#1 – cheton 于 2017-01-14

#### Tool Change in bCNC
https://github.com/vlachoudis/bCNC/wiki/Tool-Change

Hi @mandrav,

Do you have an example of “tool change” macro as described in bCNC’s wiki page? Thanks.

#2 – mandrav 于 2017-01-14

Hi @cheton ,

the following macro assumes that there’s a touch plate (or other means of Z-probing) at [X-300 Y-300 Z-50] in machine coordinates (G53).

here’s the program that would replace the M6 command to GRBL:

; [1]: keep a backup of current state ($G) as well as current XY
M5 ; stop spindle
G90 ; absolute coordinates
G53 G0 Z-1 ; raise the spindle up to (almost) the top of the travel
G53 G0 X-300 Y-300 ; go to tool change position
M0 ; pause the program to allow the manual tool change
G53 G0 Z-40 ; move above the touch plate
G91 G38.... ; probe command
; [2]: now calculate the offset and adjust WCS
G53 G0 Z-1 ; raise spindle up again to safe height
M0 ; optional extra pause (e.g. to remove probe wires if required)
; [3]: reset state ($G) to what was saved on [1] (also restart spindle etc)
G0 X[saved] Y[saved] ; [4]: move to XY that contained M6
... continue with program

Keep in mind that the above are NOT a macro in bCNC but instead provided by the program at runtime. The reason is, as you understand, that there’s a couple of places that need some simple calculations (as well as the saving/restoring of the current state).
The way it works is like this:

1. Zero out your workpiece (Z=0 on top of it)
2. Calibrate the tool: it’s a similar macro which just does the probing part of the above so it knows the probe offset in respect to your workpiece Z=0
3. Run the job
4. On each tool change, run the above code and at point [2] adjust the WCS Z=0 by adding to Z the difference of the current probe location (with the new tool) minus the previous tool’s probe location.
5. Continue the job

Having written all that, I understand it maybe doesn’t quite match the philosophy of your “program player” and would need quite a few modifications.
That’s why I proposed to just run a user-defined macro when M6 is encountered. It will require some knowledge about the program by the user but, at least, will allow for using M6 in your code without GRBL throwing an error that it’s not supported.
Such a user macro could look like this (for use with a touch plate that you put on your workpiece to zero it out):

M5 ; stop spindle
G53 G0 Z-1 ; raise spindle to the top
G53 G0 Xx Yy ; go where it's convenient to change the tool (machine coordinates!)
M0 ; pause for the tool change
; also put touch plate on the workpiece, on X0Y0
G0 X0 Y0 ; go to workpiece X0Y0
G0 Zprobe ; go to Z=touchplateheight+10 give room for height diff. of new tool)
G91 G38 ... ; run the probe command as you like
G10 L20 P1 Zplate... ; adjust Z=0 by adding the touch plate's height
G91 G0 Z5 ; move up
G90 ; absolute coordinates
M0 ; pause for cleanup by the user (remove touch plate, wires, etc)
M3 ; restart spindle and go on

Let me know if you think its feasible.

#3 – cheton 于 2017-01-14

Thank you for the detailed explanation. Do you see any problems for the steps below?

1. Pause sending g-code to the controller when M6 is encountered
2. Save current modal state ($G) as well as machine position
3. Run a user-defined macro for tool changing
– Grbl will enter Hold state on M0, click Play or Cycle Start button to resume
4. Restore previously saved modal state and machine position
5. Continue sending g-code

—

One more question here: Do you expect to manually choose an user-defined macro when M6 is encountered? This will display a pop-up window before Step 3.

#4 – mandrav 于 2017-01-14

Hi @cheton ,

yes, I think that would work fine
As for choosing the macro, either ask to select one from a list of macros or make it a setting (like “Tool change macro”).

Finally, it’d be nice if a message was shown so the user knows it’s time for a tool change and doesn’t wonder why the program stopped

#5 – cheton 于 2017-01-14

I raised a question in https://github.com/gnea/grbl/issues/91. Tool number is also useful for automatically choosing Tool Change macros.

#6 – mandrav 于 2017-01-14

Nice catch!

#7 – xpix 于 2017-04-07

If this implemented now and can i get a example macro for a Toolchange?

#8 – AustinSaintAubin 于 2017-04-07

It is not released yet. Still part of the #139 1.9 Release Backlog.

#9 – cheton 于 2017-05-02

v1.9.4 enables support for evaluating expression after the % symbol (similar to bCNC). You can manually replace M6 command with below expressions. A Manual Tool Change UI will be added in a later release.
“
%wait
%x0=posx,y0=posy,z0=posz ; Keep a backup of current XYZ
: : :

: : :
G0 X[x0] Y[y0] ; Move to XY that contained M6
“

#10 – mandrav 于 2017-05-03

Some great news!
Will try it out and let you know.

#11 – AustinSaintAubin 于 2017-05-05

@mandrav Please post your macro once you have had a chance to test it out. Have you had a change to test?

#12 – mandrav 于 2017-05-05

@AustinSaintAubin no, I haven’t had the time to test this yet but, according to @cheton , from what I understand you have to manually replace the M6 commands (no support for auto-replacing with macros or otherwise).

