The settings on this page are for firmware version 0.97. The version number can be found as the fv variable in the startup JSON message, or by typing $fv. Version 0.97 encompasses builds 412.01 - 440.xx and later.

If you have an older firmware version:

• Configuration for Firmware Version 0.96
• Configuration for Firmware Version 0.95
• Configuration for Firmware Version 0.94

Note: If you are scripting or otherwise automating settings see Scripting Settings

Connect to the TinyG USB at 115,200 baud. To see a value enter $cmd. To set a value enter $cmd=value. Most commands are self explanatory. See the sections following the cheat sheet for those that require further explanation.

All of the commands in this cheat sheet are also available using JSON, which is the preferred access method if you are writing a UI or controller. The equivalent JSON commands follow these examples:

$1ma   equivalents: {"1ma":null}  {1ma:null}   {1ma:n}    {1:{ma:null}}
$1ma=0 equivalents: {"1ma":0}     {1ma:0}                 {1:{ma:0}}

There are a few exceptions where JSON offers commands that are not available in text mode. These are noted. See also:

• JSON Operation - for basic on JSON use
• JSON Details - more information

Settings specific to a given motor. There are 4 motor groups, numbered 1,2,3,4 as labeled on the TinyG board.

Please note: In TinyG the motor travel settings are independent of each other. You don't need to put them into an equation. The board does this for you. Please see note about this in the Motor Settings section.

Settings specific to a given axis. There are 6 axis groups, X,Y,Z linear axes, and A,B,C rotary axes. Not all axes have all parameters.

There is currently only one PWM channel (p1), but the configs are structured for multiple PWM groups. The PWM channel is set up to act as a remote control Electronic Speed Controller (ESC), but can be used for other PWM functions using these settings.

The system group contains the following global machine and communication settings. The system group can be listed by requesting $sys or {"sys":""} in JSON mode

Identification Settings These are reported on the startup strings and should be included in any support discussions.

Global System Settings

Communications Settings Set communications speeds and modes.

Gcode Initialization Defaults Gcode settings loaded on power up, abort/reset and Program End (M2 or M30). Changing these does NOT change the current Gcode mode, only the initialization settings.

These $configs invoke reports and functions

    ^x | Reset tinyG | cntl+x restarts tinyG same as hardware rest button

$help | Show help screen | Show system help screen; $h also works

Note: Status report parameters is settable in JSON only - see JSON mode for details

Hidden System Settings

The following settings are accessible but do not appear in the system group listings. This is because they really should not be messed with.

Note: In TinyG the motor travel settings are independent of each other. You don't need to put them into an equation - the board does that for you. For example, if you want run motor #1 with a 200 step per revolution motor, a 3mm GT2 timing belt with a 20 tooth pulley, and 8 microsteps you simply enter:

• $1sa=1.8
• $1tr=60 (which is 3 * 20)
• $1mi=8

Axes must be input as numbers, with X=0, Y=1, Z=2, A=3, B=4 and C=5. As you might expect, mapping motor 1 to X will cause X movement to drive motor 1. The example below is a way to run a dual-Y gantry such as a 4 motor Shapeoko setup. Movement in Y will drive both motor2 and motor4.

 $1ma=0    Maps motor 1 to the X axis
 $2ma=1    Maps motor 2 to the Y axis
 $3ma=2    Maps motor 3 to the Z axis
 $4ma=1    Maps motor 4 to the Y axis

This is a decimal number which is often 1.8 degrees per step, but should reflect the motor in use. You might also find 0.9, 3.6, 7.5 or other values. You can usually read this off the motor label. If a motor is indicated in steps per revolution just divide 360 by that number. A 200 step-per-rev motor is 1.8 degrees, a 400 step-per-rev motor has 0.9 degrees per step.

 $1sa=1.8This is a typical value for many motors

TR needs to be set to the distance the mapped axis will move for one revolution of the motor. - e.g. if motor 1 is mapped to the X axis, then $1tr applies to the Xaxis. If the machine is in mm mode (G21) the TR value for XYZ axes should be entered in mm. If in inches mode (G20) XYZ should be entered in inches. ABC axes are always entered in degrees. See examples below.

For XYZ the travel-per-revolution value is usually the result of the lead screw pitch or pulley circumference.

