Millennium Machines GCode Flavour
Warning
This document is a work in progress, and will lag behind changes made in MillenniumOS itself. To understand the latest available macros and how these should be called when using them directly, please refer to the code in the GitHub Repository.
Misc
G27 - PARK
G27 [Zn]
Used to park the spindle in a safe location, by default it will move the spindle to the top of the Z axis, trigger an M5.9 (stop spindle and wait for spin-down), and then move the table to the centre of the X axis and at the front (towards the operator) of the Y axis.
If called with the Z1 argument, it will only raise and stop the spindle - the table location will not be changed.
Parking is used widely throughout probing and tool changing to move the spindle to a known starting location which is safe for lateral moves. CNC Firmwares do not always provide a generic park function (including RRF), because this can be machine-specific, so we implement our own.
G37 - PROBE TOOL LENGTH
G37
When using multiple milling tools, we must compensate for length differences between the tools. G37 can be used to (re-)calculate the length of the current tool in relation to a reference surface or the previous tool.
G37 is used widely by CNC mills to probe tool lengths but is not implemented by RRF, so again we implement our own.
M3000 - PROMPT OPERATOR WITH CONFIRMABLE DIALOG
M3000 R"Title" S"Message"
Takes both R (title) and S (message) string parameters, and will display an RRF dialog box. If the machine is currently processing a file and not paused, the dialog box will contain Continue, Pause and Cancel options. If M3000 is called while the machine is not processing a file, only Continue and Cancel options will be shown. This can be used by post-processors to display messages to the operator.
M6515 - CHECK CO-ORDINATES ARE WITHIN MACHINE LIMITS
M6515 [Xnnn] [Ynnn] [Znnn]
Takes at least one of X, Y and Z co-ordinates and checks that they are within the axes limits of the machine, otherwise triggers an abort. This is used by other macros to make sure we do not try to move outside of machine limits.
G6550 - PROTECTED MOVE
G6550 [Innn|Inull] [Xnnn] [Ynnn] [Znnn]
Takes at least one of X, Y and Z co-ordinates as the target location, and an optional probe ID (I). If the probe ID is given, it will attempt to move to the target location while watching the specified probe for activation due to collision. If a probe ID is not given, this move acts like a G1 move to the target, implementing an unprotected move at the manual probing speed. This macro is called by probing macros to try to avoid damaging any probe due to accidental collisions.
G8000 - RUN CONFIGURATION WIZARD
G8000
Triggered when installing MillenniumOS for the first time, and can be called later to reconfigure MillenniumOS. Runs through a modal-driven configuration wizard prompting the user for all of the settings required to run MillenniumOS properly.
M8001 - CHECK PROBE STATUS CHANGE
M8001 [Dnnn] [Wnnn]
Iterates through all configured probes every D milliseconds (default 100) checking to see if their values have changed. This can be used to identify the right probe via user input when configuring MillenniumOS. Will wait for a maximum of W seconds (default 30).
Probing
META
G6600 - PROBE WORKPIECE
G6600 [Wnn]
Called by the post-processor to indicate that workpiece should be probed to set WCS origin, if the W parameter is set then this will be the WCS offset that will be zeroed, rather than asking the operator.
If the post knows what type of workpiece probe should be executed, it can call the specific probing operation directly (e.g. G6500, G6501 etc) and then set the WCS using G10. Calling G6600 will prompt the operator to select a probing methodology based on their knowledge of the work piece.
Two Axis
G6500 - BORE
G6500 [Wnn]
Guided bore probe, prompts the user for approximate diameter, overtravel, approximate center position and probe depth.
Executes G6500.1 with the relevant parameters to run the actual probe.
If the W parameter is set then this will be the WCS offset that will be zeroed. If no parameter is set then no WCS will be zeroed.
G6500.1 - BORE - EXECUTE
G6500.1 [Wnn] Jnnn Knnn Lnnn Hnnn [Onnn] [R0]
Calculates the center of a bore and its radius, by running 3 probes outwards from the chosen starting position towards the edge of the bore. The overtravel is added to the radius of the bore and this sets the distance moved from the center point in each of the 3 directions before the probe cycle will error if it does not trigger.
Parameters J, K and L represent the starting point of the probe in X, Y and Z axes. H specifies the approximate diameter of the bore, O specifies the overtravel distance and when specified, R0 suppresses reporting of the probe results.
