Power failure and resurrection on a CNC machine

infiniteloop

@nightowl999 said in Power failure and resurrection on a CNC machine:

Yes, here it is, but I'm not sure if I've done it correctly...

Thx, and well done! From a first glance, I get the impression that this resurrect.g is missing all the things which are specific to CNC routers.

Could you please try to edit this commented version and insert comment lines with the CNC specific commands you miss? Think carefully, the sequence of commands is essential, else you can wreck your machine in the worst case.

With this "script" ready, we can see if the required additions can be called from resurrect-prologue.g or if we have to write the whole M911 stuff ourselves.

Nightowl

@infiniteloop Whew, let's see how this goes...

; File "0:/gcodes/Calibration Toolpath.gcode" resume print after power failure at 2022-05-29 16:49
G21					; sets units to mm
G92 X182.895 Y658.930 Z66.000		; sets the position for X, Y and Z
G60 S1					; I think a user-defined save slot can be 0, 3, 4 or 5 (0 is default)
? T-1 P0				; I'm not sure why the tool is deselected
Assuming this data has been saved in the state.restorePoints nodes...
T0					; select the last tool used - this should be stored in the relevant state.restorePoints[*].toolNumber
Set savedSpindleSpeed			; select the last tool's spindle speed - this should be stored in the relevant state.restorePoints[0].spindleSpeeds
M98 P"resurrect-prologue.g"		; runs the user-defined resurrect-prologue.g
; M116					; not relevant for CNC
; M290 X0.000 Y0.000 Z0.000 R0		; not relevant for CNC
; Workplace coordinates
G10 L2 P1 X147.00 Y584.00 Z67.00	; I think this is necessary 
; G10 L2 P2 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P3 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P4 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P5 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P6 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P7 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P8 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P9 X0.00 Y0.00 Z0.00		; not relevant for CNC
? G54					; select coordinate system 1
; M106 S0.50				; not relevant for my CNC
M106 P0 S0.50				; turns user-configured fan on (I've got a case fan configured)
; M116					; not relevant for CNC
; G92 E0.00000				; not relevant for CNC
; M83					; not relevant for CNC
? M486 S-1				; not relevant for CNC
? G17					; not sure if this is relevant for CNC - it's not in the config.g file
M23 "0:/gcodes/Calibration Toolpath.gcode"
M26 S249				; set file offset from the start of the interrupted file
G0 F6000 Z68.000			; rapid move to above saved Z height
G0 F6000 X182.895 Y658.930		; rapid move to saved XY axes
G0 F6000 Z66.000			; reaped move to saved Z height
? G1 F2500.0 P0				; controlled linear move relating to output pins
G21					; sets units to mm
M24					; start/resume SD print

Before the power failure happens, I know where the spindle information is held, as I use that in my pause.g (which includes a test M28/M29 script) and resume.g files. These may help, so I've added them below...

; pause.g
M28 savedCNC.g
echo "Duet and RepRap are fantastic"
M29
set global.savedSpindleSpeed = spindles[0].active ; sets the global variable
echo "Spindle speed saved at " ^ {global.savedSpindleSpeed} ^ "RPM" ; shows saved spindle speed in the Console
G1 Z{max(move.axes[2].userPosition+5,move.axes[2].max-5)} F2400 ; move the Z axis to a safe height		
G0 X273.5 Y560 ; move XY to a safe place
M5 ; turn the spindle off

; resume.g
if state.currentTool =-1
	echo "No tool active.  Selecting tool zero"
	T0 ; select tool zero
if state.currentTool >= 0
	echo "Spindle state on tool ", state.currentTool, " is ", spindles[state.currentTool].state
if {state.currentTool >= 0} & {tools[state.currentTool].spindleRpm >= 0}
	M3 S{global.savedSpindleSpeed} ; resume saved spindle speed
	G4 S1 ; wait 1 second to allow the spindle to spin up
	echo "Spindle speed resumed at " ^ {global.savedSpindleSpeed} ^ "RPM" ; this should show the setting was successful
G0 R1 X0 Y0 ; move X and Y back to saved work XY location
G1 R1 Z0 F240 ; move Z slowly down to saved work Z location

infiniteloop

@nightowl999 Some remarks to your resurrect.g:

G60 S1 - this saves the current coordinate values in the memory slot which is later referred to from M24 (resume print). For this to work, the coordinates must have been set before. That’s the G92 line, in front of G60.
M486 S-1 - the context is object cancellation, but I don’t quite understand the meaning. In my resurrect.g, the parameter was T-1, which is not documented but could have meant something like „don’t cancel objects“.
G1 F2500.0 P0 - this one sets the feed rate, but the P0 is special - from the GCode Reference: „Pnnnn (supported only in some builds of RepRapFirmware)“. I once figured out the port bits (IOBITS), but I have no guess whether P0 is used by our RRF or simply ignored.