• A 10 thread-per-inch (TPI) leadscrew moves 0.100" per revolution. TR in inches would be 0.100, or 2.54 in mm mode.
• A 0.500" radius pulley will travel 3.14159" per revolution, absent any other gearing. A typical value for a Shapeoko or Reprap belt driven machine is on the order of 36.540 mm per revolution. Don't take this as exact - you will need to do your own calibration on your machine to get this setting exact.

For ABC the travel-per-revolution value is entered in degrees. This value will be 360 degrees for an axis that is not geared down - one revolution = 360 degrees. The value for a geared rotary axis is 360 divided by the gear ratio. For example, a motor-driven rotary table with 4 degrees of table movement per handle rotation has a gear ratio of 90:1. The Travel per Revolution value should be set to 4.

Note that the travel-per-revolution is independent of the radius setting in the rotary axis settings. Set TR first to reflect the gearing, then set any Radius values if that is needed.

Note that Travel per Revolution is a motor parameter, not an axis parameter as one might think. Consider the case of a dual Y gantry with lead screws of different pitch (how weird). The travel per revolution would be different for each motor.

$1tr=2.54          Sets motor 1 to a 10 TPI travel from millimeters (2.54 mm per revolution)

Note that the equation for units-per-step is:

units = travel-per-revolution / ((360/step-angle) * microsteps)

Example: 0.00078125 mm = 1.25 / ((360/1.8) * 8)

TinyG microsteps are set in firmware, not as hardware jumpers as on some other systems. The following microstep values are supported:

• 1 = no microsteps (whole steps)
• 2 = half stepping
• 4 = quarter stepping
• 8 = eighth stepping

$3mi=8        Set 1/8 microsteps for motor 3

TinyG can also drive external stepper drivers using the breakout headers. Some drivers use other values than the above, so any value is accepted. Values other than those above are warned as non-standard.

Note about Microsteps: It is a misconception that higher microstep values are better - beyond a certain point they are a detriment to performance. In a typical setup the total power delivered to the motor (and hence torque) will go down as you increase the microsteps, especially at higher speeds. Also, using microsteps to set the finest machine resolution is source of error as the shaft angle isn't necessarily going to be at the theoretical point. Don't just assume that 1/8 microstepping is the right setting for your application. Try out different settings to balance smoothness and power.

Set to one of the following:

• 0 = Normal motor polarity
• 1 = Invert motor polarity

Polarity sets which direction the motor will turn when presented with positive and negative Gcode coordinates. It's affected by how you wired the motors and by mechanical factors. Set polarity so the indicated axis travels in the correct orientation for your machine.

Travel in X and Y is dependent on the conventions for your particular machine and CAD setup. Typically X is left/right movement, and Y is towards and away from you, but people often set up the machine to agree with the visualization their CAD program provides, and can depend on where you stand when operating the machine. Typically X+ moves to the right, X- to the left, Y+ away from you, and Y- towards you. Z is by convention the cutting axis, which is the vertical axis on a typical milling machine. Z+ should move up, and Z- should move down, into the work.

$3po=0        Set polarity to normal

Power management is used to keep the steppers on when you need them and turn them off when you don't. See Power Management page.

Sets the function of the axis.

• 0 = Disable. All input to that axis will be ignored and the axis will not move.
• 1 = Standard. Linear axes move in length units. Rotary axes move in degrees.
• 2 = Inhibited. Axis values are taken into account when planning moves, but the axis will not move. Use this to perform a Z kill or to do a compute-only run.
• 3 = Radius mode. (Rotary axes only) In radius mode gcode values are interpreted as linear units; either inches or mm depending on the prevailing G20/G21 setting. The conversion of linear units to degrees is accomplished using the radius setting for that axis. See $aRA for details.

$zam=2      Inhibit the Z axis; $zam1 will restore standard operation

(aka traverse rate or seek rate). Sets the maximum velocity the axis will move during a G0 move (traverse). This is set in length units per minute for linear axes, degrees per minute for rotary axes.

Note that the max velocity is per-axis. Diagonal / multi-axis traverses will actually occur at the fastest speed the combined set of axes and the geometry will allow, and may be faster than the individual axis max velocities. For example, max velocity for X and Y are set to 1000 mm/min. For a 45 degree traverse in X and Y the toolhead would travel at 1414.21 mm/min.

