First time setting up post processor for Laguna CNC router/software exceed limit error message

[Vintagetunes]

Hi there!

I'm trying to set up fusion to run our Laguna SmartShop SUV for the first time. (I've been using vCarve on this machine for a couple months now.  I selected the Laguna post, then edited it to output the .nc extension instead of .prg, and I'm getting two error messages when I run the program.  

"Motion 17    Zaxis First Positive software limit exceed"

"Coordinate  40     TheNcProgramL21: exceed software limit"

I'm not even 100% certain that it has anything to do with the post processor, but this is the first time I've seen these error messages.

Any ideas would be super helpful! 

Thank y'all!

[seth.madore]

Could you share any code from V-Carve that you've run on your machine? I'm curious to see how much the output differs between the two files (Fusion vs V-Carve)

[Vintagetunes]

Sure!  Here's a 2D cutfile we made in vCarve.  Thanks so much for taking a look!  We're searching hard for a solution

[seth.madore]

Sorry for the delay in response, it's been quite busy..

When does this error occur, right off the bat, or relatively later in the program?

There are substantial differences between the beginning lines of code in the two programs, and my suspicion lies there. 

V-Carve:

N6 G00 G17 G71 G40 G49 G80 G90
N7 G54
N8 G53 Z0
N9 (Tool: 3/16 alm deco)
N10 T8 M06
N11 M03 S20000
N12 G43 H8 Z50.8000
N13 G00 X70.9667 Y56.3119 Z38.1000

Now, the code above is pretty darn close to what I would expect to see for a standard g-code based machine. Let's break it down a bit:

G00 G17 G71 G40 G49 G80 G90  these codes set the "safe" G values;

(G0) rapid,

(G17) workplane

(G71) Metric, (this isn't a standard milling g-code, so it's likely Laguna specific)

(G40) cancel cutter comp,

(G49) cancel tool length offset,

(G80) canned drill cycle cancel,

(G90) absolute position

Then it's followed by a G54, this sets the current work coordinate system (This is defined in the Setup, and you can have G54, G55, G56 etc etc)

G53 Z0, this sends the tool home in the Z, this is likely the top travel of your Z axis

T8 M06, this is your tool change

M03 S20000, this is spindle forward, rpm of 20000

G43 H8 Z50.8000

G00 X70.9667 etc etc, this is your first move to the part.

So, the above code is everything your V-carve post is giving you in the beginning of the toolpath. Now, let's contrast that with what the Fusion post is giving us:

N12 G17 G40 G90
N13 G70
N14 D0
N15 G00 Z0.

(2D CONTOUR2)
N16 G53
N17 G00 X0. M05
N18 G53
N19 G00 Y0.
N20 T4 M06
N21 G54
N22 M03 S18000
N23 G04 5
N24 G00 X13.1078 Y8.4547

G17 G40 G90, some of the same "safe" codes, but many are missing

G70 (this is like the G71, but G70 is Imperial for this machine)

D0 (I'm guessing this is supposed to cancel tool length, can you confirm that this is supported?)

G00 Z0, this is a rapid move to Z zero, but it's possible that your machine doesn't like this

G53, this is a machine coordinate system selection, but with no axis specified in this line, nothing should happen

G00 X0. M05, since the above G53 is "modal" (stays on until cancelled or RESET), the machine should now proceed to X zero (M05 is spindle off)

G53 (same as above)

G00 Y0 (now the Y axis should move home)

T4 M06 (tool change)

G54 (same as v-carve program)

M03 S18000 (same as v-carve)

G04 5, I'm guessing this is a dwell code?

G00 X13.1078 etc, this is the first move

So, as you can see there's substantial difference.

If I was to guess, I'd want to gut out the beginning of the Fusion posted code and replace this:

N12 G17 G40 G90
N13 G70
N14 D0
N15 G00 Z0.

(2D CONTOUR2)
N16 G53
N17 G00 X0. M05
N18 G53
N19 G00 Y0.
N20 T4 M06
N21 G54
N22 M03 S18000
N23 G04 5

With this:

N6 G00 G17 G70 G40 G49 G80 G90
N7 G54
N8 G53 Z0
N9 (Amana Tool 46415)
N10 T4 M06
N11 M03 S18000
N12 G43 H4 Z1.71

HOWEVER!

