Starting the tool at the first cut position?

Discussion of post processors for various CNC machines

Starting the tool at the first cut position?

Postby MikeH » Thu Dec 08, 2016 5:22 am

Hi, I'm new here and would really appreciate some help. I had a post processor for MeshCAM made for the FAGOR 8037 controller.
When we run the tool path, it goes to the zero home and then to the first cutting position. How can I start at the first cut instead?
I am not sure if there is a command or which line in the processor I should change.

Here is the post in case anyone can use it:

; MeshCAM config
; This config is the Fagor8037-MM machine controller
; http://www.artofcnc.ca
;
; 2/29/04 Changed comments to be enclosed by () rather than start with ;
; Added CutViewer config output
; 5/13/04 Added toolchange gcode
; 3/17/05 Changed stock definition to use CUTVIEWERSTOCK variable
; 3/22/05 Added UNITS statement
; 8/02/05 Removed [F] statement from rapid moves
; 1/21/07 Added 4 axis support
; 2/16/07 Added G64 in start
; 2/11/09 Changed to Fagor8037-MM
; 10/13/09 Enabled spindle start/stop and spindle speed
; 9/28/10 branched to the "arcs" version
; 06/16/11 Changed END statement
;
DESCRIPTION = " Fagor8037-MM(*.PIM)"
FILE_EXTENSION = "PIM"
UNITS=MM
;Feeds
FORMAT = [F|#|F|1.1]
;Moves
FORMAT = [I|@|I|1.4]
FORMAT = [J|@|J|1.4]
FORMAT = [X|#|X|1.4]
FORMAT = [Y|#|Y|1.4]
FORMAT = [Z|#|Z|1.4]
FORMAT = [R|#|A|1.4]
;
;
COMMENT_START = ";"
COMMENT_END = " "
;
START = "%[FILENAME],MX--"
;START = ";[FILENAME]"
;START = ";[TOOLDESC]"

;;the following sets the stock for CutViewer
;START = "([CUTVIEWERSTOCK])"
START = "G90 G44 G40 G80 G0"
START = "G53"
START = "G0 Z0"
; START = "(ORGX58=0,ORGY58=0,ORGZ58=0)"
START = "M61 ; VACUUM ON"
START = "M63 ; DUST COLLECTOR ON"
START = "G70"
START = "S16000 M3"
START = "G4 K300"
START = "G51 A085 E0.01"
START = "; Toolpath : Bot__om__1"
START = "G57"
START = "G71"
;
;TOOLCHANGE = "([CUTVIEWERTOOL])"
;TOOLCHANGE = "M6 [T]"
;TOOLCHANGE = "M3 [S]"
;START = "G00 [X] [Y]"
;START = "G43 [Z] D1"
;
START = "G00 X0 Y0"
START = "G43 Z [ZMAX] D1"
;FIRST_RAPID_RATE_MOVE = "G43 G00 [Z] D1"
RAPID_RATE_MOVE = "G00 [X] [Y] [Z]"
;
FIRST_FEED_RATE_MOVE = "G01 [X][Y] [Z] [F]"
FEED_RATE_MOVE = "[X] [Y] [Z]"
;
FIRST_CW_ARC_MOVE = "G02 [X] [Y] [I] [J] [F]"
CW_ARC_MOVE = "G02[X][Y][I][J]"
;
FIRST_CCW_ARC_MOVE = "G03 [X] [Y] [I] [J] [F]"
CCW_ARC_MOVE = "G03 [X] [Y] [I] [J]"
;
;
END = "M5"
END = "M62 ; VACUUM PUMP OFF"
END = "M64 ; DUST COLECTOR OFF"
END = "G44"
END = "G70"
END = "G53"
END = "G53 G0 Z0"
END = "X0.1 Y0"
END = "M30"
;END = "(END)"
;END = "(OF PROGRAM)"
MikeH
 
Posts: 2
Joined: Thu Dec 08, 2016 4:39 am

Re: Starting the tool at the first cut position?

Postby Randy » Tue Dec 13, 2016 1:19 am

Hi MikeH, and welcome to the forum. I'm sorry about the delay in passing your posts, but I was away from the forum for a few days.

First of all, thank you for contributing the post! That is a nice gift to the user base.

The move to X0.0000 Y0.0000 Z[something] is something that MeshCAM just does. It isn't configurable in the postprocessor, and it appears in every gcode file MeshCAM outputs.

The way I deal with it, is to open the gcode in a text editor, go to that line, and remove the X0.0000 Y0.0000 and leave just the Z value, which should be the safety (retract) height.

Then, the spindle will go from wherever it is straight to the beginning of the cut.

When I've touched down the first tool on the stock I generally just move it up a little and leave it there. It is indeed a little frustrating to have the tool take a detour over to X0 Y0 and then back.

Randy
All opinions in this post are mine alone. I am not a MeshCAM employee, I do not have a financial interest in MeshCAM, nor do I speak for MeshCAM. MeshCAM user since Beta 5 in 2003. viewtopic.php?f=11&t=15333 :ugeek:
Randy
 
Posts: 1812
Joined: Wed May 14, 2008 9:50 am
Location: North Texas, USA

Re: Starting the tool at the first cut position?

Postby cnczane » Thu Aug 17, 2017 5:56 pm

I do EXACTLY the same thing: I don't like the idea of moving in X or Y unless and until I am sure the cutter is at a safe height.

(Sometimes, even when I'm sure, I'm wrong... :shock: )
If you have not received a reply from me in over a year, I am not ignoing you: more likely I am fallen asleep under a tree. Again. Please poke me if you think it worth your trouble.
cnczane
 
Posts: 277
Joined: Sun Sep 21, 2008 4:15 am

Re: Starting the tool at the first cut position?

Postby cnczane » Thu Aug 17, 2017 6:23 pm

I recommend adding a line like this, early in the .con/post file:
START = "G53 G90G0 Z<averysafeveryhighelevationintheabsolutecoordsystem>"

At least, presumably, you'll be coming DOWN later when MeshCAM executes G0 X0Y0Z<safe>

BTW, I note what I consider are wasted lines in your post file.
MikeH wrote:...
START = "G53"
START = "G0 Z0"
...
END = "G53"
END = "G53 G0 Z0"
...


In my case, LinuxCNC, the absolute coordinate system "G53" is "non-modal" which is to say that one cannot tell the controller to "go into it and stay there". G53 commands are good for the life of the command line they are found on. In LinuxCNC case, line containing only "G53" means "go into the absolute coordinate system, do nothing, and go back to the coord system you were in just before." That also means that the line "G0 Z0" following a simple "G53" line means "go to Z0 in the current coordinate system"--which won't be G53, because it is not on the same line with the G0.
If you have not received a reply from me in over a year, I am not ignoing you: more likely I am fallen asleep under a tree. Again. Please poke me if you think it worth your trouble.
cnczane
 
Posts: 277
Joined: Sun Sep 21, 2008 4:15 am


Return to Post Processors

cron