W represents the WCS offset to set the origin on, if passed.
G6501 - BOSS
G6501 [Wnn]
Guided boss probe, prompts the user for approximate diameter, clearance, overtravel, approximate center position and probe depth.
Executes G6501.1 with the relevant parameters to run the actual probe.
If the W parameter is set then this will be the WCS offset that will be zeroed. If no parameter is set then no WCS will be zeroed.
G6501.1 - BOSS - EXECUTE
G6501.1 [Wnn] Jnnn Knnn Lnnn Hnnn [Tnnn] [Onnn] [R0]
Calculates the center of a boss and its' radius, by running 3 probes inwards towards the operator-chosen center of the bore. The overtravel is subtracted from the radius of the boss to identify the target location of each probe, and the clearance is added to the radius of the boss to identify the starting locations.
Parameters J, K and L represent the starting point of the probe in X, Y and Z axes. H specifies the approximate diameter of the bore, O specifies the overtravel distance, T the clearance distance, and when specified, R0 suppresses reporting of the probe results.
W represents the WCS offset to set the origin on, if passed.
G6502 - RECTANGLE POCKET
G6502 [Wnn]
Guided rectangle pocket probe, prompts the user for an approximate width (X), length (Y), overtravel and clearance, an approximate center position and probe depth. Executes G6502.1 with the relevant parameters to run the actual probe.
If the W parameter is set then this will be the WCS offset that will be zeroed. If no parameter is set then no WCS will be zeroed.
G6502.1 - RECTANGLE POCKET - EXECUTE
G6502.1 [Wnn] Jnnn Knnn Lnnn Hnnn Innn [Tnnn] [Onnn] [R0]
Calculates the center of a rectangle pocket, its surface angles, rotation angle (in relation to the X axis) and its dimensions based on 8 different probes. Using the provided width, height, clearance and starting location, we probe outwards from inside the expected edges of each surface by the clearance distance. We probe each surface twice to get a surface angle, and validate that the pocket itself is both rectangular and how far it is rotated from the X axis.
Parameters J, K and L represent the starting point of the probe in X, Y and Z axes. H and I specify the approximate X and Y dimensions of the pocket, O specifies the overtravel distance, T the clearance distance, and when specified, R0 suppresses reporting of the probe results.
W represents the WCS offset to set the origin on, if passed.
G6503 - RECTANGLE BLOCK
G6503 [Wnn]
Guided rectangle block probe, prompts the user for an approximate width (X), length (Y), overtravel and clearance, an approximate center position and probe depth. Executes G6503.1 with the relevant parameters to run the actual probe.
If the W parameter is set then this will be the WCS offset that will be zeroed. If no parameter is set then no WCS will be zeroed.
G6503.1 - RECTANGLE BLOCK - EXECUTE
G6503.1 [Wnn] Jnnn Knnn Lnnn Hnnn Innn [Tnnn] [Onnn] [R0]
Calculates the center of a rectangle block, its surface angles, rotation angle (in relation to the X axis) and its dimensions based on 8 different probes. Using the provided width, height, clearance and starting location, we probe inwards from the expected edges of each surface by the clearance distance. We probe each surface twice to get a surface angle, and validate that the block itself is both rectangular and how far it is rotated from the X axis.
Parameters J, K and L represent the starting point of the probe in X, Y and Z axes. H and I specify the approximate X and Y dimensions of the block, O specifies the overtravel distance, T the clearance distance, and when specified, R0 suppresses reporting of the probe results.
W represents the WCS offset to set the origin on, if passed.
G6504 - WEB X
Not implemented.
G6505 - POCKET X
Not implemented.
G6506 - WEB Y
Not implemented.
G6507 - POCKET Y
Not implemented.
G6508 - OUTSIDE CORNER
G6508 [Wnn]
Guided outside corner probe, prompts the user for an approximate width (X) and length (Y) of the 2 surfaces that make up the corner, a clearance and overtravel distance, a probing depth, a starting location and the corner that we want to probe (front left, back right etc). Executes G6508.1 with the relevant parameters to run the actual probe.
If the W parameter is set then this will be the WCS offset that will be zeroed. If no parameter is set then no WCS will be zeroed.