All of the other entries have a potential meaning with 3D printers, depending on the setup, but I have not the faintest idea which entries you really need for your mill: do you heat a nozzle, use multiple coordinate systems or do you extrude something? OK, just see your latest post - I’ll go through that in a minute … [contemplating] …

infiniteloop

@nightowl999 After some contemplation, I commented your commented resurrect.g:

; File "0:/gcodes/Calibration Toolpath.gcode" resume print after power failure at 2022-05-29 16:49
G21					; sets units to mm



; >>> These two lines belong together and prepare the latter use of M24
G92 X182.895 Y658.930 Z66.000		; sets the position for X, Y and Z
G60 S1					; I think a user-defined save slot can be 0, 3, 4 or 5 (0 is default)



? T-1 P0				; I'm not sure why the tool is deselected
; >>> ALL tools are deselected or, in a sense, deactivated. I’m not sure, but I think that in CNC mode, this would prevent any motorized tool from spinning?

 Assuming this data has been saved in the state.restorePoints nodes...
 T0					; select the last tool used - this should be stored in the relevant state.restorePoints[*].toolNumber
 Set savedSpindleSpeed			; select the last tool's spindle speed - this should be stored in the relevant state.restorePoints[0].spindleSpeeds

; >>> At the time this macro is generated, these data can directly be read from the object model - in a way, you "store" them in resurrect.g for later use



M98 P"resurrect-prologue.g"		; runs the user-defined resurrect-prologue.g
; M116					; not relevant for CNC
; M290 X0.000 Y0.000 Z0.000 R0		; not relevant for CNC
; Workplace coordinates
G10 L2 P1 X147.00 Y584.00 Z67.00	; I think this is necessary 
; >>> Yes.

; G10 L2 P2 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P3 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P4 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P5 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P6 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P7 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P8 X0.00 Y0.00 Z0.00		; not relevant for CNC
; G10 L2 P9 X0.00 Y0.00 Z0.00		; not relevant for CNC

? G54					; select coordinate system 1
;  >>> Needed to activate G10 L2 P1


; M106 S0.50				; not relevant for my CNC
M106 P0 S0.50				; turns user-configured fan on (I've got a case fan configured)
 ; M116					; not relevant for CNC
 ; G92 E0.00000				; not relevant for CNC
 ; M83					; not relevant for CNC
 ? M486 S-1				; not relevant for CNC
; >>> Fine. One problem less :-)

 ? G17					; not sure if this is relevant for CNC - it's not in the config.g file
; >>> Don’t know either - do your .gcode files contain G2 oder G3 commands? I think the larger problem is to get to know the proper command in use from the object model: G17, G18 or G19


M23 "0:/gcodes/Calibration Toolpath.gcode"
M26 S249				; set file offset from the start of the interrupted file
G0 F6000 Z68.000			; rapid move to above saved Z height
G0 F6000 X182.895 Y658.930		; rapid move to saved XY axes
G0 F6000 Z66.000			; reaped move to saved Z height
; >>> Not quite: the first G0 puts Z 2 mm above the saved height (to ensure lee-room for the following X/Y move), the third G0 goes to the bone.
; >>> That's suitable for 3D Printers, don't know how to best navigate a tool on your router ..

? G1 F2500.0 P0				; controlled linear move relating to output pins
; >>> How can I translate "extrusion rate" into the CNC world? Are any "extruders" in use?

G21					; sets units to mm
M24					; start/resume SD print

Fine. That's less work than needed for a 3D Printer to recover properly.

In the next step, I have to figure out what trick you apply to manage your spindle. Was a good idea to add your pause/resume scripts to your post

Nightowl

@infiniteloop Thank you

In response to your comments, here are mine...

