- edited description
BETA: Toolchange always enabled - breaks GRBL support - fixed for next version
Issue #461
new
Regardless if I only have one single tool or if I have “Tool change Z“ enabled or disabled the toolchange GCODE is always insered into my gcode.
This breaks GRBL controllers with only a single tool and manual toolchange.
This bug has benn introduced to the code in the last month.
(CODE GENERATED BY FLATCAM v8.994 - www.flatcam.org - Version Date: 2020/11/7)
(Name: clapposc-F_Cu.gbr_iso_combined_cnc)
(Type: G-code from Geometry)
(Units: MM)
(Created on Sonntag, 08 November 2020 at 17:27)
(This preprocessor is used with a motion controller loaded with GRBL firmware.)
(It is configured to be compatible with almost any version of GRBL firmware.)
(TOOL DIAMETER: 0.4982 mm)
(Feedrate_XY: 120.0 mm/min)
(Feedrate_Z: 60.0 mm/min)
(Feedrate rapids 1500.0 mm/min)
(Z_Cut: -0.0899 mm)
(DepthPerCut: 0.045 mm <=>2 passes)
(Z_Move: 2.0 mm)
(Z Start: None mm)
(Z End: 3.0 mm)
(X,Y End: None mm)
(Steps per circle: 64)
(Steps per circle: 64)
(Preprocessor Geometry: GRBL_11_no_M6) ← IT IS THE SAME WITH ALL PREPROCESSORS
(X range: 0.2836 ... 51.7164 mm)
(Y range: -35.7164 ... -0.2836 mm)
(Spindle Speed: 1000.0 RPM)
G21
G90
G17
G94
G01 F120.00
/////////////////// UNNECESSARY CODE STARTS HERE
M5
G00 Z1.0000
G00 X0.0000 Y0.0000
T1
<--- THIS BREAKS SINGLE-TOOL GRBL-MACHINES
(MSG, Change to Tool Dia = 0.4982)
M0 <--- THIS BREAKS SINGLE-TOOL GRBL-MACHINES
G00 Z1.0000
/////////////////// UNNECESSARY CODE ENDS HERE
M03 S1000.0
G4 P1.0
G01 F120.00
G00 X0.2836 Y-1.0330
(…)
Comments (15)
-
reporter
-
reporter
- edited description
-
reporter
- edited description
-
Hi,
This is not a bug but a feature introduced on purpose. Unfortunately, due of the GRBL limitations, it made FlatCAM beta GCode incompatible with GRBL controllers which is another thing.
I will try to find a way to disable this for the case of GRBL code. -
-
reporter
Thank you!
Unfortunately I’m not the Python guy, so I cannot submit a patch myself.
I’m hoping for a quick and easy fix.
-
Same problem
I will wait fix
-
-
assigned issue to
Marius Stanciu
-
assigned issue to
-
HI, I have the same problem with the latest download. It no longer works with my Workbee CNC using Duet controller. I will have to go back a version.
-
Try to use ‘Toolchange manual’ preprocesor with pause/resume and ‘(MSG…’ commands. I this case there are no any ‘T1' commands And if you have only one tool also you don’t have pause-change-resume cycles.
Works fine wih grbl1.1f.
-
-
Albeit a dated thread but connected - is there a Config setting / switch that removes the M0 or a switch to remove the tool change sequence completely ?
Alan
-
Hi,
Nothing changed from the above, I’ve put development on hold for the time being. If there were any other solutions I would have mentioned them.
BR,
Marius -
Hi Marius, good to hear from you and I hope all is well.
Reason for the post was regarding the Prefs/Geometry/Geometry Options the Tool Change and Enable Dwell tick boxes.
Tool change seems to be there in the resulting code all the time even if the boxes are not ticked.
Not a big issue in that I can edit the resulting code.
Keep safe and kind regards
Alan
-
I recently got a 3018 CNC, and FlatCAM is clearly the best software I’ve found so far, so this bug has basically made the software useless for me. Since this bug has been here for years, and development is on hold, it’s either fix it, edit every gcode file I output, or stop using FlatCAM before I really start to like it. SO… here’s a quick and dirty fix.
This is found in “camlib.py” starting on line 3155. There are a couple of options I can think of, like appending a condition to the second if statement to rule out GRBL machines, but since I’m not familiar with the code, I’m just going to comment out the gcode I don’t want.
From this:
for tool in tools: # Only if tool has points. if tool in points: # Tool change sequence (optional) if toolchange: gcode += "G00 Z%.4f\n" % toolchangez gcode += "T%d\n" % int(tool) # Indicate tool slot (for automatic tool changer) gcode += "M5\n" # Spindle Stop gcode += "M6\n" # Tool change gcode += "(MSG, Change to tool dia=%.4f)\n" % exobj.tools[tool]["C"] gcode += "M0\n" # Temporary machine stop if self.spindlespeed is not None: # Spindle start with configured speed gcode += "M03 S%d\n" % int(self.spindlespeed) else: gcode += "M03\n" # Spindle start # Drillling! for point in points[tool]: x, y = point.coords.xy gcode += t % (x[0], y[0]) gcode += down + up_to_zero + up gcode += t % (0, 0) gcode += "M05\n" # Spindle stop self.gcode = gcodeto this:
for tool in tools: # Only if tool has points. if tool in points: # Tool change sequence (optional) if toolchange: # gcode += "G00 Z%.4f\n" % toolchangez # gcode += "T%d\n" % int(tool) # Indicate tool slot (for automatic tool changer) # gcode += "M5\n" # Spindle Stop # gcode += "M6\n" # Tool change # gcode += "(MSG, Change to tool dia=%.4f)\n" % exobj.tools[tool]["C"] # gcode += "M0\n" # Temporary machine stop if self.spindlespeed is not None: # Spindle start with configured speed gcode += "M03 S%d\n" % int(self.spindlespeed) else: gcode += "M03\n" # Spindle start # Drillling! for point in points[tool]: x, y = point.coords.xy gcode += t % (x[0], y[0]) gcode += down + up_to_zero + up gcode += t % (0, 0) gcode += "M05\n" # Spindle stop self.gcode = gcode
I’m not home at the moment, so I haven’t had a chance to try it out, but I’m quite confident it will work, because it prevents the program from EVER adding these lines to the gcode, so if you don’t use GRBL or have multiple machines, take appropriate measures to make sure you don’t break a feature you sometimes find useful.
- Log in to comment
