No Levelled GCode file is created

[GastonGagnon]

Version 0.8.2 , Mach3 and windows 7
I created a separate probe.txt file then Loaded that file along with original GCode file but when I push Create Levelled GCode button, nothing seems to happen. At least the original GCode file is not modified and no new file is generated in the same directory.

I'm I missing something?
Thanks,¸
Gaston

[Country_Bubba]

Gaston,
Did you clear the "create probe file only" check box????

I just tried it for Mach3 with some files I had and when I clicked on "Create Levelled GCode", it popped up a dialogue box requesting a file name. Gave it one and it proceeded merrily on it way to produce the file.

[kvnrydberg]

I am having the same problem. Have tried different settings, probe files, g-code files, etc. Have tried it with the "create probe file only" boxed checked and unchecked. Neither does the probe persistence feature work in version 8.0. I'm using Mach3 on Windows 7, too.

[daedelus]

Hi both,

I released 0.8.3 today and this problem could be due to a bug I fixed with the probe log file in this version.

Try 0.8.3 and if it doesnt help please try to attach the raw probe log file to this thread and I will debug and fix it.

Thanks

[GastonGagnon]

Hi James,
I have tried released 0.8.3 and the same thing happened, no Levelled GCode created in the directory of Original GCode File.
The files are very short so I made a copy/paste of them here:

The original gcode file:

( 4 tour 0625 )
( File created: Thursday, July 17, 2014 - 04:24 PM)
( for Mach2/3 from Vectric )
( Material Size)
( X= 0.900, Y= 0.618, Z= 0.060)
()
(Toolpaths used in this file:)
(4 tour 0625)
(Tools used in this file: )
(1 = End Mill {0.0625 inch} mdf)
N100G00G20G17G90G40G49G80
N110G70G91.1
N120T1M06
N130 (End Mill {0.0625 inch} mdf)
N140G00G43Z0.3000H1
N150S10000M03
N160(Toolpath:- 4 tour 0625)
N170()
N180G94
N190X0.0000Y0.0000F40.0
N200G00X-0.4812Y-0.3092Z0.2000
N210G1Z-0.0290F20.0
N220G1Y0.3092F40.0
N230G2X-0.4500Y0.3404I0.0313J0.0000
N240G1X0.4500
N250G2X0.4812Y0.3092I0.0000J-0.0313
N260G1Y-0.3092
N270G2X0.4500Y-0.3404I-0.0313J0.0000
N280G1X-0.4500
N290G2X-0.4812Y-0.3092I0.0000J0.0313
N300G1Z-0.0580F20.0
N310G1Y0.3092F40.0
N320G2X-0.4500Y0.3404I0.0313J0.0000
N330G1X0.4500
N340G2X0.4812Y0.3092I0.0000J-0.0313
N350G1Y-0.3092
N360G2X0.4500Y-0.3404I-0.0313J0.0000
N370G1X-0.4500
N380G2X-0.4812Y-0.3092I0.0000J0.0313
N390G00Z0.2000
N400G00Z0.3000
N410G00X0.0000Y0.0000
N420M09
N430M30
%

And the probe file:


-0.48120,-0.34039,0.00000
-0.00000,-0.34039,-0.00058
0.48120,-0.34043,-0.00121
0.48120,0.34043,-0.00417
-0.00304,0.34039,-0.00458
-0.48420,0.34039,-0.00488

Tanks for you help,
Gaston

[GastonGagnon]

Sorry, I think the file you wanted is this one ALProbe4tour0625.tap

(AutoLeveller, Version: 0.8.3, http://autoleveller.co.uk)
(Copyright 2013-2014 James Hawthorne PhD)
(Original GCode file: 4 tour 0625.txt)
(Creation date: 17/07/2014 time: 18:40)

(This program and any of its output is licensed under GPLv2 and as such...)
(AutoLeveller comes with ABSOLUTELY NO WARRANTY; for details, see sections 11 and 12 of the GPLv2)

(prerequisites)
(1. need a working probe)
(2. Zero your Z axis on or just above the surface)
(Note: The first probe will touch off Z to 0.000 when it first touches to copper, )
(all other probe values are relative to this first point)

G20 (Inches)
G90 (absolute distance mode, not incremental)