Line 13 - M3 would stop the spindle spinning
Line 19 - I know where they are, but at what point can the values be 'recovered' and saved
Line 52 - Not in config.g, but I CAN find G3 in the toolpath (gcode) files (e.g. "G3X31.755Y28.580I3.175J0.000" from a Vectric CAD file (these are G2 - clockwise, and G3 - counterclockwise, arc movements)
Line 60 - OK, understood
Line 61 - I think movement is controlled by G1 X*Y*X*  with speed defined with F*, e.g. G1X49.124Y56.098F3683.0
Line 64 - No, there are no extruders

infiniteloop

@nightowl999 OK, now I have edited (faked) a resurrect.g, easy to read as it is really short. I've reflected some of your comments…

; File "0:/gcodes/Calibration Toolpath.gcode" resume print after power failure at 2022-05-29 16:49


G21					; sets units to mm
G92 X182.895 Y658.930 Z66.000		; sets the position for X, Y and Z
G60 S1					; save to slot 1 for latter use of M24

T-1 P0					; this enables the macros tpreN.g and tpostN.g to be called by the following T0
T0						; change(!) to tool T0, call the corresponding macros

M3 S10000				; set spindle speed - don’t worry, we create a macro with this line like we created HelloWorld :-)

M98 P"resurrect-prologue.g"		; runs the user-defined resurrect-prologue.g

G10 L2 P1 X147.00 Y584.00 Z67.00	; restore the coordinates for coords-system #1
G54					; select coordinate system 1

G17					; or G18, G19 - needed for circular moves

M23 "0:/gcodes/Calibration Toolpath.gcode"		; select the interrupted CNC file
M26 S249				; set file offset from the start of the interrupted file
G0 F6000 Z68.000			; rapid move to above saved Z height
G0 F6000 X182.895 Y658.930		; rapid move to saved XY axes
G0 F6000 Z66.000			; rapid move to saved Z height

G21					; sets units to mm
M24					; start/resume SD print

With the G0 movements, formerly known as line 61, you misunderstand my concerns: It's not the syntax, but what path is safe for these head moves on a CNC? Are you fine with the movements as they are done in resurrect.g?

So, your homework for now: carefully check my faked resurrect.g, especially with regard to the position of the M3 command: shall the spindle start that early in the recovery process?

infiniteloop

@nightowl999 In case you can put the M3 before resurrect.g, the solution is pretty simple: Here is a macro which just stores the spindle speed in the file "RestoreSpindleSpeed.g", which in turn can be called from your resurrect-prologue.g. The only thing left to figure out is how to insert the call of "SaveSpindleSpeed.g" into the M911 command.

; SaveSpindleSpeed.g
; Macro to store the actual spindle speed (RPM) at the time this is called
; To restore the saved datum, call the macro "RestoreSpindleSpeed.g".
; Requires RRF 3.4 and a CNC configuration with valid spindles[0] entry in the object model

var fName = "RestoreSpindleSpeed.g"

echo >{var.fName} "; "^var.fName
echo >>{var.fName} "; Spindle speed saved from running """^{job.file.fileName}^""" CNC file"
echo >>{var.fName} ""
echo >>{var.fName} "M3 S"^{spindles[0].active}
echo >>{var.fName} ""
echo >>{var.fName} ";EOF"

Nightowl

@infiniteloop said in Power failure and resurrection on a CNC machine:

So, your homework for now

It's a very long time since I've had homework!

With regard to the G0 movements, I need to ask a question. If the XYZ values are saved when the power loss workflow starts (based on the M911), then these should be fine in this circumstance, but would change when overwritten by the next power loss event. Have I got that right?

It was suggested to me that the spindle should start before the axes move, as it would then cut its way through an obstruction, rather than not and end up it breaking and damaging the stock.

The most important axis save is the Z axis. With a power failure X and Y can physically stay where they are, although I appreciate their respective 3 dimensional locations must be saved as the axes must be re-homed after restarting.

Note: I get that a 3D printer should not re-lay material a second time following restart, but this is not an issue for the CNC. As the part to be cut has already been cut, it will only cut air.

infiniteloop

@nightowl999 said in Power failure and resurrection on a CNC machine:

If the XYZ values are saved when the power loss workflow starts (based on the M911), then these should be fine in this circumstance, but would change when overwritten by the next power loss event. Have I got that right?

Perfectly!

It was suggested to me that the spindle should start before the axes move

Fine, than you can try my latest macro

The most important axis save is the Z axis. With a power failure X and Y can physically stay where they are, although I appreciate their respective 3 dimensional locations must be saved as the axes must be re-homed after restarting.

Yeah, I ask because, with 3D printers, all X/Y moves above the current Z-height of the print are perfectly safe. That's what resurrect.g assumes. However, with routers, this might be different - I simply don't know that.

