Tormach PathPilot

[scslowik]

Is anyone using Meshcam with the new Tormach PathPilot controller?
If so, does anyone have a post processor for it?

[Randy]

Hi scslowik, and welcome to the forum. I use Mach3 on my Tormach, so I'm not sure what would be different about the PathPilot controller. MeshCAM is geometry-driven so its motion gcode won't be any different whatever machine you have.

For what it's worth here is my Tormach Mach3 post

Code: Select all

; MeshCAM config
; This config is for Randy's Tormach PCNC
;
; 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
; 11/19/06      Added G43, M3 lines to toolchange (RG-G)
; 11/26/06      Added PLUNGE_RATE_MOVE, Tools FORMAT (courtesy JeffD)
; 12/16/06      Moved CUTVIEWERTOOL to M6 line
; 1/1/07        Added S word format
; 1/20/07       Added dummy "S4500" for default rpm
; 7/21/07       Added M9 and M8 statements to toolchange
; 8/8/07        Added M998 statement to toolchange
; 8/19/07       Changed M2 to M30
; 9/23/07       Added FP and SZ formats, added SZ and FP to PLUNGE_RATE_MOVE
; 11/17/08      Reworked toolchange
; 10/22/09      Changed SZ format from # to @
; 3/30/10       Added COMMENT lines, courtesy jeffD and Robert
; 12/23/10      Added arc moves for V4
; 2/4/11        Added A axis format
; 8/23/11       Changed dummy RPM into real RPM
; 10/30/13      Added I,J format lines
;
DESCRIPTION = "Tormach-Inch RG-G(*.nc)"
FILE_EXTENSION = "nc"
UNITS = INCH
;Feeds
FORMAT = [F|#| F|1.1]
FORMAT = [FP|#| F|1.1]
;Moves
FORMAT = [X|#| X|1.4]
FORMAT = [Y|#| Y|1.4]
FORMAT = [Z|#| Z|1.4]
FORMAT = [R|#| A|1.4]
FORMAT = [I|#| I|1.4]
FORMAT = [J|#| J|1.4]
FORMAT = [SZ|@| Z|1.4]
;Tools
FORMAT = [T|@||1.0]
FORMAT = [S|@| S|1.0]
;
START = "%"
START = "(FILENAME: [FILENAME])"
START = "([CUTVIEWERSTOCK])"
START = "G20 G17 G40 G80 G90"
;
TOOLCHANGE = "M09 (coolant off)"
TOOLCHANGE = "M05 (spindle off)"
TOOLCHANGE = "M998"
TOOLCHANGE = "M06 T[T] G43 H[T] ([CUTVIEWERTOOL])"
TOOLCHANGE = "G0[SZ]"
TOOLCHANGE = "M08 (flood coolant on)"
TOOLCHANGE = "M03 [S]"
;
COMMENT_START = "("
COMMENT_END = ", Tool [T])"
;
RAPID_RATE_MOVE        = "G0[X][Y][Z]"
FIRST_FEED_RATE_MOVE   = "G1[X][Y][Z] [F]"
FEED_RATE_MOVE         = "G1[X][Y][Z]"
;
FIRST_CW_ARC_MOVE      = "G2[X][Y][I][J][F]"
CW_ARC_MOVE            = "G2[X][Y][I][J]"
;
FIRST_CCW_ARC_MOVE     = "G3[X][Y][I][J][F]"
CCW_ARC_MOVE           = "G3[X][Y][I][J]"
;
;
;rapid down to safe Z, plunge to final Z
PLUNGE_RATE_MOVE       = "G0[SZ]"
PLUNGE_RATE_MOVE       = "G1[Z] [FP]"
;
END = "M09 (coolant off)"
END = "M05 (spindle off)"
END = "M998"
END = "M30 (END OF PROGRAM)"
END = "%"


I like to lower the head to the safe Z level before I turn on the flood coolant, to save some splashing and I've added the Tormach M998 call to raise the head to toolchange postition because I change tools manually. Otherwise it's really standard arc-enabled code.

Randy

[scslowik]

Hi Randy,

Thanks for the reply.

I merged the EMC post processor with your code to get a valid post processor for Tormach with PathPilot.

One question ... you have two lines that use the PLUNGE_RATE_MOVE variable.

A rapid to Safe Z and a G1 to Z at plunge feed rate.

How does Meshcam translate that? I seem to only get the G1 move in my final g code.

[Randy]

scslowik, you're welcome. And I'm glad you worked things out for your PathPilot.

You'll only see a G0 at the plunge move if you're starting out above the Safe Height (=Retract Height). I added the G0 line becuase the first move downwards from the M998 tool change height starts 8-10 inches typically above my workpiece, and I didn't want the coolant to come on until the head was most of the way back down. In normal machining, the tool will never go above the safe/retract height so the only time the G0 appears is on the first downwards move after a toolchange.

Randy