Othermill Pro Post-Processor

Discussion of post processors for various CNC machines

Othermill Pro Post-Processor

Postby DesignMakeTeach » Thu Dec 01, 2016 10:09 pm

Howdy,

Is there a dedicated Othermill Pro - post processor? Have not found one via search.

The following Instructable suggests using Basic GCode-Inch(*.nc) but then requires additional hand editing of the gcode file. http://www.instructables.com/id/Chocola ... he-G-code/

Thanks and have a great day.
-Josh
DesignMakeTeach
 
Posts: 1
Joined: Thu Dec 01, 2016 10:05 pm

Re: Othermill Pro Post-Processor

Postby Randy » Fri Dec 02, 2016 2:06 am

Hi Josh, and welcome to the forum. I'd never heard of Othermill. But their support page https://othermachine.co/support/2d-3d-d ... d-and-cam/ recommends MeshCAM so they must have done some testing. Have you tried emailing their support and see if they have an internally-used MeshCAM post?

The Instructables page to which you linked just says that you need to add spindle commands to the gcode. That is easy to add in the postprocessor. I'll edit up a basic gcode post and attach it later.

If you want to do some reading in the meantime, check the threads viewtopic.php?f=3&t=15550&p=24806 and viewtopic.php?f=3&t=15420&p=24125 which discuss adding spindle commands to a post.

Overview about the postprocessor is in MC's Help and also at http://www.grzsoftware.com/manual/overview.htm

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: Othermill Pro Post-Processor

Postby Randy » Fri Dec 02, 2016 6:02 am

Josh, give this a try. You'll need to enter your endmills into the MeshCAM tool list, and you'll probably need to still hand-edit the output gcode for the spindle RPM you want. I always do. There has never been a MeshCAM output gcode that I didn't tweak in some way...

Code: Select all
; MeshCAM config
; This config is the basis for the minimum
; gcode output. If you're looking for
; the shortest output file then this is the config
; to start with.  Also show how to integrate CutViewer config into
; the output.
;
; 2/29/04    Changed comments to be enclosed by () rather than start with ;
;      Added CutViewer config output
; 5/13/04    Added toolchange gcode
; 2/12/05   Changed name and added units
; 3/17/05   Changed stock definition to use CUTVIEWERSTOCK variable
; 5/19/05   Removed feedrate command for rapid moves
; 5/25/05   Added dummy tool for CutViewer
; 6/27/05   Changed the formats to 1.4 to get 4 decimal places of accuracy
; 9/28/10       branched to the "arcs" version
; 12/01/16      added spindle commands
;
DESCRIPTION = "Basic GCode-Inch Arcs spindle(*.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 = [SZ|@| Z|1.4]
;Tools
FORMAT = [T|@||1.0]
FORMAT = [S|@| S|1.0]
START = "%"
START = "(FILENAME: [FILENAME])"
; The following is a dummy tool to keep CutViewer from generating an error when G20 is called without a tool
START = "(TOOL/MILL,0.1,0.05,0.000,0)"
START = "G20G17"
START = "([CUTVIEWERSTOCK])"
;
TOOLCHANGE = "([CUTVIEWERTOOL])"
TOOLCHANGE = "M5 (spindle off)"
TOOLCHANGE = "M6 [T]"
TOOLCHANGE = "M3 [S] (spindle CW)"
;
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][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]"
;
;
END = "M5 (spindle off)"
END = "(END OF PROGRAM)"
END = "%"


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


Return to Post Processors

cron