Dynapath 20 Basic Programming question

[wildwhl]

Yes, a copy and past of what I sent to the machine this afternoon. I notice after it loads the Dyna-controller says *editing* before it is done. When I view the code it is slightly different than what I have posted above, but essentially the same. Machines fine, without errors, all the way down to line 45.

I noticed the sample posted by michaelthomas also has 2 gcodes on the first line N15:


(NMTB)
N15G70G90
N20E01T5M06(1 1/2 Face Mill)


Please excuse my basic questions, as I'm still pretty new to this. Should line 45 possibly be posting as a G2 or G3 event? Maybe I need to alter the post-processor in such a fashion? Looking at the part, this is when the first arc would begin I think, too. I am climb milling, CCW direction I believe. Also notice the S and M event together in line N30 of michael's sample and line N5 of mine...hmmm...

Program is for a simple 2" square pocket (ran fine) until I set corner radius to something other than zero (technically tool radius I suppose).

I'll plug away more tomorrow - just want to have some ammo to throw at it

Bill

[Fighter]

I believe you are still in incremental on your arc moves, and the Dynapath is looking for Absolute. Hence the error message.

I don't do any Incremental programming, so it looks like Chinese to me.

[wildwhl]

Thanks Fighter -

In this line:

N47G3X1.175Y0.9125I0.0J0.025

EDIT: Found this:

I code = Absolute center of arc in x-axis
J code = Absolute center of arc in y-axis

and this:

The difference between programming in "Absolute" and "Incremental" is very simple on this control. All you do is add a "/" after the number you want to be Incremimental, and no "/" if you want absolute. This is in conversational mode which is what i use almost exclusivly, although you can mix "Regular" g-code in with it if you want.

Still googling...

[Fighter]

The Absolute/Incremental setting that needs to be changed is in your CamBam
"Machining" folder. Set the "Arc Center Mode" to "Absolute" prior to generating G-code and then see if the controller still faults on arc moves.

If you are programming the Dynapath using G-Code, G90 and G91 set Absolute or Incremental mode. If programming using Conversational, you would use the "/" for Incremental.

You can't generate G-code in Incremental mode and have it run properly if the controller is in Absolute mode, which is what you seem to have done above.

They need to match or it will fault as it did.

[wildwhl]

Thanks Fighter. Pretty sure I have CamBam set for absolute, but I'll verify in the a.m.

Bill

EDIT: Used the laptop and recreated the simple program/post processor settings best I could from memory. Think you've nailed it on the head Fighter, code looks like this now (haven't run through editor for block numbers/etc.) take note to how the origins look after the G3 command...think I'll go in early tomorrow


(TEST)
G20 G90 G64 G40
G0 Z0.25
T6 M6
G17
M3 S4000
G0 X0.9875 Y0.9875
G1 F10.0 X1.0125 Z-0.0375
G1 Y1.0125 Z-0.075
G1 X0.9875 Z-0.1125
G1 Y0.9875 Z-0.15
G1 X1.0125
G1 Y1.0125
G1 X0.9875
G1 Y0.9875
G0 Z0.0
G0 Y0.8
G1 X1.2 Z-0.0199
G1 Y1.2 Z-0.0574
G1 X0.8 Z-0.0949
G1 Y0.8 Z-0.1324
G1 X0.9875 Z-0.15
G1 X1.2
G1 Y1.2
G1 X0.8
G1 Y0.8
G1 X0.9875
G0 Z0.0
G0 Y0.6125
G1 X1.3875 Z-0.0194
G1 Y1.3875 Z-0.0569
G1 X0.6125 Z-0.0944
G1 Y0.6125 Z-0.1319
G1 X0.9875 Z-0.15
G1 X1.3875
G1 Y1.3875
G1 X0.6125
G1 Y0.6125
G1 X0.9875
G0 Z0.0
G0 Y0.425
G1 X1.575 Z-0.0192
G1 Y1.575 Z-0.0567
G1 X0.425 Z-0.0942
G1 Y0.425 Z-0.1317
G1 X0.9875 Z-0.15
G1 X1.575
G1 Y1.575
G1 X0.425
G1 Y0.425
G1 X0.9875
G0 Z0.0
G0 Y0.2375
G1 X1.65 Z-0.0168
G3 X1.7625 Y0.35 Z-0.0213 I1.65 J0.35
G1 Y1.65 Z-0.0543
G3 X1.65 Y1.7625 Z-0.0588 I1.65 J1.65
G1 X0.35 Z-0.0918
G3 X0.2375 Y1.65 Z-0.0963 I0.35 J1.65
G1 Y0.35 Z-0.1293
G3 X0.35 Y0.2375 Z-0.1338 I0.35 J0.35
G1 X0.9875 Z-0.15
G1 X1.65
G3 X1.7625 Y0.35 I1.65 J0.35
G1 Y1.65
G3 X1.65 Y1.7625 I1.65 J1.65
G1 X0.35
G3 X0.2375 Y1.65 I0.35 J1.65
G1 Y0.35
G3 X0.35 Y0.2375 I0.35 J0.35
G1 X0.9875
G0 Z0.0
M5
E

