked
Avoid Excellon holes	When checked, the probe points avoid the holes of the selected Excellon object.	From the Preferences
Excellon Object	The Excellon object whose holes the probe points avoid. Shown when Avoid Excellon holes is checked.	First Excellon object
Avoid Step	Same as in Levelling.	0.5
Probe Tip Dia, Probe Z travel, Probe Z depth, Probe Feedrate	Same as in Levelling.	0.3, 2.0, -1.0, 120
Mode and Method	Same as in Levelling. Method is disabled in Manual mode.	Grid, Voronoi
Columns, Rows	Same as in Levelling.	4, 4
Add Probe Points	Creates the probe points in the current mode.	-
Import Height Map	Reads a height map file.	-
Precision probing (two touches)	GRBL only. Retracts after the coarse touch, then probes again at the fine feed. Only the second measurement is used.	Unchecked
Fine probe feedrate	The feedrate of the second touch, in units per minute. Shown and enabled only with Precision probing.	10.0
Precision retract	The distance above the coarse contact. It must release the probe without going over Probe Z travel. Enabled only with Precision probing.	0.5

Plot 3D and simulation

Parameter	Description	Default
Simulation: Start, Pause, Resume, Stop, Reset	Runs the program on the virtual controller. Pause and Resume toggle. Stop ends the run. Reset returns the speed to 1x.	-
Simulation: Speed slider	Sets the speed multiplier. The slider range is 0 to 100. At 0 the multiplier is 0.5x. Values 0 to 25 give 0.5x to 1x. Values 26 to 34 give 2x to 10x. Values 35 to 100 give up to 100x.	1x
Simulation: Close	Closes the simulation dialog.	-

Advanced

Console

• The Program tab shows the lines of the job. The highlighted line is the line that GRBL reads. Follow scrolls with the job.
• The Console tab shows the replies and sends commands.
• The status line shows Acknowledged line and the number of Errors on the lines.

Stop, reset and recovery

• Stop (job or probing) sends a feed hold (!). The machine then needs a reset and a home cycle before more motion.
• After Stop, Resume and the Pause/Resume toggle are blocked. A resume would continue the held motion.
• Reset sends the soft reset byte (0x18). The tool waits for the startup banner. Home is blocked until the banner is read.
• A soft reset stops the spindle. The tool shows Spindle as off.
• The tool does not trust the position after an uncertain motion. Press Reset, then Homing button.

Check mode

• Check mode uses $C. GRBL reads the next program without motion. The tool exits check mode after one job.
• Start refuses to build a levelled job in check mode when no height map exists.

Simulation

• The simulation uses a virtual GRBL. It does not open a serial port.
• With Level the G-code checked, the simulation also runs the probe moves of the height map.

Plot 3D

• The Plot 3D view shows the accepted lines of the job, the selected line and the tool position.
• It shows the height map surface when Plot height map is checked.
• The view starts in isometric view. Show in Plot 3D opens the Plot 3D tab.

Settings stored by the application

The tool stores these options in the application settings. The factory values are in defaults.py.

Option	Use	Default
tools_grbl_baudrate	Baud rate	115200
tools_grbl_jog_step	Jog step	5
tools_grbl_jog_fr	Jog feedrate	1500
tools_grbl_travelz	Safe Z for the origin jog and the probe travel	15.0
tools_grbl_console_visible	Console dock shown	False
tools_grbl_status_ms	Status poll interval, in ms	200
tools_grbl_arc_mode	How arcs are sent	split
tools_grbl_arc_segment	Arc segment size	0.5
tools_grbl_seg_len	Segment length	1.0
tools_gcode_fit_view	Fit View	True

GRBL details

• At connect, the tool reads $13 to learn the report units. Jog commands use G20 (inch) or G21 (mm) for the application units.
• Each probe move is G38.2. The probe result line [PRB:x,y,z:1] is read. A result with flag 0 means that the probe did not touch.
• Overrides use the GRBL real-time bytes (0x90 to 0x9D).

Tcl

No Tcl command was found for this tool. See Tcl Command Reference.

See also

• Levelling - the same probing without a live connection.
• E-Cut - the E-Cut USB motion board, which uses this tool's Connect and Control tabs.
• CNCJob Object - the source of the G-code.
• Preprocessors - the G-code format.
• Preferences-CNCJob and Preferences-Plugins.
• Keyboard Shortcuts and FAQ and Troubleshooting.