Editing/Customizing Post Processor.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
How does one go about creating a new post processor in Fusion 360? We use a CNC Masters Supramill with the below information from the manufacturer. There doesn't seem to be any options in Fusion 360 to make a new processor or edit from an old one? Thanks!
You can hand this over to your CAM techincian to develop your post processor for the CAM software you are choosing to use.
You can also begin with a FANUC post as your base post and re-write it from
there according to the codes and definitions below.
Below is our current list of G-codes with definitions and instructions how our operational software reads
these codes. These are the typical file formats that our Master software can read: .txt, .nc, .cnw, .tap
The following list applies to all of our CNC Masters "Milling Machines":
G00 = Position (Rapid speed)
G01 = Linear interpolation (Feed speed) can be used with a F coordinate at the end of the line.
G02 = Circular interpolation (CW)
Format: X__Y__I__J__ I,J are relative distance from start to center.
Incremental Z can be added for helical designs. Important: The G02/03
commands must be written with X value Y Value I Value and J value on every
line for it to work properly. If you place a Z coordinate on the same line,
that will command the toolpath to run a helical program with X Y and Z running at the
same time.
G03 = Circular interpolation (CCW)
G40 = Tool Radius compensation off
G41 = Tool Radius compensation left -- IMPORTANT: At our setup window is
where we place the diameter of the tools. The G41/42 will then offset the
radius of the tool. So we don't need an extra D value. In order for a
G41/42 cycle to work properly -- every G-code must be entered individually
after the G41/42 until it is canceled with a G40. You cannot have toolpaths
without the G code listed in front of it, or the G41/42 will not work
properly. Lastly, you can only use these codes starting on a "linear" path,
and ending on a "linear" path. You cannot begin these codes on a G02/03.
You can only begin it and end it on a G00/G01. D values are not used. The user must
enter the diameter of the tool in the Master Software Setup, Tools Tab.
G42= Tool Radius compensation right
G70 = Input in inches
G71 = Input in millimeters
G73 = High-Speed Peck Drilling Cycle, Format: X____Y____Z____R____Q____P____F____
G81 = Drilling Cycle, Format: X____Y____Z____R____F____
G82 = Counter Boring Cycle, Format: X____Y____Z____R____P____F____
G80 = Cancel G73, G81, G82, or G83 Cycle
G83 = Deep Hole Peck Drilling Cycle, Format: X____Y____Z____R____Q____P____F____
Note on Peck, Drilling, and Boring Cycles: All values must be written except P and F which are optional.
The Q, which is the cut-in value cannot be left at 0.00 or the Z will not move down on this command.
The R point is above the work piece for G83. For G73, the R point retracts a small pre-determined distance
to break the chips and then feeds to the next peck allowing the tool to go deeper.
G90 = Absolute move (Modal)
G91 = Relative move (Modal)
M00 = Pause
M03 = Spindle on
M04 = Spindle on reverse
M05 = Spindle off
M08 = Coolant on
M09 = Coolant off
M30 = End program
/Notes -- The user can place notes in between lines of the program. When placing a note in between two lines of code,
the user must indicate the line after the note with a G or M code, if the code is not written in front of the line.
In this case it is best to write each tool path with its proper G-code/M-code in front of the toolpath so the operator
does not accidently break the modal with notes.
Resolution setting: The minimum resolution setting in inches is 0.0002".
The minimum resolution setting in mm is .005 -- only if the CAM can generate multiples of the .005 mm.
But if your system cannot handle multiples, then it is best to put your resolution setting at .01 mm
so your system can properly generate the correct values from there to run the program.
Tool Change, T commands
When placing a T command to do a tool change, a spindle off and Z quill retraction are not required. The T command
automatically will turn off the spindle and retract the Z going up. When the user is done makeing the tool change,
and resumes operation the Spindle will automatically turn on, Z will lower and offset and continue to machine from there.
If the operator needs to make a spindle speed change on the T command, use M03 to adjust the spindle on a separate line "before"
the T command line. Do not include PAUSE next to the T command. Do not generate files instantly with the T1 command at the
top. Only generate these T values if the user has "more" than one tool change in his program.
4th Axis Option
Our Fourth axis is recognized in the software as the W axis. It recognizes degrees only. It can interpolate with the other three
axes if the command is placed on the same tool path line.
Lastly, no spaces in between lines. Create toolpaths in list format.
*************************************************************************************************************************************
LATHE G-CODE AND M-CODE LIST
EXPLANATION OF CODE WILL ONLY BE WITH THOSE THAT DIFFER FROM THE ABOVE LIST
G00 = Position (Fast speed)
G01 = Linear interpolation (Feed speed)
G02 = Circular interpolation (CW)
G03 = Counter Clockwise Circular interpolation (CCW)
Format: X__Z__I__K__ I,K are relative distance from start to center.
G04 = Dwell time
G20 = Input in inches
G21 = Input in millimeters
G40 = Tool Nose Radius compensation cancel
G41 = Tool Nose Radius compensation left
G42 = Tool Nose Radius compensation right
G71 = Turning Cycle
START PT. X_Z_
FINAL DIA(X), LENGTH(Z), TAPER(I), TOTAL DEPTH(K), FIRST DEPTH(D), FEED(F)
G72 = Facing Cycle
START PT. X_Z_
FINAL DEPTH(Z), LENGTH(X), TAPER(I), TOTAL DEPTH(K), FIRST DEPTH(D), FEED(F)
G74 = Peck Drilling *(SAME FORMAT AS MILL G83)
G76 = Threading cycle
SPINDLE CODE G99 (S)SPEED M_
START PT. X_Z_
FINAL DIA(X), LENGTH(Z), TAPER(I), TOTAL DEPTH(K), FIRST DEPTH(D), INSERT ANGLE(A), INFEED(P), THREAD PITCH(F)
G90 = Absolute move (Modal)
G91 = Relative move (Modal)
G98 = Linear feed rate per time
M03 = Spindle on
M04 = Spindle on reverse
M05 = Spindle off
M08 = Coolant on
M09 = Coolant off
M30 = End program