(begin initial probe and set Z to 0)
G0 Z1(Move clear of the board first)
G0 X-0.4812 Y-0.3404(Move to bottom left corner)
G0 Z0.125(Quick move to probe clearance height)
G31 Z-0.0625 F5
G92 Z0
G0 Z0.125
G31 Z-0.0625 F2.5
G92 Z0
M40 (Begins a probe log file, when the window appears, enter a name for the log file such as "RawProbeLog.txt")
G0 Z0.125
G0 X-0.4812 Y-0.3404
G31 Z-0.0625 F5
G0 Z0.125
G0 X0 Y-0.3404
G31 Z-0.0625 F5
G0 Z0.125
G0 X0.4812 Y-0.3404
G31 Z-0.0625 F5
G0 Z0.125
G0 X0.4812 Y0.3404
G31 Z-0.0625 F5
G0 Z0.125
G0 X0 Y0.3404
G31 Z-0.0625 F5
G0 Z0.125
G0 X-0.4812 Y0.3404
G31 Z-0.0625 F5
G0 Z0.125
G0 X-0.4812 Y-0.3404 Z1
M41 (Closes the opened log file)

M2
%

[daedelus]

I shall look at this immediately. Thanks for the info.

[daedelus]

OK Just to keep you informed, I have found the problem and am thinking of the best way to deal with it.

First of all lets try to define names to these files to avoid confusion:

Original gcode file = The gcode file, unmodified by the Autoleveller and produced by some CAM or tool unrelated to autoleveller
Autolevelled file = The file produced by Autoleveller from the orginal gcode file which makes adjustments to the Z value(with or without using the raw probe file)
Probe File Generator (PFG) = The gcode file which produces a raw probe file (after selecting the 'probe-only' option in the Autoleveller)
Raw Probe File (RPF) = The file which contains a list of the axis values (a log, not a gcode file) produced by your controller software from the PFG

If anyone has any other suggestions for these file name definitions, please discuss.

Anyway, Back to the problem... The values for X and Y in your RPF do not match exactly with the values in the PFG. For example, the line: 'G0 X-0.4812 Y0.3404' in your PFG corresponds to '-0.48420,0.34039,-0.00488' (the first 2 values are your X and Y) in your RPF. So not exactly the same. This is a problem because Autoleveller should be generating a grid from the RPF of 2 rows by 3 columns, but because the values are different, it thinks its a different size and generates an incorrect grid (or tries and fails).

I have modified your RPF below to exactly match the values given in your PFG. If you use this instead of your previous RPF, it should work fine.

Code: Select all

-0.4812,-0.3404,0.00000 
-0.0000,-0.3404,-0.00058 
0.4812,-0.3404,-0.00121 
0.4812,0.3404,-0.00417 
-0.0000,0.3404,-0.00458 
-0.4812,0.3404,-0.00488 

I suspect your machine is slightly overshooting or undershooting slightly. Maybe you need to change some settings for your axis or maybe its some hardware issue. I am not the best person to ask, maybe others will have a better idea. All I know is this doesnt happen to me i.e. if I issue a command like 'G0 X1.5 Y1.5' the machine will go to X1.5 Y1.5 exactly everytime without fail.

Now for the software solution... My initial thoughts are that I can add a tolerance value there so that all X values in the RPF within about 100th of an inch should be seen as the same and not 2 separate values as it does now, the same for Y.

A safer option would be to feed the RPF and PFG in together to the autoleveller so that the X and Y values can be taken from the PFG and the corresponding Z values taken from the RPF.

regards,

[GastonGagnon]

Hi James,
I never noticed the difference as my DRO indicate 4 decimals only which is plenty for my machine.
The log file (RPF) gathers coordinates positions with 5 decimal numbers. Could it be possible to round these coordinates with 4 decimals instead of 5? This may solve the problem.
Is this something I can do in Mach3 settings?
Gaston

[daedelus]

Rounding to 4 decimal places would definitely help in this particular case but would it still work for larger RPF's, and for different machines? Maybe, maybe not.

In general, you could be right though and that level of precision is probably not necessary. Let me see what I can do.

P.S. I could be completely wrong, but I dont think you can change the probe file setting in Mach3 without making a mod or something. It will need to be done in Autoleveller.