–––––

I have been looking in how to insert a macro call into M911 - alas, the reality check on my printer fails: although configured, M911 does not execute on a simulated power loss. Could you help me out with that?

It's simple: out-comment the M911 line in your config, then put something like this below:

M911 S13.1 R24.0 P"M98 P""SaveSpindleSpeed.g"" M913  X0 Y0  G91 M83 G1 Z3 E-5 F1000"

Parameters can be different on your milling machine (especially S and R of M911).

If you have put the "SaveSpindleSpeed.g" macro into /sys before, you should find the spindle speed at power-off in the macro "RestoreSpindleSpeed.g" after you have repowered your mill.

Nightowl

@infiniteloop

Just so I'm clear (sorry), do I need to run a project file and power off during that, or will the file be generated without running a project file?

Also, there isn't a file of that name in the \sys folder yet.

Also also I probably don't need to include anything after Y0 as I don't have an extruder (except perhaps the Z3?)

Nightowl

@infiniteloop

Talk about slow! I'm not getting topic updates, so missed the bit about writing the macro.

I've done it now and, with the spindle running, switched off the machine at the mains, then turned it back on again.

This is the resulting SavedSpindleSpeed.g file...

; SaveSpindleSpeed.g
; Macro to store the actual spindle speed (RPM) at the time this is called
; To restore the saved datum, call the macro "RestoreSpindleSpeed.g".
; Requires RRF 3.4 and a CNC configuration with valid spindles[0] entry in the object model
var fName = "RestoreSpindleSpeed.g"
echo >{var.fName} "; "^var.fName
echo >>{var.fName} "; Spindle speed saved from running """^{job.file.fileName}^""" CNC file"
echo >>{var.fName} ""
echo >>{var.fName} "M3 S"^{spindles[0].active}
echo >>{var.fName} ""
echo >>{var.fName} ";EOF"

I've also written a RestoreSindleSpeed.g file with just a REM line at Line 1, and this is what's in it when I run the SavedSpindleSpeed.g file...

; RestoreSpindleSpeed.g
; Spindle speed saved from running "null" CNC file

M3 S0

;EOF

infiniteloop

@nightowl999 said in Power failure and resurrection on a CNC machine:

I've also written a RestoreSindleSpeed.g file with just a REM line at Line 1.

Then, something goes wrong. The macro RestoreSpindleSpeed.g is generated by a call of SaveSpindleSpeed.g. So, if you have put SaveSpindleSpeed.g into the M911 line in your config,g, then cut power off …
After repowering the machine, RestoreSpindleSpeed.g should be to find in your /sys folder of the SD card. Every time you see it in /sys, you can delete it right away. It is just needed until you have run your resurrect.g - which in turn calls resurrect-prologue.g, into which you - hopefully - have insert the line

M98 P"RestoreSpindleSpeed.g"

As long as no job is in progress during the power fail, you will get "null" as CNC file name, and if the spindle speed is 0, the resulting M3 S0 is ok.

I probably don't need to include anything after Y0

That's right for your router.

Nightowl

@infiniteloop
So I tried to experiment a little...

I ran a small gcode file which set the spindle speed to 18,000rpm then initiated a power cut.

When I ran the RestoreSpindleSpeed.g from the MDI, the spindle started up - at 18,000rpm.

This is the file:

; RestoreSpindleSpeed.g
; Spindle speed saved from running "0:/gcodes/Calibration Toolpath.gcode" CNC file

M3 S18000

I've now added the M98 line to resurrect-prologue.g file, so it looks like this:

; resurrect-prologue.g
M98 "RestoreSpindleSpeed.g"

infiniteloop

@nightowl999 said in Power failure and resurrection on a CNC machine:

This is the file:

That's what I've expected. The only thing I miss is my beloved ";EOF" at the end of RestoreSpindleSpeed.g

Now the big question: does this setup what you want or do you need additional functions to be restored after a power off? With the same technique, we could generate a complete replacement or a better suited version of resurrect.g.

Nightowl

@infiniteloop

That's awesome, thank you

Because this is following a power failure, and from a safety perspective, there are some procedures I will need to initiate from starting up after the power failure (it's never my intention to be away from the machine while it's running, by the way).

I understand the machine must be homed, so it knows where it is, return to its last known XY location, remember what file it was running, remember where in that file it had got to, then wait for me to say OK for it to carry on. At the 'carry on' it should start the spindle and plunge slowly down to it's last known Z height then continue the project.

Simples!