[Fighter]

I don't believe you have G20 or G64.

I prefer the X,Y G0 prior to the Z after a tool change.

Maybe this:

(TEST)
G90E00
G40
T6 M6
G17
M3 S4000
G0 X0.9875 Y0.9875
G0 Z.250
G1 F10.0 X1.0125 Z-0.0375
G1 Y1.0125 Z-0.075
Etc...

[wildwhl]

Fighter -

if you were here, I'd be buying drinks and/or dinner tonight.

Incremental was still selected - time to get serious now

Bill

[jagardner4]

Just adding my two cents:

The code would indicate that you are moving the Z axis during your XY arc move:

'G1 X1.65 Z-0.0168
G3 X1.7625 Y0.35 Z-0.0213 I1.65 J0.35
G1 Y1.65 Z-0.0543
G3 X1.65 Y1.7625 Z-0.0588 I1.65 J1.65
G1 X0.35 Z-0.0918
G3 X0.2375 Y1.65 Z-0.0963 I0.35 J1.65
G1 Y0.35 Z-0.1293
G3 X0.35 Y0.2375 Z-0.1338 I0.35 J0.35
G1 X0.9875 Z-0.15
.
.
.'

I'm not certain how the control will react, but G Code arc moves on this control are definitely limited to 2 axes. (side note: helical arcs are possible with conversational arc events - giving you arc moves in 2 axes and a simultaneous straight line move in Z only.)

I also think the control may execute a line with multiple G Codes, but will only execute the first G Code on the line, ignoring any others.

[wildwhl]

Thank you for the response jagardner4.

I made huge progress yesterday, first importing 3d objects into cambam, then post-processing (nearly) perfect g-code that required very little edits (block numbers only), then drip feeding with easyDNC. Still a long ways to go, but very happy with the results and can't say enough good things about the kind and helpful members on this forum.

I did not let this cut file finish - but the process was waterline roughing, then vertical and horizontal finishing with a reasonably small step over. Goal was more to get a lot of code to run successfully, and not so much to make a finished part that was correct - that will come next.

Bill

[Fighter]

Geez, I never even noticed the X,Y,Z arc moves! I was paying attention to the I,J.

Funny how the control sometimes acts.

I ran a complete part program once (drip feeding) and on the second part it stopped about half way through the program. I couldn't figure out why it just stopped until I realized that I had not added event numbers! It ran the first part perfectly without them.

I have also noticed differences in what the controller will digest between loading a part program into memory and running it, and drip feeding.

Any particular reason you use EasyDNC to drip feed since you also use CodeShark? I use CodeShark as well, and just drip feed directly from it after editing the program.

Nice work!!

[wildwhl]

No reason on the easydnc - except I had downloaded the demo previously. Didn't even consider loading from code shark but that makes total sense - one less step!

I have an awful long ways to go in this hobby, but have to say I'm starting to really enjoy the power and speed this mill has compared to my old x2 (understatement of the year?). Today I'll add a few tool changes to the mix. Going to mill out 30 pinewood derby trophies by Jan 15th for our scout pack. Should be a good bit of practice!