M and G codes

[zmuda01]

I did a search and came up empty so I'll ask here.  Apologies if this has already been covered as it is odd that i did not see it anywhere.  I'm looking for a list of M and G codes that work for the Axiom ProV machines using the Rich Auto control.  I'm looking for G54, G28, M04 etc...  A full useable list would be nice.

Thanks
JZ

[dadealeus]

Hey JZ,

I'm not entirely sure what you're asking for, but I believe you might be looking for a compatible post processor for the Axiom machines? Basically a program that converts your cut paths from your software into something compatible for your machine to read?

If that's the case, I use the RS-274D / rs274 post processor with my AR8 Pro and it's never given me any issues (I use Fusion 360).

If that's not what you're asking for, then I don't believe I'm educated enough to give you a solid answer!

[zmuda01]

dadealeus,

I also use Fusion 360 and SolidWorks for modeling but have not posted a program out of either of them yet.  I will try the post you have recommended for Fusion 360 for sure.

In my career I have done a fair amount of CNC programming both via CAM software and MS Notepad.  I like to be able to edit G code to achieve favorable rough machining passes,  eliminate chatter, taper, decrease cycle time, etc....   Also, it's a hobby and I like it.

What I'm looking for here is a list of codes the Rich Auto controller will accept.  I know we can use the following:

M3
M4
M5
M30

G0
G1
G2
G3

Can we use M0, G28, G54, 55, 56?  Or any others?

I would like to be able to use variables and macros but I don't think it's a possibility on our platform.  

[dadealeus]

Ahhh, thanks for the explanation. I've only been a hobby-level machinist for around 3 years, so I haven't delved that deeply into what you're doing - but it does sound interesting.

Unfortunately, I'll have to leave your question to someone with more experience. However, If you don't receive an answer here, try giving Axiom a call; their support for things like this has always been great in my experience.

[pedro]

Oct 21, 2021 9:21:51 GMT -5 zmuda01 said:

dadealeus,

I also use Fusion 360 and SolidWorks for modeling but have not posted a program out of either of them yet.  I will try the post you have recommended for Fusion 360 for sure.

In my career I have done a fair amount of CNC programming both via CAM software and MS Notepad.  I like to be able to edit G code to achieve favorable rough machining passes,  eliminate chatter, taper, decrease cycle time, etc....   Also, it's a hobby and I like it.

What I'm looking for here is a list of codes the Rich Auto controller will accept.  I know we can use the following:

M3
M4
M5
M30

G0
G1
G2
G3

Can we use M0, G28, G54, 55, 56?  Or any others?

I would like to be able to use variables and macros but I don't think it's a possibility on our platform.  

Google for "RichAuto—AutoNow B18" , the manual of the controller. It has the list of all G Codes, about 2 complete pages. ITs a PDF, the link I had does not work, but I have the file. If you cant find it let me know and I can send it.

[pedro]

This is a copy and paste of that manual


G00 Rapid positioning
G01 Linear interpolation
G02 Circular interpolation CW
G03 Circular interpolation CCW
G04 Dwell (Unit: millisecond)
G17 Selection of XY coordinate plane
G18 Selection of ZX coordinate plane
G19 Selection of YZ coordinate plane
G20 Input in inch
G21 Input in metric
G28 Auto back to reference point
G30 Back to secondary reference point
G40 Cancel tool radius compensation
G41 Left tool compensation(the tool offsets radius distance on the left side of tool
moving direction)
G42 Right tool compensation(the tool offsets radius distance on the right side of tool
G43 Tool length compensation (compensation along positive direction)
G44 Tool length compensation (compensation along negative direction)
G49 Cancel tool length compensation
G54 Work coordinate system 1
G55 Work coordinate system 2
G56 Work coordinate system 3
G57 Work coordinate system 4
G58 Work coordinate system 5
G59 Work coordinate system 6
G73 High-speed peck drilling cycle for deep holes
G80 Canned cycle cancel
G81 Drilling cycle
G82 Drilling cycle of dwell at bottom of hole
G83 Peck drilling cycle for deep holes
G84 Right hand tapping cycle
G90 Absolute programming
G91 Incremental programming
G98 Return to initial point
G99 Return to point R
G101 Move with processing speed until the signal is triggered. Meanwhile Rollback
and pinpoint signal edge (similar to backing home)
G102 Move with fast speed until the signal is triggered. Meanwhile Rollback and
pinpoint signal edge (similar to backing home)
G103 Move with processing speed until the signal is triggered.
G104 Move with fast speed until the signal is triggered.
M03 Spindle on(CW rotation)
M04 Spindle on(CCW rotation)
M05 Spindle stop
M06 Tool change
M08 Coolant on (Flood)
M09 Coolant off
M30 End of program,and return to program top
M37 Spindle on(CW rotation)
M38 Spindle on(CCW rotation)
M129 4th spindle on
M208 Cycle machining
M210 Set output logic low level
M211 Set output logic high level
M214 Run the next line of G code after waiting for the specified input signal logic low
M215 Run the next line of G code after waiting for the specified input signal logichigh
M216 Run the next line of G code after waiting until all the specified input signal logic
high
M217 Run the next line of G code after waiting until anyone of all the specified input
signal logic high
M220 Set Y1 logic low level
M221 Set Y1 logic high level
M222 Set Y2 logic low level
M223 Set Y2 logic high level
M224 Set Y3 logic low level
M225 Set Y3 logic high level
M226 Set Y4 logic low level
M227 Set Y4 logic high level
M350 Set the extension output logic low level
M351 Set the extension output logic high level
T Tool function
S Spindle speed
F Feed rate
H Tool length offset

[pedro]

oh, I guess I bumped up a quite old post ;-)