I think the parameters for most of that will be in the resume.g file?

I've added the EOF line!

infiniteloop

@nightowl999 said in Power failure and resurrection on a CNC machine:

I think the parameters for most of that will be in the resume.g file?

That depends. Currently, your resume.g is mainly meant to be called after a pause - I doubt you want this to permanently call for permission to continue. Also, at that stage of resurrect.g, i.e. when resurrect.g calls resume.g, the spindle is already running. Nothing to dream of - you want to be asked before.

A better place to ask might be your resurrect-prologue.g. From there, you can cancel further execution of resurrect.g.

I understand the machine must be homed, so it knows where it is, return to its last known XY location, remember what file it was running, remember where in that file it had got to, then wait for me to say OK for it to carry on. At the 'carry on' it should start the spindle and plunge slowly down to it's last known Z height then continue the project.

The question here is: does resurrect.g what you want? As I said, we can insert a dialog in the prologue which then asks for permission to continue … but are you fine with the part of resurrect.g which follows on the call of the prologue?

Nightowl

@infiniteloop
So it's about the event timing (I'm not sure I actually meant the resume.g file!)...

On power fail, the M911 string initiates the SaveSpindleSpeed.g file which writes the RestoreSpindleSpeed.g file, taking (some) information from the active job file and elsewhere, and the default resurrect.g file is also written.

On power resume, the resurrect.g file calls the resurrect-prologue.g file, which calls the RestoreSpindleSpeed.g file to set the variables and other information ready for the specific file to continue.

It might be worth homing the machine on power resume and for it to wait there until I allow it to continue (if everything is OK, or Cancel if I need to stop the project.

Cancel will be the same as Cancel Job on the DWC.

On OK, the spindle should move to the last known XY, turn on at the saved Spindle speed, thendrop down to the last known Z height and continue on it's way.

So, in answer to your question, I think the resurrect.g file does do what I want, except for the homing sequence, which I think is necessary. I could be wrong, if all the necessary information is held in the resurrect.g file and precludes the need to home. That's what I'm not sure about.

Thank you!

infiniteloop

@nightowl999 said in Power failure and resurrection on a CNC machine:

On power fail, the M911 string initiates the SaveSpindleSpeed.g file which writes the RestoreSpindleSpeed.g file, taking (some) information from the active job file and elsewhere, and the default resurrect.g file is also written.

Correct.

@nightowl999 said in Power failure and resurrection on a CNC machine:

On power resume, the resurrect.g file calls the resurrect-prologue.g file, which calls the RestoreSpindleSpeed.g file …

Up to here: correct.

… to set the variables and other information ready for the specific file to continue.

No, the file RestoreSpindleSpeed.g just restores the previously saved spindle speed - that's it. After that, it returns control back to resurrect-prologue.g (which, at this point, has no more instructions available), and, after finishing execution of the prologue, control returns to resurrect.g which then executes all lines following the call of resurrect-prologue.g.

I think the resurrect.g file does do what I want, except for the homing sequence, which I think is necessary.

That's the main job of resurrect-prologue.g - allow me to cite the documentation:

At the very least, your sys/resurrect-prologue.g file must do the following:
Home the printer, without crashing the head into the print. On a delta, or on a Cartesian or CoreXY printer with a Z max homing switch, you can home all axes. On other types of printers you may have to skip homing Z and use a G92 command to tell the printer the current Z coordinate. If you choose not to home an axis, then even if the print head hasn't moved since power down, the motor positions will change by up to 4 full steps compared to their position at power down. Note: recent firmware versions write a G92 command containing the coordinates at the time of failure into resurrect.g, just before the call to resurrect-prologue.g. So you may get away without homing axes. But it is still best to home any axes that you can (typically X and Y on a cartesian or CoreXY printer).

Nightowl

@infiniteloop

I’m definitely going to try and help others with this in the future, as payback for all your help!

Although I feel like I’m wading through treacle, I’m learning as I go!

infiniteloop

@nightowl999 said in Power failure and resurrection on a CNC machine:

Although I feel like I’m wading through treacle, I’m learning as I go!

Don't worry, it's easy. Just take your commented resurrect.g and follow the lines. Near the beginning, you will come up with the line

M98 P"resurrect-prologue.g"

At that point, the control flow is handed over to the macro (which in turn can call other macros). After the macro (or chain of macros) is done, control goes back to the next line in resurrect.g. That's all - just one command after the other. Well, and some of the commands (the macros) contain their own list of commands … so what?