[FR] Manual tool change

[DerAndere1]

Is your feature request related to a problem? Please describe.

Until now, manual toolchange was not possible in Marlin. The Toolchange command did not stop movement for manual tool exchange and repeated toolchanges to the same tool index were skipped.

Are you looking for hardware support?

• A toolhead that allows tools (hotends/nozzles, Laser, probe, machining tools for a spindle)
• a tool setter mounted to the frame or bed and connected to the CALIBRATION_PIN

Describe the feature you want

Support for manual toolchange. It should be possible to perform manual tool changes by initiating a tool change to any new tool with tool index i where 0 >= i < TOOLS, as well as by initiating repeated tool changes with the same tool index (e.g. repearted T1). It should be possible to initiate the tool change with G-code T or via the LCD display using MarlinUI. The machine should

1. move to a defined tool change position
2. wait for the user to acknowledge tool change is finished and continue
3. if the new tool is a hotend, heat up, purge and whipe the nozzle according to configuration
4. Move to the old position, respecting pre-configured tool length when simple tool length compensation (G43) or tool centerpoint control (G43.4) is active.
5. It should be possible to perform automatic tool length measurement with G-code G425.

Additional context

In branch Marlin2ForPipetbot, I implemented this feature.
Use these config options:

#define NOZZLE_PARK_FEATURE
#define ADVANCED_PAUSE_FEATURE
#define HOST_ACTION_COMMANDS
#define EMERGENCY_PARSER
#define MANUAL_SWITCHING_TOOLHEAD
#define TOOLS 3 // T0: Empty (Master tool), T1: Machining tools, T2: Probing tool.
#define CALIBRATION_GCODE
#define HOTEND_OFFSET_Z {0.0, -10.0, -2.0}
#define SAFE_TOOLCHANGE_START_Z 100 // A safe hight for tool change
#define MAN_ST_EEPROM_STORAGE

With these setting, G-code T1 moves up a few mm and then moves the Z axis to SAFE_TOOLCHANGE_START_Z and waits for the user to continue. The user can continue by doing one of the following things:

• Send M108
• On the LCD display in Touch mode, go out of the menus to the main status screen, observe a message that asks whether the user wants to continue and select "Continue"
• On the LCD display in Marlin mode (with MarlinUI), press the rotary encoder button or the "OK" button of the LCD display module.

At that point, if a tool index i >= HOTENDS was selected, a message "cold extrusion prevented" appears on the LCD display in touch mode. Otherwise, the hotend heats up and when the target temperature is reached, it is purged with filament. Finally, the tool moves the old position. It respects pre-configured tool length, if G43 or G43.4 are active.

---

Using the LCD display in Marlin Mode to initiate tool change:

1. User navigates back to the main status screen and touches the display for 5 seconds or presses the rotary encoder of the LCD for 5 seconds and selects Marlin mode
2. In Marlin Mode, the user navigates to the LCD menu "Tool Change" -> "Tools" and selects the tool to change to. The user can choose to change to the current tool index or any other tool index.
3. After selecting the desired tool, the machine moves up a few mm and then moves the Z axis to SAFE_TOOLCHANGE_START_Z.
4. The machine waits until the user does one of the following things:

• Sends M108,
• changes to touch mode and selects "Continue" or
• presses the button on the rotary encoder of the LCD module or the "OK" button of the LCD module.

[DerAndere1]

@printercnc this feature is ready for testing in the Marlin2ForPipetBot branch

[printercnc]

I will test the new feature in the next few days after I complete the automatic tool measurement system. As I've discussed before, the reason I developed the G38 inspection part is simply because it's easy for me to access, as I'm just a CNC CAM programming engineer. Besides automatic tool measurement, I also aim to measure deviations for future TCPC kinematics. Okay, let's test it and see what else we might need in the future.

[printercnc]

you are missing

#elif ENABLED(MANUAL_SWITCHING_TOOLHEAD) 

extern millis_t last_tool_change; 
inline millis_t ms_since_tool_change(const millis_t ms=millis()) { return ms - last_tool_change; } 
void mst_init(); 

inline FSTR_P tool_name(const uint8_t tool) { 
switch (tool) { 
case 0: return F(TOOL_NAME_0); 
case 1: return F(TOOL_NAME_1); 
#if TOOLS >= 3 
case 2: return F(TOOL_NAME_2); 
#endif 
#if TOOLS >= 4 
case 3: return F(TOOL_NAME_3); 
#endif 
default: return F("Tool"); 
} 
}

leads to error, I added the line void mst_init();

[printercnc]

Do I need to turn it on?

