Post Processor for RichAuto 11

[Anonymous]

Hello, 

Recently our school purchased an Axiom Auto Pro 8, when it was purchased we were advised to use AutoDesk Fusion 360 as our design software, as we can use a student version for free since the school budget is extremely tight. For about a month now checking forums and trying different ideas we cannot get the CNC to replicate what we designed on the program. In the manual it reads that the RichAuto 11 controller will read standard GCode, we have tried Grbl/grbl, and RS-274D/rs274d, neither one will produce a completed project without some kind of issue. Below I attached our latest try. We are also struggling with time, the program forecasts about 10 minutes, and the actual project takes almost 2 hours. I am definitely a novice so there can be other problems within the program. I am hoping to find an answer in why we are having these dependencies between what Fusion is showing and what is actually getting done, and is there a better generic G - Code to use? Is there a different program we should use? 

Your help is greatly appreciated

Thank you

[michaelkelly7104]

Hi René, thanks for your work on this post processor. I don't have the ability to test it currently, however attached are some files that may be of interest to your pursuit to perfect your post processor for this controller. One is a list of accepted G and M codes and the other is a file from Vectric that works correctly with the controller. Also, can I ask what the implications of the current post processor not outputting arcs in the Z plane would be for 3D machining? Thanks!

[daniel_lyall]

@michaelkelly7104  Have a look on the HSM forum for the RichAuto post there, the newest one was working ok for the guy that needed it.

https://forums.autodesk.com/t5/hsm-post-processor-forum/bd-p/218

[michaelkelly7104]

Thank you Daniel. I actually got around to testing the RichAuto post in this thread (just in air, with a variety of operations and motions) and it seems to work fine. The only problem is the machine doesn't pause for tool changes. Is there any way to make this happen?

Edit* As a matter of fact, the G/M code list I uploaded doesn't show M06 as a function of this controller - does that mean tool changes are not possible? Perhaps the controller needs to be updated?

Thanks

[daniel_lyall]

You have to do one toolpath at a time, you can try and see if a M01 or a M00 will work.

[michaelkelly7104]

I was hoping this wouldn't be the case 😞 It's surprising to me that this was an oversight if it's not possible. Thanks again.

[daniel_lyall]

Yep most people when they realize this are very disappointed that the machine needs toolpaths one by one, it is just the way low-end DSP controllers are personly I would never buy a machine with one.

[Anonymous]

The RichAuto A11 DSP does support tool change.  Refer to their manual but you might have to enable it in Advanced Setup as well.  This is not explained very well (like most operational capabilities).

Cheers,

[michaelkelly7104]

Wow, thank you! I've actually only been told that it doesn't up until now by people who own it, so I'll definitely have to dig deeper!

[rbtHTJJU]

Well, make sure your spindle ACCEPTS tools. Most of the machines (Axiom,
Powermatic and some Laguna tools to name a few) using RichAuto merely have
a collet receptacle and collet nut but do not actually support swapping out
tools.

Look for a tool retainer nut at the top of the spindle - when removed you
should be able to look completely through the bore of the spindle if so.

Good luck

[michaelkelly7104]

Hi, the spindle is an ELTE 0.8kW spindle and looks like this. When I remove the threaded collet holder (so it looks like in this photo) there is a bored out barrel which does stop after a few inches: 

[Anonymous]

Hold on...

ATC (Auto Tool Change) and manual tool change are two different things.  For manual tool change (Axiom and others using the A11), the machine will go to the tool change XYZ co-ordinate (manually) programmed into the A11 control and allow you to change the tool, it then allows a tool/depth setting to then proceed.  Your PostProcessor also needs to provide code for you (ie: stop spindle/restart) - this is part of the G-code.

To run an AutoTool Changer, this is also a part of the G-code generated to handle this but I doubt there are enough control signals on a basic RichAuto 3-Axis breakout board to handle this.  EG: control signals for the clamping mechanism within an ATC spindle.

[michaelkelly7104]

Hi Harry, all I'm really interested in is the manual tool change facility. The present issue for me is that the machine doesn't pause to allow me to change tools. The spindle powers down however the machine does not change position or wait for me to tell it to proceed. Haven't had a chance to mess about in the settings yet but I will have a look, thanks 🙂

[daniel_lyall]

Do any of you dudes have a pdf manual you could post?

[Anonymous]

The spindle icture you posted is a typical manual tool change model.  That's OK.  IT's a matter of setting up the A11 to go to the tool change position (by that it means XYZ co-ordinates).

This manual is re-written quite well: http://content.powermatic.com/assets/manuals/1797022_man_EN.pdf

This is more original:

https://system.na3.netsuite.com/core/media/media.nl?id=2325085&c=860860&h=1cc9976c8f3e3783e4cf&_xt=....

The RichAuto web-site also has the latest firmware and manuals:

http://www.richauto.com.cn/download/

A sequence of G-code to perform the G-code tool change is below but you have to tell the A11 via its "machine setup - G-code" and/or "advanced setup" to honor the behaviour.  Look for the Tool Change position (I set mine to be the G53 home position but you can set to be any where within the work envelope).

N1940 (ToolChangeOrg)
N1950 M05 (Stop spindle)
N1960 T3 M6 (TLDIA=4) (Select Tool number 3 and invoke Tool Change)

If you have the A11 set up properly, it will stop on the above line and wait/prompt you on the DSP hand pendant.  It will offer to do a "Tool Set" or "Tool has been changed".  If you select the first it will go through a length set.  The second will resume at the next line (in this case N1970).

Warning: Ensure you have a touch-off probe setup and know how to use it, otherwise you have to manually set the Z zero height for the new tool length.  If you don't know how to use this, be prepared to break some bits while you learn!

N1970 G01 X130.074 Y99.413 F100 M03 (This is the line after you tell it to continue)
N1990 (ToolChangeEnd)

Just so you know, you can also control spindle speed with the "S" word (if your spindle can be controlled) but again, you have to set up the DSP control using the Pendant under "Spindle Speed".  Where it has 8 speed settings, set S1 to zero and the others to the approximate values your spindle can be controlled for S8 being the highest.

[michaelkelly7104]

Hi Daniel, there's a brief section on tool changing here in the manual, but it's not very clear. https://system.na3.netsuite.com/core/media/media.nl?id=2325085&c=860860&h=1cc9976c8f3e3783e4cf&_xt=....

[daniel_lyall]

Thank you Guys

[michaelkelly7104]

Thank you Harry, this is fantastic to know. Really appreciate your help! 🙂

[Anonymous]

Hi, 

This post processors looks like its generating good g-code for my router. For spindle speed I understand we can alter the dsp controller to convert the programmed speed to the correct range number. 

However is it possible to get the post to output a number s1,s2,s3 etc for the chosen speed in fusion?

The reason I would like this option is I am still using v-carve to output g-code for the machine. If I alter the dsp then it would create an issue with my other post processor that is proven and still in use. The post processor from v-carve outputs the chosen spindle speed as s1,s2,s3 etc.

Thanks in advance 

[seth.madore]

Does S1,2,3 correspond to a set number, or range of numbers?

[Anonymous]

it applies to a range of numbers in 3000 rpm increments,

eg if we select rpm in program of between 1 and 3000 rpm it will post s1

3001-6000 rpm it will post s2

etc