Buildlog.Net Blog

Creating A Laser Post Processor

Virtually all CAM systems allow you to target different CNC machines through the use of a Post Processors (post).  Post Processors tailor the ouptut to the target machine.  While most machines can handle G-Code, each machine has it’s own requirements.  Many Post Processors are so flexible that you can even get them to output HPLG, DXF, and other vector based file formats.

Post Processor formats and rules vary between manufacturers, but the general procedure of creating a custom one is basically the same.  I will detail how I created a basic Mach3 E1P1 style post processor for my Vectric Aspire CAM program.  Aspire is way overkill for a laser, but this Post Processor will work for all the Vectric products including the more affordable CUT2D which is perfect for a laser.  Most CAM vendors will produce a guide for the post processor format.  I got the one for Vectric from their forum.

Most programs ship with many Post Processors.  Start with one that is closest to what you want.  In my case I picked a Mach2/3 Arcs (inch) post.  This targets Mach3, and uses arcs for curves instead of multiple line segments.  You should also create a simple CAM file to test.  I created one with a 1″ x 2″ rectangle and a 1″ diameter circle.  Both items are offset from home.  Locate the items on a simple grid so it is easy to find the items in the resulting G-Code.

Study the existing post’s output.

I started by creating a G-Code file from the existing post.  To simplify the resulting g-code, do a profile cut on the lines with a single pass.  My file had a home position of 0,0,1 and did a single pass cut at Z = -1.  The rapid clearance gap was 0.5″.  A snippet of the resulting G-Code file is here.

N100G00G20G17G90G40G49G80

N110G70G91.1

N120T1M06

N130 (Tool: End Mill {0.25 inch})

N140G00G43Z1.0000H1

N150S12000M03

N160(Toolpath:- out)

N170()

N180G94

N190X0.0000Y0.0000F100.0

N200G00X1.0000Y1.0000Z0.5000

N210G00X1.0000Y1.0000Z0.2000

…

…

N360G00Z1.0000

N370G00X0.0000Y0.0000

N380M09

N390M30

So what the heck does all this mean?  Well, me to the rescue (again).  I created this G-Code Commenter.  You paste G-Code on one side and it copies it to the other with comments explaining the code.

.

By looking at the resulting file I created a list of things I need and want to change.

• Remove spindle control commands, M03 (on) near the beginning and M05 (off) near the end.
• Remove any spindle speed commands like the S1200 in the file above.
• Remove any tool change commands T1M06, tool offsets, compensation, etc.
• Remove any mist coolant type commands like M07,M08,M09.  (Later you may want to re-purpose these for assist air).
• Remove any references to the Z axis.  For this cutter application, we only want 2D motion.
• Add in the beam on, E1P1 and beam off, E1P0 commands before and after each cut.
• Readability.  G-Code does not care where spaces and line feeds are, so adding a few of these can make the code a lot easier to read.

Create the new post.

The post processor file is divided into sections, like HEADER, FOOTER, RAPID_MOVE, FIRST_FEED_MOVE, etc.  When the CAM program is creating the output file, it follows the format in these sections.  Below is the section for RAPID_MOVE.

+—————————————————

+  Commands output for rapid moves

+—————————————————

begin RAPID_MOVE

“[N]G00[X][Y][Z]”

The letters in square brackets are variables.  In this case, N is an incrementing line number, XYZ are the desired XYZ destination for the rapid move.  All we need to do to this line is remove the [Z].  I also added spaces between all the commands and variables for readability.

+—————————————————

+  Commands output for rapid moves

+—————————————————

begin RAPID_MOVE

“[N] G00 [X] [Y]”

Leaving the E1P0/E1P0 issue for later we go through each section and apply the desired changes from the list above.  In the HEADER section I also split up the commands onto their own lines.  You may want to try creating G-Code from your post a few times along the way to see it is is doing what you want.  I also ran my on my laser a few times to see if it was doing what I intended.  Be sure to lockout the beam during your initial tests.

The last task is to apply the E1P1/E1P0 Beam On/Off commands to the file.  The post file has a FIRST_FEED_MOVE section.  This was a good place to turn my beam on.  I put “[N] E1P1” as the first line of the section.  To turn off the beam, I put “[N] E1P0” at the beginning of the RAPID_MOVE section and just for safety, I also put it at the beginning of the FOOTER section.

The compete post is here.

Here is the G-code from my post.

( t3 )
( File created: Saturday, July 10, 2010 - 01:34 PM)
( for Mach2/3 from Vectric/bdring )
( Material Size)
( X= 2.000, Y= 2.000, Z= 0.234)
()
(Toolpaths used in this file:)
(t3)
(Tools used in this file: )
(1 = Laser Mill {0.005 inches})
N100 G00
N110 G20
N120 G17
N130 G90
N140 G80
N150 G70
N160 G91.1
N170 (Laser Mill {0.005 inches})
N180 G00
N190 (Toolpath:- t3)
N200 ()
N210 G94
N220 X0.0000 Y0.0000 F150.0
N230 E1P0
N240 G00 X0.0000 Y0.0000
N250 E1P1
N260 G1   F30.0
N270 E1P1
N280 G1 X1.0000  F150.0
N290 G1  Y1.0000
N300 G1 X0.0000
N310 G1  Y0.0000
N320 E1P0
N330 G00
N340 E1P0
N350 G00 X0.03 Y0.03 (Insure a move before end)
N360 G00 X0.0000 Y0.0000
N370 M30
%