#13 – cheton 于 2017-05-05

The macro that I am going to use will be similar to bCNC’s manual tool change code. You can check out CNC.py as shown below:

https://github.com/vlachoudis/bCNC/blob/master/CNC.py#L1642

“python
#----------------------------------------------------------------------

code to change manually tool

#----------------------------------------------------------------------
def toolChange(self, tool=None):
if tool is not None:
# Force a change
self.tool = tool
self._lastTool = None

# check if it is the same tool
if self.tool is None or self.tool == self._lastTool: return []

# create the necessary code
lines = []
lines.append("$g") # remember state and populate variables
lines.append("m5") # stop spindle
lines.append("%wait")
lines.append("%x,y,_z = wx,wy,wz") # remember position
lines.append("g53 g0 z[toolchangez]")
lines.append("g53 g0 x[toolchangex] y[toolchangey]")
lines.append("%wait")

if CNC.comment:
lines.append("%%msg Tool change T%02d (%s)"%(self.tool,CNC.comment))
else:
lines.append("%%msg Tool change T%02d"%(self.tool))
lines.append("m0") # feed hold

if CNC.toolPolicy < 4: lines.append("g53 g0 x[toolprobex] y[toolprobey]") lines.append("g53 g0 z[toolprobez]") # fixed WCS lines.append("g91 [prbcmd] f[prbfeed] z[-tooldistance]") if CNC.toolPolicy==2: # Adjust the current WCS to fit to the tool # FIXME could be done dynamically in the code p = WCS.index(CNC.vars["WCS"])+1 lines.append("G10L20P%d z[toolheight]"%(p)) lines.append("%wait") elif CNC.toolPolicy==3: # Modify the tool length, update the TLO lines.append("g4 p1") # wait a sec to get the probe info lines.append("%wait") lines.append("%global TLO; TLO=prbz-toolmz") lines.append("g43.1z[TLO]") lines.append("%update TLO") lines.append("g53 g0 z[toolchangez]") lines.append("g53 g0 x[toolchangex] y[toolchangey]") if CNC.toolWaitAfterProbe: lines.append("%wait") lines.append("%msg Restart spindle") lines.append("m0") # feed hold # restore state lines.append("g90") # restore mode lines.append("g0 x[x] y[y]") # ... x,y position
lines.append("g0 z[_z]") # ... z position
lines.append("f[feed] [spindle]")# ... feed and spindle

# remember present tool
self._lastTool = self.tool
return lines
“

#14 – neilferreri 于 2017-08-03

@cheton Any updates on this?
@mandrav Do you have a macro to share?

#15 – neilferreri 于 2017-08-14

@cheton I’ve tried a macro to do a tool change and it comes close, but I always get errors. Sometimes the errors are for invalid statements, and sometimes the machine goes idle and freezes in the middle of a job. It seems that anytime I put a %wait in the gcode, it causes problems. The same simple macro worked without issue in BCNC (not using the built in tool change). I just replaced my M6 commands with:
%wait
G53 Z-15
M5
G53 X-220 Y-220

M0
G91
G38.2 F50 Z-50
G10 L20 P1 Z1.2

M0
G90

I’m not sure what else to share with you to help.
Thanks…I’d love to switch to your GUI on all of our machines.

#16 – cheton 于 2017-08-14

@neilferreri

The %wait is just a dwell command that waits for the planner queue to empty. It will be replaced with G4 P0.5 (%wait) as shown below:
https://github.com/cncjs/cncjs/blob/v1.9.7/src/app/controllers/Grbl/GrblController.js#L219-L230
“js
dataFilter: (line, context) => {
if (line === WAIT) {
const { sent, received } = this.sender.state;
log.debug(Wait for the planner queue to empty: line=${sent + 1}, sent=${sent}, received=${received});

this.sender.hold();

return G4 P0.5 (${WAIT}); // dwell
}

return this.dataFilter(line, context);
}
`

Could you try below program and check if it works for you?
`
G4 P0.5
G53 Z-15
M5
G53 X-220 Y-220

M0
G91
G38.2 F50 Z-50
G10 L20 P1 Z1.2

M0
G90
“

#17 – neilferreri 于 2017-08-15

@cheton
I’m still getting all kinds of errors. I get to the probe with no problem, the probe works fine, but it throws errors coming out of the probe. Sometimes immediately, sometimes a few lines down. Have you tried a tool change macro?

#18 – neilferreri 于 2017-08-15

@cheton After reading what you discovered in issue #186 , I reverted to 1.8.17 and the tool change macro worked with no errors.

#19 – cheton 于 2017-08-15

@neilferreri
Thank you for your findings.

#20 – neilferreri 于 2017-08-24

@cheton The find / replace macro works with the new 1.9.8 version. Seems that the issues were the same as those in issue #186. Thank you.

#21 – cheton 于 2017-08-24

@neilferreri
I’m still pushing some changes and bug fixes to 1.9.8, I will publish 1.9.8 once it’s ready.

#22 – cheton 于 2017-08-25

Release Notes of CNCjs 1.9.8
https://github.com/cncjs/cncjs/releases/tag/v1.9.8

#23 – cheton 于 2017-10-01

The preliminary support for pausing G-code execution with M0, M1, M2, M6, and M30 commands is now available in the master branch. You can run any macros or jog during a pause. I will make a thorough test in the next few days.

#24 – cheton 于 2017-10-07

#### Remaining Todo Items
* [x] Restore work position after completion
(1) Move to Z-safe height defined by user
(2) Move to the previous position along the X and Y axis
~~(3) Move to the previous position along the Z axis~~

* [x] Restore modal state after completion

Modal Group | Member Words
:—– | :—–
Coordinate System Select | G54, G55, G56, G57, G58, G59
Plane Select | G17, G18, G19
Distance Mode | G90, G91
Feed Rate Mode | G93, G94
Units Mode | G20, G21
Spindle State | M3, M4, M5
Coolant State | M7, M8, M9

* [x] Update M6 Tool Change instructions on wiki

#25 – cheton 于 2017-10-13

https://github.com/cncjs/cncjs/releases/tag/v1.9.11

CNCjs 1.9.11 is now available with M6 tool change support. You can upgrade to 1.9.11 and read the wiki page at https://github.com/cncjs/cncjs/wiki/Tool-Change to learn how to create a tool change macro.