$xvm=1200        sets X maximum velocity (G0) to 1200 mm/min - assuming G21 is active (i.e. the machine is in MM mode)
$zvm=30.0        sets Z to 30 inches per minute - assuming G20 is active (i.e. inches mode)
$avm=36000       sets A to 100 revolutions per minute (360 * 100)

Sets the maximum velocity the axis will move during a feed in a G1, G2, or G3 move. This works similarly to maximum velocity, but instead of actually setting the speed, it only serves to establish a "do not exceed" for Gcode F words. Put another way, the maximum feed rate setting is NOT used to set the Gcode's F value; it is only a maximum that may be used to limit the F value provided in a gcode file.

Axis feed rates should be equal to or less than the maximum velocity. See TinyG Tuning for more details.

$xfr=1000       sets X max feed rate to 1000 mm/min - assuming G21 is active (i.e. the machine is in MM mode)

Defines the maximum extent of travel in that axis. This is used during homing. See Homing for more details on how this is used.

Both values can be positive or negative, but maximum must be greater than minimum or equal to minimum. If minimum and maximum are equal the axis is treated as an infinite axis (i.e. no limits). This is useful for rotary axes - for example:

$xtn = -1
$xtm = -1
or
$xtn = 0
$xtm = 0

Sets the maximum jerk value for that axis. Jerk is settable independently for each axis to support machines with different dynamics per axis - such as Shapeoko with belts for X and Y, screws for Z, Probotix with 5 pitch X and Y screws and 12 pitch Z screws, and any machine with both linear and rotary axes.

Jerk is in units per minutes^3, so the numbers are quite large (but see note below). Some common values are shown in millimeters in the examples below

$xjm=50,000,000          Set X jerk to 50 million MM per min^3. This is a good value for a moderate speed machine
$zjm=25,000,000          A reasonable setting for a slower Z axis
$xjm=5,000,000,000       X jerk for Shapeoko. Yes, that's 5 billion

The jerk term in mm is measured in mm/min^3. In inches mode it's units are inches/min^3. So the conversion from mm to inches is 1/(25.4). The same values as above are shown in inches are:

50,000,000 mm/min^3      is 1,968,504 in/min^3 2,000,000 would suffice
25,000,000 mm/min^3      is 984,251 in/min^3 1,000,000 would suffice
5,000,000,000 mm/min^3   is 196,850,400 in/min^3 200,000,000 would suffice

Note: Jerk values that are less than 1,000,000 are assumed to be multiplied by 1 million. This keeps from having to keep track of all those zeros. For example, to enter 5 billion the value '5000' can be entered.

Sets the jerk value used for homing to stop movement when switches are hit or released. You generally want this value to be larger than the $xJM value, as this determines how fast the axis will stop once it hits the switch. You generally want this as fast as you can get it without losing steps on the accelerations.

This one is somewhat complicated. Junction deviation - in combination with Junction Acceleration ($JA) from the system group - sets the velocity reduction used during cornering through the junction of two lines. The reduction is based on controlling the centripetal acceleration through the junction to the value set in JA with the junction deviation being the "tightness" of the controlling cornering circle. An explanation of what's happening here can be found on [Sonny Jeon's blog: Improving grbl cornering algorithm] (http://onehossshay.wordpress.com/2011/09/24/improving_grbl_cornering_algorithm/ onehossshay.wordpress.com/2011/09/24/improving_grbl_cornering_algorithm/).

It's important to realize that the tool head does not actually follow the controlling circle - the circle is just used to set the speed of the tool through the defined path. In other words, the tool does go through the sharp corner, just not as fast. This is a Gcode G61 - Exact Path Mode operation, not a Gcode G64 - Continuous Path Mode (aka corner rounding, or splining) operation.

While JA is set globally and applies to all axes, JD is set per axis and can vary depending on the characteristics of the axis. An axis that moves more slowly should have a JD that is less than an axis that can move more quickly, as the larger the JD the faster the machine will move through the junction (i.e. a bigger controlling circle). The following example has some representative values for a Probotix Fireball V90 machine. The V90 has 5 TPI X and Y screws, and 12 TPI Z. All values in MM.