#define G38_PROBE_TARGET
#if ENABLED(G38_PROBE_TARGET)
  //#define G38_PROBE_AWAY        // Include G38.4 and G38.5 to probe away from target
  #define G38_MINIMUM_MOVE 0.0275 // (mm) Minimum distance that will produce a move.
#endif

The order of the test commands will be:
G28
T2 (TOOL PROBE)
G38.2 Z0
OK, replace tool T1
G425 (to find the deviation of tool T1 from reference tool T2)

I also need to clarify something.
#define TOOLS 3 // T0: Empty (Master tool), T1: Machining tools, T2: Probing tool.
Why is T2 a probing tool for finding the workpiece coordinates, and not T0 or T1? Or is it just a name definition? The execution order still follows the principle of using a probing tool to find the workpiece coordinates (x, y, z), then T1 (which could be a CNC machining tool or a 3D extruder).

[DerAndere1]

You are right, I checked the code from the MarlinFirmware/Marlin repo, pull request 23575 and the line is indeed needed. I updated my Marlin2ForPipetBot branch. We will see if my solution is good enough for your use case or whether some of your changes to G38 are needed.
Current G425 implementation assumes that tool length compensation (G43 or G43.5) is always on. It uses tool 0 as the reference tool and always sets tool length for tool 0 to 0. So you should insert non-zero length tools only with T1 (or higher tool indices) and then use G425 T1.
If you test G425 T1 for the first time, make sure you add these config option and adjust them to your needs:

#define CALIBRATION_SCRIPT_PRE  "G49\nG53\nG1X0Y0Z200A0C0\nG43" // move high above the tool setter and enable tool length compensation
#define CALIBRATION_MEASUREMENT_UNKNOWN 150 // more than longest tool

[DerAndere1]

The order of the test commands will be:

G28
T2 (TOOL PROBE)
G38.2 Z0
OK, replace tool T1
G425 (to find the deviation of tool T1 from reference tool T2)

The following sequence is less confusing for the purpose of further discussions:

G28
T2 (tool change to TOOL PROBE. after sending the command, replace tool manually so now tool 2 is mounted)
G53 (Native machine coordinate system)
G43 (tool length compensation on)
G38.2 Z0
T1 (tool change. after sending the command, replace tool manually so now tool 1 is mounted)
G425 T1 (to find tool length of tool 1) 

G425 T1 measures the tool length of tool 1 (deviation from T0). The measurement is independent of other tools, independent of G38 probing results, and independent of currently set work offsets. Because the tool setter is fixed to a position on the floor plate or frame, G425 solely relies on:

• the accuracy of the current position (i.e. the accuracy of the limit switch used for homing and the amount of backlash)
• the accuracy of the tool setter
• how well the values for CALIBRATION_OBJECT_CENTER... and CALIBRATION_OBJECT_DIMENSIONS.... match reality.

So G38.2 Z0 is not strictly needed. If you use G38.2 Z0 to probe the base plate of your machine or the bed of your printer as you proposed, It can serve as a confirmation that MANUAL_HOME_Z_POS and Z_MAX_POS, nozzle-to-probe offset and HOTEND_OFFSET_Z for the probing tool (tool 2) are set correctly.

I also need to clarify something.
#define TOOLS 3 // T0: Empty (Master tool), T1: Machining tools, T2: Probing tool.
Why is T2 a probing tool for finding the workpiece coordinates, and not T0 or T1?

T0 is for empty spindle, see https://www.linuxcnc.org/docs/html/gcode/other-code.html#sec:select-tool . In Marlin, T0 always has a hotend offset (tool length offset) of 0.
T1 for probing tool AND machining tools can work but it would make explanations more difficult.
T2 for machining and T1 for probing tool is possible, if you prefer that.

