g54 issue

i clear it, but it keeps coming back, sometimes in the home z line as well as the g54 z line, other times in the home z line as well as the tl0 z line.
and i also now have a situation where as soon as i ok the insert tool command and step to the next line, it plunges the end mill right up to the chuck jaws.

jacques

p.s. i think the deities are bored and amusing themselves with me.....

i clear it, but it keeps coming back, sometimes in the home z line as well as the g54 z line, other times in the home z line as well as the tl0 z line.
and i also now have a situation where as soon as i ok the insert tool command and step to the next line, it plunges the end mill right up to the chuck jaws.

jacques

p.s. i think the deities are bored and amusing themselves with me.....

jlroch wrote:

p.s. i think the deities are bored and amusing themselves with me.....

They do seem like to do that sort of thing.

It is kind of hard to guess what you have going wrong without seeing everything and how they interact. (machine config, g-code file, and even the actual physical machine.)

yeah, i know. is there a way of "resetting " everything to default (short of uninstall/install linux cnc)?

ok. finally i get to thumb my nose at the deities!!!!
turns out that there is some kind of setting in my cam software (artcam) that is inserting that value "automagically" (probably as the result of my lack of comprehension of the cam software). i have put in a tech support call to autodesk so that they can help me with the problem. i will keep you posted.
thanks for your everlasting patience and sense of humor....

andypugh wrote:

jlroch wrote:

ok. finally i get to thumb my nose at the deities!!!!
turns out that there is some kind of setting in my cam software (artcam) that is inserting that value "automagically

Many CAM softwares insert a "G53 Z0" at the start of each program.

Now, on most machines Z = 0 is the top of travel and if there is 200mm or travel then the bottom of Z travel is -200.

I suspect you have set your machine up as 200 > 0 rather than 0 > -200 ?

Change the Z axis limits in the INI file and you will probably be OK.

That and stop using the home button as a touch off. Keep the machine Z0 at the top of travel where it belongs.

ok. so here's the result after autodesk support intervention.
turns out that in the post file for the "linux cnc inch" created by autodesk, there is a g43 line with an h value that conflicts with the manual value (when the z is set via home) of the z axis. the technician remarked that line out and all is well.
here is the post file with the rem line if anyone is interested:

; LinuxCNC PostP file for TC and ARC support
;
; === ======== ========================================
; JT 12/27/13 Created
;
DESCRIPTION = "LinuxCNC_Arc_inch_TC_No_H(*.NGC)"
;
FILE_EXTENSION = "ngc"
;
UNITS = INCH
;
; Cariage return - line feed at end of each line
;
END_OF_LINE = "[13][10]"
;
; Spindle Speed
FORMAT = [S|@|S|1.0]
; Feed Rate
FORMAT = [F|#|F|1.0]
; Tool moves in x,y and z
FORMAT = [X|#|X|1.4]
FORMAT = [Y|#|Y|1.4]
FORMAT = [Z|#|Z|1.4]
; Arc Center Coords
FORMAT = [I|@|I|1.4]
FORMAT = [J|@|J|1.4]
; Home tool positions
FORMAT = [XH|@|X|1.4]
FORMAT = [YH|@|Y|1.4]
FORMAT = [ZH|@|Z|1.4]
;
; Tool Number
FORMAT = [T|@||1.0]
;
; Set up program header
;
START = "([FILENAME])"
START = "(Material Size) (X=[XSIZE], Y=[YSIZE], Z=[ZMATERIAL])"
START = "G90G80G20G49"
START = "G64 P0.001"
START = "M6 T[T]"
START = "(Tool Number:[T]) ([TOOLDESC])"
;START = "G43 H[T] G0[ZH]"
START = "M3 "
;
; Program moves
;
FIRST_RAPID_RATE_MOVE = "G0 [X] [Y] [Z]"
;
FIRST_FEED_RATE_MOVE = "G1 [X] [Y] [Z] [F]"
FEED_RATE_MOVE = "[X] [Y] [Z]"
;
FIRST_CW_ARC_MOVE = "G2 [X] [Y] [J] [F]"
CW_ARC_MOVE = "G2 [X] [Y] [J]"
;
FIRST_CCW_ARC_MOVE = "G3 [X] [Y] [J] [F]"
CCW_ARC_MOVE = "G3 [X] [Y] [J]"
;
NEW_SEGMENT_POST_TOOLCHANGE="(Tool Number:[T]) ([TOOLDESC])"
NEW_SEGMENT_POST_TOOLCHANGE= "M3 "
;
;Setup Toolchange Commands
;
TOOLCHANGE = "G0[ZH]"
TOOLCHANGE = "M5"
TOOLCHANGE = "G49"
TOOLCHANGE = "M6 T[T]"
TOOLCHANGE = "G43 H[T] G0[ZH]"
;
; End of file
;
END = "G0[ZH]"
END = "G0[XH][YH]"
END = "M5"
END = "M30"
; M30 = program end and rewind


thanks for all the help from everyone in this time of difficulty. i will pay it forward whenever i can...

jacques

I appreciate the info on the G43 and Fusion 360, I was having the same issue with starting a file homing, touching off and then getting a plunge into the material 0.511 I saw where the tool offset was set.....but was going down the wrong path to compensate for it.

Now that I know to either comment out the G43 or add a G49 (Tool length cancel) I can move on to my next learning exercise.

Thanks DJB