 $xJD 0.05     Units are mm
 $yJD 0.05
 $zJD 0.02     Setting Z to a smaller value means that moves with a change in the Z component will move proportionately slower depending on the contribution in Z.
 $JA 200,000   Units are mm/min^2. As before, commas are ignored and are provided only for clarity

The radius value is used by rotational axes only (A, B and C) to convert linear units to degrees when in radius mode.

For example; if the A radius is set to 10 mm it means that a value of 62.8318531 mm will make the A axis travel one full revolution - as 62.383... is the circumference of the circle of radius R ( 2PIR, or 10 * 2 * 3.14159...) (Assuming $nTR = 360 -- see note below). Receiving the gcode block G0 A62.83 will turn the A axis one full revolution (360 degrees) from a starting position of 0. All internal computations and settings are still in degrees - it's just that gcode units received for the axis are converted to degrees using the specified radius.

Note that the Travel per Revolution value ($1TR) is used but unaffected in radius mode. The degrees per revolution still applies, it's just that the degrees were computed based on the radius and the Gcode axis values. See Travel per Revolution (See $1TR) in the motor group.

Please see TinyG Homing for details and more help on homing settings:

• $xSN - Minimum switch mode
• $xSX - Maximum switch mode
• $xSV - Homing Search Velocity
• $xLV - Homing Latch Velocity
• $xLB - Homing Latch Backoff
• $xZB - Homing Zero Backoff

By way of example, my Shapeoko is set up this way:

Read-only value. Example $fb=345.06
Indicates the build of firmware and changes frequently. Please provide this number in any communication about an issue.

Read-only value. Example $fv=0.97
Indicates the major version of the firmware; changes infrequently. Generally all settings, behaviors and other system functions will remain the same within a version - that's why this page is useful for all 0.97 versions.

Read-only value. Returns:

• 1 = TinyG Xmega series
• 2 for Arduino Due G2 (ARM)
• 3 for TinyG v9 G2 (ARM)

Read-write value. Used to set behaviors inside the firmware. Defaults to 8 for v8. If you have a TinyG v6 or earlier you must set this value to 6.

Read-only value.

###Global System Settings

In conjunction with the global $jd setting sets the cornering speed. See $jd for explanation

$ja=50000   - 50,000 mm/min^2 - a reasonable value for a modest performance machine
$ja=200000  - 200,000 mm/min^2 - a reasonable value for a higher performance machine

Arcs are generated as sets of very short straight lines that approximate a curve. Each line is a "chord" that spans the endpoints of that segment of the arc. Chordal tolerance sets the maximum allowable deviation between the true arc and straight line that approximates it - which will be the value of the deviation in the middle of the line / arc.

Setting chordal tolerance high will make curves "rougher", but they can execute faster. Setting them smaller will make for smoother arcs that may take longer to execute. The lower-limit of $ct is set by the minimum arc segment length, which really should not be changed (See hidden parameters).

$ct=0.01   - Normally a good value (in mm)

Sets the type of switch used for homing and/or limits. All switches must be of the same type (mixes are not supported).

$st=0   - Normally Open switches (NO)
$st=1   - Normally Closed switches (NC)

Note that probing cycles (G38.2) will work regardless of the switch setting. Probing (currently) assumes a normally open switch in the Z minimum position. During the probe cycle switches are set to NO (and ignored). They are restored to their actual $st setting when probing is complete.

Sets the number of seconds motors will remain powered after the last 'event'. E.g. set to 60 to keep motors powered for 1 minute after a move completes. Only applies to motors with power management modes that actually time out the motors (modes 2 and 3). See also $ME and $MD commands, further down this page.

$mt=5        - Keep motors energized for 5 seconds after last movement command
$mt=1000000  - Keep motors energized for 1 million seconds after last movement command (11.57 days)

See also Power Management

This sets the startup mode. JSON mode can be invoked at any time by sending a line starting with an open curly '{'. JSON mode is exited any time by sending a line starting with '$', '?' or 'h'

$ej=0      - Disable JSON mode on power-up and reset
$ej=1      - Enable JSON mode on power-up and reset

Note: The two startup lines on reset will always be in JSON format regardless of setting in order to allow UIs to sync with an unknown board.