You do not need a probing tool if you do not want to use G38. But if you want to use G30 to measure the bed or G38 for measuring fixtures and your work piece, you need a probing tool with correctly set NOZZLE_TO_PROBE_OFFSET, and you need hotend offsets for the probing tool that equal NOZZLE_TO_PROBE_OFFSET values, and of course you need to enable #define G38_PROBE_TARGET.

[printercnc]

Marlin\src\module\tool_change.cpp: In function 'void mst_set_new_tool(uint8_t)':
Marlin\src\module\tool_change.cpp:405:20: error: 'class Temperature' has no member named 'temp_hotend'; did you mean 'degHotend'?
     thermalManager.temp_hotend[new_tool].reset();
                    ^~~~~~~~~~~
                    degHotend
Marlin\src\module\tool_change.cpp: At global scope:
Marlin\src\module\tool_change.cpp:418:3: error: 'PauseMessage' does not name a type
   PauseMessage mst_pause_message(const uint8_t new_tool) {
   ^~~~~~~~~~~~
Marlin\src\module\tool_change.cpp: In function 'void mst_tool_change(uint8_t)':
Marlin\src\module\tool_change.cpp:440:5: error: 'PauseMessage' was not declared in this scope
     PauseMessage pm = mst_pause_message(new_tool);
     ^~~~~~~~~~~~
Marlin\src\module\tool_change.cpp:442:9: error: 'pause_print' was not declared in this scope
     if (pause_print(0.0, motion.position, true, 0)) {
         ^~~~~~~~~~~
Marlin\src\module\tool_change.cpp:442:9: note: suggested alternative: 'isprint'
     if (pause_print(0.0, motion.position, true, 0)) {
         ^~~~~~~~~~~
         isprint
Marlin\src\module\tool_change.cpp:443:39: error: 'pm' was not declared in this scope
       wait_for_confirmation(false, 2, pm);
                                       ^~
compilation terminated due to -fmax-errors=5.
*** [.pio\build\mega2560\src\src\module\tool_change.cpp.o] Error 1

I haven't been able to verify this in practice, due to the error above. If I disable the 3D extruder configuration and leave the machine in its original CNC form, then if it's a hybrid 3D printing machine with a 3D extruder, then because I don't have a thermal sensor attached to my CNC machine, I can't access the home screen on the LCD.

[printercnc]

I've temporarily modified the tool_change file to prevent the temperature sensor check error when #define EXTRUDERS = 0.

tool_change.zip

I'm not sure if this applies to your entire system, however, when I set #define EXTRUDERS = 1, the LCD will still always warn about a faulty temperature sensor.

[printercnc]

Something still seems off, or perhaps I misunderstood the issue when checking the actual operation.

This is a model of my spindle-type machine, where milling cutter changes are entirely manual. And with most CNC router machines, the Z-home point will be Zmax, and the workpiece center point (WCS) must match the WCS point in the CAM software. It will be located anywhere, as shown in the image, and not at Z0 on the machine table like in 3D printing. Therefore, with tool_probing, the machine needs to know the WCS coordinates of the workpiece. I feel the machine doesn't know this point or needs M500 to save and understand it (I'm hesitant to use M500 because it will quickly reduce the chip's lifespan; if it doesn't save M500, it will be deleted when encountering the g28 Marlin command). Let's assume that after calling the g38.2 z0 command, then calling the g10 l20 p0 z0 command so the machine automatically recognizes this coordinate as the z0 WCS point (or the new Z0 point, which is considered the zero plane of the machine table), then when I call the g1 z0 f1000 command, the z-axis must move to this exact plane. Due to limitations in using the M500 and Marlin's automatic deletion of coordinates upon encountering the G28 command, I improved the G10, L20, and P#Z0 command libraries so that Marlin temporarily stores those coordinates in RAM during the work session (if the power is turned off, it has to re-establish the coordinates), as discussed previously (you can also modify G425 or G28 to prevent Marlin from losing this). Why did I do this, or suggest you do this? Look at my machine model: changing milling tools takes a long time, about several minutes. After this time, Marlin automatically disconnects the coordinates, leading to a loss of reference to the home point, so you have to re-home, and after re-home, all data is lost.

[printercnc]

After hours of testing the code, I think you're developing a WCS point that always lies on the printing table surface, rather than a universal case applicable to all situations. This is a bit difficult because CNC milling involves additional fixtures.

