[ron1ron]

Universal Gcode Sender (version 2.0 [nightly] / Jan 06, 2020)
Same problems on all axis !

I enter Y-50 on the command line and hit enter, works fine, I enter Y50 on the command hit enter to return to the same position i started from, it goes past and hits the limit switch or it travellers in the wrong direction with a none specified amount.

I've got this CNC 3 years ago and gave up on it about a year later because of this issue. I've read and played with everything i can think of but still have the problem.



Any help would be a appreciated as I've been trying all over Christmas to see if I can solve it.

[he1957]

Movement mode can be incremental or absolute.
Words can be modal or non-modal. Modal meaning "remembered" and applied to the next command word. Non-Model meaning they are not "remembered". The ANSI standard specifies which operations are "supposed" to be but some makers may not adopt these standards.

For some controllers, they remember what the last movement mode and/or word (and possibly direction) was so if you have not set or stated in a command line exactly what the machine control command is to do, it might be operating from previous command words. For example, if you said move -50, depending on incremental or absolute, the reference point will move either another -50 from current position (incremental) or go to the -50 (absolute) position from where zero was set.

A typical startup sequence to set a control into a "known state" might be as follows:

N10 % (SOF Header Start)
N20 (POST PROCESSOR: MACH2-3) ( SOF PostProcessorName)
N30 (X.NC) ( SOF by: HarryE)
N40 ()
N50 (SOF Machine Setup)
N60 G21 (SOF Measurement Units: MM)
N70 G00 G17 G40 G49 G80 G90 G64 (SOF CanOffsets+ConstantVelocityMode)
N80 ()

Note the G90 - set the machine to absolute positioning.

Also, if you used a G00 (Rapid move) versus a G01, the former says to move at the programmed rapid (max) move rate rather than a (possibly programmed) move at some much slower cutting rate.

[EVX]

The only idea I can come up with is that you are in G90 Absolute mode and your work offset is somewhere off the travel of the machine. When you go to return, it attempts to go past the travel to reach where it thinks it should go. Try jogging to the center of the table, maybe bring the Z down a bit and do a G10 command there to store xyz. From there, you should be able to move around and diagnose the problem more accurately.

[EVX]

G10 P1 L20 X0 Y0 Z0
Sets G54 X0 Y0 and Z exactly where you are at.
I set my tool using this command, using the probe routine and then G10 Z(block thickness).

[EVX]

http://linuxcnc.org/docs/html/gcode.html

[cyclestart]

I'm running grbl 1.1 and UGCS Classic (not platform).
When machine connects the console shows this:

>>> $G
[GC:G0 G54 G17 G21 G90 G94 M5 M9 T0 F0 S0]
ok

G54 offset is active, G90 absolute positioning is active, G21 meric is active, and feed is 0.
There are 2 sets of machine positions in the gui, If you make a G00 or G01 worry about the numbers under "Work Position".
A command like "G01 X0 F1000" at machine start-up won't move 0mm, it will move until the "Work Position" reads X0. To simply move 10mm from current position switch to G91.

[mactec54]

Universal Gcode Sender (version 2.0 [nightly] / Jan 06, 2020)
Same problems on all axis !

I enter Y-50 on the command line and hit enter, works fine, I enter Y50 on the command hit enter to return to the same position i started from, it goes past and hits the limit switch or it travellers in the wrong direction with a none specified amount.

I've got this CNC 3 years ago and gave up on it about a year later because of this issue. I've read and played with everything i can think of but still have the problem.



Any help would be a appreciated as I've been trying all over Christmas to see if I can solve it.

Then if you started at Y0 then to return from Y-50 you should of just used Y0, From Y-50 is going to go Y50 =100 so you would go 50 past the start point