G6508.1 - OUTSIDE CORNER - EXECUTE
G6508.1 [Wnn] Jnnn Knnn Lnnn Nn [Qn] [Hnnn] [Innn] [Tnnn] [Onnn] [R0]
Calculates the corner position of a square corner on a workpiece in X and Y, as well as calculating the rotation angle and corner angle of the item. Using the provided width, height, clearance, overtravel and starting location, we move outwards along each surface forming the corner, probing at 2 locations on each surface to find their angles, and then calculate where these surfaces intersect at the relevant corner.
Parameters J, K and L represent the starting point of the probe in X, Y and Z axes. N indicates the corner number to probe, where the Front Left corner is 0 and the number increases anti-clockwise, with the Back Left corner at 3.
Q identifies the mode - with Q1, quick mode is enabled, and no H or I parameter needs to be passed. Only a single probe point will be taken on each surface of the corner.
With Q0 (the default), you must also pass H and I - which specify the approximate X and Y dimensions of the block in millimeters.
In both modes, you can specify O, the overtravel distance, and T, the clearance distance.
R0 suppresses reporting of the probe results, and W represents the WCS offset to set the origin on, if passed.
G6509 - INSIDE CORNER
Not implemented.
Single Axis
G6510 - SINGLE SURFACE
G6510 [Wnn]
Guided single surface probe, which prompts the user for a starting location, overtravel distance, which surface to probe, a maximum probing distance and for X and Y surfaces, a probing depth below the starting location. Can be used to probe the Z height of a workpiece, or a single surface on X or Y if the operator knows these are aligned with the machine axes. This macro only probes a single point so cannot calculate surface angles.
If the W parameter is set then this will be the WCS offset that will be zeroed. If no parameter is set then no WCS will be zeroed.
G6510.1 - SINGLE SURFACE - EXECUTE
G6510.1 [Wnn] Jnnn Knnn Lnnn Hn Innn [Onnn]
Calculates the X, Y or Z co-ordinate of a surface using the provided starting location, surface number, probing distance and depth.
Parameters J, K and L represent the starting point of the probe in X, Y and Z axes. H specifies the axis to probe on, starting at 0 for Left, 1 for Right, 2 for Front, 3 for Back, and 4 for Top. I specifies the distance to probe towards the surface, and O specifies the overtravel distance. R0 suppresses reporting of the probe results.
W represents the WCS offset to set the origin on, if passed.
G6511 - PROBE REFERENCE SURFACE
Probes the touch probe reference surface in Z, and sets the touch probe activation point. Will be called automatically when changing to the touch probe with the feature enabled.
Three Axis
G6520 - VISE CORNER
G6520 [Wnn]
Guided probing macro that combines OUTSIDE CORNER and SINGLE SURFACE (Z) macros to zero all 3 axes of a WCS in a single probing operation. This macro prompts the user for the required parameters for the OUTSIDE CORNER macro, as well as a starting location. It calls the macros in sequence, probing the Z surface first before moving outwards and probing each X and Y surface that forms the corner.
If the W parameter is set then this will be the WCS offset that will be zeroed. If no parameter is set then no WCS will be zeroed.
G6520.1 - VISE CORNER - EXECUTE
G6520.1 [Wnn] Jnnn Knnn Lnnn Nn Pnnn [Qn] [Hnnn] [Innn] [Tnnn] [Onnn] [R0]
Executes a Vise Corner probe using the parameters gathered by the operator. Runs a Z probe first, then each corner probe after and sets the WCS origin of all 3 axes at once.
Parameters J, K and L represent the starting point of the probe in X, Y and Z axes. N indicates the corner number to probe, where the Front Left corner is 0 and the number increases anti-clockwise, with the Back Left corner at 3.
P indicates the depth to probe the corner surfaces at relative to the probed top surface.
Q identifies the mode - with Q1, quick mode is enabled, and no H or I parameter needs to be passed. Only a single probe point will be taken on each surface of the corner.
With Q0 (the default), you must also pass H and I - which specify the approximate X and Y dimensions of the block in millimeters.
In both modes, you can specify O, the overtravel distance, and T, the clearance distance.
R0 suppresses reporting of the probe results, and W represents the WCS offset to set the origin on, if passed.