[DerAndere1]

Hi, sorry for replying with a bit of delay. The workspace offsets remained properly stored during G28, but after G28, this offset was not applied anymore. It seems to be an known issue with Marlinfirmware/Marlin: https://forum.v1e.com/t/marlin-workspaces-and-homing/35876. I added a simple fix to Marlin2ForPipetBot. I also fixed the compilation errors with EXTRUDERS 0. For the further tests I assume the config settings I explained above are set, and

• Hotend offset for tool 2 (probing tool) and NOZZLE_TO_PROBE_OFFSET are manually set correctly for your probe,
• the tool setter is mounted on the base plate / frame / rotary table at fixed native machine coordinates, e.g. X200 Y0. G425 relies on pre-compiled positions of the tool setter in native machine space (CALIBRATION_OBJECT_CENTER) and does not work if you put the tool setter anywhere else, especially not if you put the tool setter on the workpiece.
• a 20 mm x 20 mm x 20 mm workpiece is mounted at the center of the scrap plate (at native machine coordinate X0 Y0)
• Z_MAX_POS is set so that with T0 active, Z0 in native machine coordinates is at the surface of the base plate.

Here is a proper test g-code:

G90 (abosute positioning)
G53 (Select native machine coordinate system)
G43 (enable simple tool length compensation)
G10 L2 P1 X0 Y0 Z0 (set workspace offset for work coordinate system 1 to 0 
G10 L2 P2 X0 Y0 Z0 (set workspace offset for work coordinate system 2 to 0
G28 (home)
G1 X0 Y0 Z180 (move to a central position)
T0 (Initiate manual tool change to Tool 0. Toolhead moves to safe Z hight and waits for user to continue)
M108 (continue)
G1 X0 Y0 Z180 (move to a central position)
T2 (initiate tool change to probing tool. Toolhead moves to safe Z hight and waits for user to continue)
M108 (continue)
G1 X0 Y0 Z180 (move to a central position, observe tool length compensation works)
M401 (deploy probe)
G38.3 Z0 (Probe towards Z0 without sending error mesage if failed)
M114 (observe current position says something like X0 Y0 Z20. Probe reached the top of the work piece)
G10 L20 P2 Z0 (set workspace offset of coordinate system 2 so that is set so that the current position in coordinate system 2 is Z0)
G55 (Select work coordinate system 2)
M114 (observe current position says X0 Y0 Z0) 
G1 Z10 (move to Z10 in currently active work coordinate system. Observe probing tool is now 10 mm above the workpiece
M402 (stow probe)
G1 Z10 (move to Z10 in the currently active work coordinate system)
G54 (Select work coordinate system 1 which has 0 offsets so it can be used to move in native work coordinate system)
G1 X0 Y0 Z180 (move to central position)
T1 (Initiate manual tool change to Tool 1. Toolhead moves to safe Z hight and waits for user to continue)
M108 (continue)
G1 X200 Y0 Z180 (move above tool setter)
G425 T1 (calibrate tool length of tool 1)
G1 X0 Y0 Z180 (move to central position, observe tool length compensation works)
G55 (Select workspace coordinate system 2. Now you could do some machining...)
G1 X0 Y0 Z30 (Move above the work piece)
G28 (home)
G1 X0 Y0 Z30 (Observe that work offsets are properly loaded)
M400 (Finish moves)

[DerAndere1]

I updated the test g-code.

[printercnc]

Marlin\src\gcode\calibrate\G28.cpp: In static member function 'static void GcodeSuite::G28()': Marlin\src\gcode\calibrate\G28.cpp:669:10: warning: variable 'coordinate_system_refresh_needed' set but not used [-Wunused-but-set-variable] Compiling .pio\build\mega2560\src\src\gcode\config\M200-M205.cpp.o bool coordinate_system_refresh_needed = select_coordinate_system(-1); ^~~~~~~~~~~Compiling .pio\build\mega2560\src\src\gcode\config\M217.cpp.o
I re-translated the new firmware and received a warning.

[DerAndere1]

Its just a harmless warning that can be ignored. I tested all except the G425 command

[DerAndere1]

If this works for you, it would great if you can upload a Video of the test, covering the final T1 tool change and the G425. If Github does not accept videos, you can upload them as a ZIP file. That could help getting more testers on board. Best regards