Trying to setup Auggie on cnc machine

[ArtF]

Hi:

>>Alternatively, Could I wire my "z0" probe to the z limit + and do a move until it reaches the limit?

  Yes, you can do that , but an Estop will occur to end the probing. A limit will trip the Estop. Not a
problem really, but you will have top press reset to continue.

  The first idea will not work, this is because Auggie sends 1ms packets, so it may have a
seconds motion already sent any any time.

  You can read inputs and set outputs. They respond within a few ms generally, but are
not ensured to be in sync with motion.

Art

[Cyrille]

Hello,

So, really, I would need to move for 20ms at 1cm/s (=0.02mm), wait for 20ms or so, to make sure that the move is finished (is there a wait/Pause in your scripting language?).
Test the input and loop.Would that work?

Cyrille

[ArtF]

Cyrille:

  Well, you wouldnt have to wait I guess, the process of switching to the script thread
and such will have at least a few ms delay, probably 100ms or so.  One of the problems is the
Engine.Feed is in absolute.. unless gcode has set it to incremental...hmmmm..

  Its been too long since Ive looked at it, Cyrille, Ill dig into the code
to see just how one could do a touchoff on an axis. I may be able
to add a simple type of move till hit routine as a script call or something...

  Give it a few days..

Art

 

[Cyrille]

Hello,

Thank you for doing/checking this, I truly appreciate the time that you are spending helping me...

I have another question. Do you have a ? list ? of the subset of code that auggie does support? I am asking as my cam tool does not produ?e code, but something quite close and I will need to program a ? transcoder ?...

Actually, this is a good question, can a ? load gcode ? ?vent trigger a script that could automatically execute an external program so that I would not need to manually run my transcoder on each tool path, but the transcoder would be automatically called by auggie? This is just a wild idea to improve user interface, there is no need for you to work on it or anyth8ng like this, I am just wondering if the right hooks and functionalities are in place in auggie or not.

Thanks,
Cyrille

[ArtF]

Cyrille:

  The scripting language has quite a few system hooks so it can probably be done.
Im not sure theres an auto Gcode load event, but it is possible to add a button to
call a created dialog.. Watch the video on Dialog creation.. or the thread..I cant recall
how I did the tutorial on that subject.
  The Dialogs library shows some system call examples I think... Theres a lot
in there that could keep you busy for a long time.

  As to the Gcode subset, I believe its easiest to say it implements pretty much
what Mach3 has with the exception of probing, threading, and G43 type cutter
compensations. Pretty much everything else I think is there with few exceptions.
When not implemented, the normal operation is to either issue an error or look
for a script, in which case the log will tell you it tried.

Art

[Cyrille]

Hello,

What do you think is my best path to convert my input files?
An external program?
Or using auggie's awsome (trully) ability to interpret input files?

Headers and the like asside, my files look like this:

TR,18000    // spindle speed  Gcode equivalent: ????
J2,0.000000,0.000000 // Jog: G01
J3,9.627712,105.045639,5.000000
M3,9.627712,105.045639,-1.000000 // feed G02
CG, ,6.040212,108.633133,0.000000,3.587494,T,1 // Arc G02/03

Creating a text processing program pauses no issues for me, but just checking if they was not an even lazier solution :-)

Cyrille

[ArtF]

Wow, one horrible file.

  If it were me, Id write a post processor to deal with it, I dont
think Auggie will conform it easily to anything. Sometimes
you just have to make a hack. :)

Art

[Cyrille]

Hello,

Well, that is what I did... I wrote a "translator"...
However, since I never learned/wrote any G-Code, I have no idea if it is valid or not:-(

Here is what I generate. Does it look valid?

G21 G17 G90
S18000 M03 G04 P2

G0 Z20.000000
G0 X0.000000 Y0.000000
G0 X9.627712 Y105.045639 Z5.000000

G01 X9.627712 Y105.045639 Z-1.000000 F1518.000000

G02 X6.040212 Y108.633133 I0.000000 J3.587494 F3036.000000

G03 X32.130943 Y102.765289 I0.000000 J0.412506 F3036.000000

M05

Cyrille

[ArtF]

Cyrille:

  Looks to me like you cracked it fine.

Im in the process of adding a G38 for probing, and I notice I never turned on
tool length offset either, so Ill see if I can attach those hooks as well. Cant promise
anything at this point,but the process is underway.

Art

[ArtF]

Cyrille:

  The new G38 command seems to work well in rough testing. It is multiaxis
so one can probe with G38X10Y10Z-10 F100 and the axis will decelerate to a
stop when probe is hit. I havent done anything as yet with the hit point
data. One can I suppose set a tool by hitting a probe plate at F100, then do
an F10 , invert the probe signal and probe off with a Z move upwards. I think
I will add a way to zero to the probe hit data before I release it.

Art

[Cyrille]

Hello,

This sounds great...

Do you have an idea of the time between signal sensing and movement stop? Just to get an idea of the precision that can be obtained (not that I need too much anyway)?

Cyrille

[ArtF]

Cyrille:

  The way it works is the command G38 is interpreted as a G1 move, BUT the probe is set
to stop the move. We dont want to lose steps, so when the probe is hit, the Pokeys
automatically switches from Auggie's trajectory planner to its internal planner, takes control
and decelerates all axis to a stop using your max accel parameter. It then switches back to
Auggies planner.
  Auggie clears its g1 move from that point onwards, and receives a
position packet from the pokeys telling it where the probe hit at.

  I dont yet give access to the hit point. So if you do a g38 xyz..F100
you will be off the real zero by the deceleration distance of the f100 move,
so by then reversing the probe signal and probing off the point with
G38Z5F1 , you will stop when the probe releases.. and with f1 as the feedrate
youd probably be off by perhaps as little as 1 step. Perhaps less.

  Conversely you could simply do a g38Z-20F1 to start with
and get pretty much an exact zero.

Eventually Ill add a button to "Zero to Probe" where the zero will be
automatically set to a offset of the probe hit point. Pressing goto zero
will then zero you to the exact point.

Art
 

[Cyrille]

Hello,

OK, I understand now...

Obviously, the "probe to 0" is, ultimately, what I Was looking for, but I can always execute the G38, and then manually set the z axis at 0. it's not like it is a complicated operation, nor is it something that is done 10 times a minute!

Can one "script" gcode excution? I mean, I can, programatically tell auggie to execute some Gcode?

Cyrille

[ArtF]

Cyrille:

  I dont think I added a way to exectute a Gcode line from script. Though you can add
scripts to GCode. In Gcode a brace signifies a switch to script.

ex:

G0X10
{
  GlobalSet("ProbeInvert", 1 );
}
G1Y12X5

  Script can be injected to the Gcode this way. But I dont think I coded the other way to add
GCode to a script. Ill look into why I didnt, there may be technical reasons.
It may be I did add it though, Ill take a look in the code, it isnt something Ive used but
I added a great deal in there thats undocumented. 

Art

[ArtF]

Cyrille:

  I just confirmed I didnt add and script command to execute GCode. So Ill have to add a script
command to allow a G38 call. Pretty much anything else can be scripted with calls such
as Engine.ArcTo or FeedTo(.. ) etc..

  Probe however, is only accessable by Gcode, Ive been testing it in MDI calls. Hadnt occured
to me till you asked it needed to be called by script. You can invert the probe by script
but not the probe itself. I will add that before I release it.

Art