Note: Disabling JSON mode using JSON {ej:0} will return a response in text mode (typically stat:N. Since you just disabled JSON mode your response will be in text mode. Parsers beware.

Sets how much information is returned in JSON mode. If you are using JSON mode with high-speed files (many short lines at high feed rates) you probably do not full verbose mode (5).

$jv=0 - Silent   - No response is provided for any command
$jv=1 - Footer   - Returns footer only - no command echo, gcode or messages
$jv=2 - Messages - Returns footers, exception messages and gcode comment messages
$jv=3 - Configs  - Returns footer, messages, config commands
$jv=4 - Linenum  - Returns footer, messages, config commands, and gcode line #s
$jv=5 - Verbose  - Returns footer, messages, config commands, and gcode blocks

Note that if you set verbosity to 0 using JSON mode you will not get a response, as that's what you just told it to do (i.e. not respond). {jv:0} or {"jv":0} will not return a response. Parsers beware.

Sets relaxed or strict syntax for JSON messages. See JSON Syntax for details.

Sets how much information is returned in text mode. We recommend using Verbose, except for very special cases.

$tv=0      - Silent - no response is provided
$tv=1      - Verbose - returns OK and error responses

Queue reports return the number of available buffers in the planner queue. The planner queue has 28 buffers and therefore can have as many as 28 Gcode blocks queued for execution. An empty queue will report 28 available buffers. A full one will report 0.

Using the planner queue depth as a way to manage flow control when sending a Gcode file is actually a much better way than managing the serial input buffer. If you keep the planner full to about 2 blocks available it will run really smoothly. You also want to make sure the queue doesn't starve, say - more than 20 blocks available.

Verbosity settings are:

$qv=0      - Silent - queue reports are off
$qv=1      - Single - returns reports when depth changes and is above hi water mark or below low water mark
$qv=2      - Triple - returns queue reports for every block queued to the planner buffer

You can also get a manual queue report by sending $qr

Note: In general you don't want to fill up the buffer with more than 24 commands as some Gcode blocks can occupy multiple planner buffer slots (4 are allowed).

Please see Status Reports for a discussion of $sv and $si status report settings.

$sv=0      - Silent   - status reports are off
$sv=1      - Filtered - returns only changed values in status reports
$sv=2      - Verbose  - returns all values in status reports

The minimum is 100 ms. Trying to set a value below the minimum will set the minimum value.

$si=250    - Status interval in milliseconds

Note: IC was removed in 0.97. Lines may be terminated with any combination of , , <CR, <LF. It doesn't matter anymore.

If this setting is OFF returned lines have a single . If on they are terminated with (2 characters).

$ec=0      - off
$ec=1      - on

This should be disabled for JSON mode. In text mode it's optional either way.

$ee=0      - Disable character echo
$ee=1      - Enable character echo

$ex=0      - Disable flow control
$ex=1      - Enable XON/XOFF flow control protocol
$ex=2      - Enable RTS/CTS flow control protocol

The default baud rate for the USB port is 115,200 baud. The following additional baud rates may be set. The sequence for changing the baud rate is: (1) Issue the $baud command, (2) wait for a response verifying the command, (3) change to the new baud rate.

$baud=0     - Illegal baud rate setting. Returns an error
$baud=1     - 9600
$baud=2     - 19200
$baud=3     - 38400
$baud=4     - 57600
$baud=5     - 115200
$baud=6     - 230400

These parameters set the values for the Gcode model on power-up or reset. They do not affect the current gcode dynamic model.

For example, entering $gun=0 will cause the system to start up from reset or power up in inches mode, but will not change the system to inches mode when it is entered. A G20 or G21 received in the Gcode stream will change the units to inches or MM mode, respectively. On reset or restart they will change back to the $gun setting.

These parameters are reported as part of the "sys" group.