Base
G6512 - PROBE
G6512 Lnnn [Inn] [Xnnn] [Ynnn] [Znnn] [Jnnn] [Knnn]
G6512 is the underlying probing macro called by the higher-level probing cycle macros. It must be passed a target position in at least one axis (X, Y and Z), and a start position in at least the Z axes (L). It may also be passed a start position in X or Y axes. The unspecified axes for both start and target positions will default to the current machine co-ordinates.
If I is not specified, the macro will trigger a guided manual probing cycle similar to the RRF jogging window, but only able to move towards or away from the target position. When complete, G6512 will update the probe position in the mosPCX, mosPCY and mosPCZ global variables, adjusting for tool radius and deflection.
G6512.1 - AUTOMATED PROBE
G6512.1 Inn [Xnnn] [Ynnn] [Znnn] [Rnn]
Probe a single point using an installed and connected touch probe. Target co-ordinates are specified using X, Y and Z and R can be used to override the number of retries rather than using the default value for the probe.
Probe position will be reported in the mosPCX, mosPCY and mosPCZ global variables, with no compensation for tool radius or deflection. Probe variance will be stored in the mosPVX, mosPVY and mosPVZ variables.
Warning
DO NOT call this macro directly - use G6512.
G6512.2 - MANUAL PROBE
G6512.1 [Xnnn] [Ynnn] [Znnn]
Probe a single point using a manual jogging process. Target co-ordinates are specified using X, Y and Z.
Probe position will be reported in the mosPCX, mosPCY and mosPCZ global variables, with no compensation for tool radius or deflection. Probe variance will be zero.
Warning
DO NOT call this macro directly - use G6512.
Tool Management
M4000 - DEFINE TOOL
M4000 Pnn Rnn S"..." [Xnn] [Ynn]
We need to store additional details about tools that RRF is not currently able to accommodate natively - this includes tool radius (R) and deflection values for probes (X and Y). Tool index is set using P and description is set using S"..". M4000stores these custom values that allows us to use them, while configuring RRF with the relevant tool details usingM563`.
M4001 - FORGET TOOL
M4001 Pnn
Remove the tool at index Pnn.
T<N> - EXECUTE TOOL CHANGE
Tnn
This macro is built in to RRF, using the t{free,pre,post}.g files. If the target tool number is specified, then these files are executed in order. The operator is prompted to change to the correct tool and if this tool is a probe tool, will be asked to verify that the tool is connected by triggering it manually before proceeding.
Spindle Control
Spindle Start / Stop
M3.9 - START SPINDLE AND WAIT
M3.9 [Snnnnn] [Pnn] [Dnnn]
This macro calls RRF's underlying M3 command to start the spindle, but waits after starting the spindle for it to accelerate based on a previously recorded acceleration value. This value will be reduced based on the rpm-change of the spindle so if it is only accelerating to 50% of its maximum speed then M3.9 will only wait 50% of the recorded wait value.
Parameters S and P are passed to the underlying M3 command if specified, and parameter D, specified in seconds, will override the wait time that would've otherwise been calculated.
Additionally, if expert mode is disabled, then this macro will pop up an operator confirmation / warning box when the spindle is going to accelerate from 0 rpm.
M5.9 - STOP SPINDLE AND WAIT
M5.9 [Dnnn]
Like the M3.9 macro above, this macro calls the underlying M5 macro and if any spindles were activated, waits for them to stop. As above, the deceleration value will be reduced based on the rpm-change of the spindle. Specifying the D parameter will override the delay time.
Variable Spindle Speed Control
Variable Spindle Speed Control (VSSC) constantly adjusts the speed of the spindle up and down over a set range to avoid resonance between the tool and the workpiece building up at constant RPMs. It can provide a quality boost in situations where resonances would otherwise occur.
M7000 - ENABLE VSSC
M7000 Pnn Vnn
Enable Variable Spindle Speed Control. The P and V parameters must be specified, and these control the period (in milliseconds) and variance (in RPM) of the VSSC function.
M7001 - DISABLE VSSC
M7001
Disable Variable Spindle Speed Control
Debugging
M7600 - OUTPUT ALL KNOWN VARIABLES
M7600 [D1]
Sometimes it is necessary to debug MillenniumOS or RRF, and this macro allows outputting the macro variables that MillenniumOS uses in a manner that can be attached to tickets or discord messages to aid debugging. Call it with the D1 parameter to enable additional RRF object model output that can help to debug the odder issues.