$gpl=0      - G17 (XY plane)
$gpl=1      - G18 (XZ plane)
$gpl=2      - G19 (YZ plane)

$gun=0      - G20 (inches)
$gun=1      - G21 (millimeters)

$gco=1      - G54 (coordinate system 1)
$gco=2      - G55 (coordinate system 2)
$gco=3      - G56 (coordinate system 3)
$gco=4      - G57 (coordinate system 4)
$gco=5      - G58 (coordinate system 5)
$gco=6      - G59 (coordinate system 6)

$gpa=0      - G61 (exact path mode)
$gpa=1      - G61.1 (exact stop mode)
$gpa=2      - G64 (continuous mode)

$gdi=0      - G90 (absolute mode)
$gdi=1      - G91 (incremental mode)

Coordinate system offsets are the values used by G54, G55, G56, G57, G58 and G59 commands to define the offsets from the machine (absolute) coordinate system for X,Y,Z,A,B and C. G54-G59 correspond to the Gcode coordinate systems 1-6, respectively.

By convention G54 is often set to no offsets (all zeroes) so it is the same as the machine's absolute coordinate system. This is true because the G53 command "move in absolute coordinates" is only in effect for the current Gcode block. After that the dynamic model reverts to the coordinate system previously in effect. So if you want to say in absolute coordinates you need a persistent machine coordinate system, by convention G54.

Another convention is to set G55 to your common coordinate system, we set this to be 0,0 in the middle of the table. So once you have zeroed issuing g55 g28 will set to this system and position the head in the middle of the table. (Note: this can be done on one line of gcode - it does not need to be 2 separate commands).

G54-G59 offsets can be set per the following example:

$g54x=0         Set G54 to be the same as the machine coordinate system
$g54y=0
$g54z=0
$g54a=0
$g54b=0
$g54c=0

$g55x=90.0      Set G55 to be in the middle of the table
$g55y=90.0
$g55z=0
$g55a=0
$g55b=0
$g55c=0

In JSON mode you can set a coordinate system in a single command. Only those axes specified are changed.

{"g55"":{"x":90,"y":90,"z":"0"}}

Offsets can be displayed individually

$g54x - returns a single value

...or as a group: $g54 - returns all 6 values in the G54 group $g92 - returns all 6 values of the origin offset group

...or all together: $o - returns all offsets in the system (not available in JSON)

Note: the G54-G59 settings are persistent settings that are preserved between resets (i.e. in EEPROM), unlike the G92 origin offset settings and the G28 and G30 "go home" settings which are just in the volatile Gcode model and are thus not preserved.

Gcode provides the G10 L2 command to perform this same coordinate system offset setting function. Coordinate offsets can be set from Gcode using the G10 command, e.g. G10 P2 L2 X20.000 - the P word is the coordinate system numbered 1-6, the L word =2 is according to standard, but is ignored by TinyG (for now)

TinyG does not persist G10 settings, however. This is not in accordance with the Gcode spec. Any G10 settings that are provided will be used until reset, power cycle, or they are overwritten by a $g5xx command or another G10 command.

These commands cause various actions, and are not technically "settings".

Returns a status report or set the contents of a status report (JSON only). Identical to ? command. See Status Reports for details.

Manually request a queue report. See $QV for details.

Removes all Gcode blocks remaining in the planner queue. This is useful to clear the buffer after a feedhold to create homing, jogging, probes and other cycles.

Unpower all motors. See Power Management

Energizes all non-disabled motors. Motors will time out according to their power management a mode and timeout value. See Power Management

Execute $test to get a listing of available tests. Run $test=N, where N is the test number.

TinyG comes with a set of defaults pre-programmed to a specific machine profile. The default profile is set for a relatively slow screw machine such as the Zen Toolworks 7x12. Other default profiles are settable at compile time by including the right settings_XXXXXX.h file. If you are having trouble with your settings and want to revert to the default settings enter: $defa=1

WARNING This will revert all settings to defaults. Do a screencap of the $$ dump if you want to refer back to the current settings

These parameters are not part of any group and generally should not be changed. Serious malfunction can occur if these are not set correctly

Don't change this unless you are seriously tweaking TinyG for your application. It can cause many things to break. This value does not appear in system group listings ($sys)

$ml=0.08    - Do not change this value

Don't change this unless you are seriously tweaking TinyG for your application. It can cause many things to break. This value does not appear in system group listings ($sys)

$ma=0.10    - Do not change this value

Don't change this unless you are seriously tweaking TinyG for your application. It can cause many things to break. This value does not appear in system group listings ($sys)

$ms=5000  - Do not change this value