One thing I'd really like to confirm is this: there are machines that only use Metric code, is your machine one of them? Your Fusion file is in Imperial, but your V-carve is in Metric

[Vintagetunes]

Thank you SO MUCH for this info!  I'm super new to reading Gcode, but it's making some sense.  I'm going to start digging in to answer all the questions that I can, but one that I can answer(sort of) from the start is about this machine being metric.  The displays on the machine are all metric, but I wasn't sure if my working in imperial inside Fusion would matter or not.  Our vCarve workspace is setup in imperial, but I'm assuming now that it must be setup to output metric.  Would changing the units in the Fusion workspace to metric before posting also change the units in the Gcode?

I'll reply with answers to the other questions soon.  Thanks so much again! It feels like I'm starting to see a tiny light at the end of the tunnel 😅

[Vintagetunes]

To hopefully answer the other questions:

The error occurs near the beginning of the program.  It will perform the tool change, then move x and y to the corner of the stock, move the z axis all the way to the top, then *error*.

Your question about the G00 Z0 seems very plausible to me, as that's when the error occurs.

As far as D0 being supported, I'm not sure.  I'm assuming that's some information that I'd have to find about the controller, but I've had trouble finding any in-depth manuals for Syntec.  I'll continue searching for more info on that.

I'm also not sure on the G04.  My searches show that it's probably a dwell code, but I'm not educated on this enough to know if that's always the case.

Yet again, this is all super appreciated!

[seth.madore]

To be on the safe side, I would set your post processor preferences to post out in MM, which is is handled here:

 

So, I would post out your code again with MM, and then let's start modifying the code to see what can get it to work on your machine. I think it's just the G0Z0 that's doing it, so you can turn that into a G0 G53 Z0 instead

[Vintagetunes]

Hmmmm... Still getting the same errors with the changes.   I made a smaller test part to run today, and it seems to be hanging at N26.  Would that be a clue?

N10 (Program name: 214231)
N11 (Program comment: )
(T3 D=3.175 CR=1.587 - ZMIN=10.775 - BALL END MILL)
(T4 D=6.35 CR=0. - ZMIN=16.002 - FLAT END MILL)
N12 G17 G40 G90
N13 G71
N14 D0
N15 G0 G53 Z0.

(POCKET1)
N16 G53
N17 G00 X0. M05
N18 G53
N19 G00 Y0.
N20 T4 M06
N21 D4
N22 G54
N23 M03 S18000
N24 G04 5
N25 G00 X231.825 Y105.016
N26 G00 Z43.179

I included the whole file if that helps.

[Vintagetunes]

I actually just realized that Z43.179 is definitely past the soft limit, and if I try to jog to a positive integer, it stops me within about 3-4mm. Is there a possibility that my Z coordinates are inverted?

Update:

I've also just noticed that in the POCKET1 operation, the Z axis is stepping down toward zero(Z31.xx,Z30.xx,Z29xx, etc.), which isn't exactly inverted.  I'm not sure if that's the right path to be looking down, but it does seem curious.

[seth.madore]

43mm is only 1.692", surely your machine has much more travel than that, no?

[Vintagetunes]

Oh yes. We have about 10 or so inches of Z travel. It does say that I've exceeded the limit if I jog further than a few mm positive (up on this machine.. I'm not sure if that's always the case). I'm not exactly sure why it would be trying to make that move up after being at zero already.

[seth.madore]

In this most recent example, could you share your Fusion file?

[seth.madore]

And that's because you've set the WCS zero to the bottom of the part, is this what you intended?

 

[Vintagetunes]

Sure!  Here's the updated version.  The smaller Test is placed in the scrap portion of the original model

[seth.madore]

Oh, I'm sorry. The Fusion file that you used to produce the code you showed above. What you sent me is still your original file (or so it appears):

 

[Vintagetunes]

Dang... I'm sorry. That was absolutely meant the be set at the top of the part. Looks like I got in a hurry 

[seth.madore]

Well, hopefully that solves it..

[Vintagetunes]

Sadly, I've still got the same error message with these files.  I had some trouble saving my updated file, so I had to recreate the test.  Here's the latest version for each.

Sorry, It's been a busy day in the shop here.  My WCS is zeroed at the machine bed

[seth.madore · Accepted solution]

---

@Vintagetunes wrote:

..but I've had trouble finding any in-depth manuals for Syntec.  

---

Houston, I think we've found the problem.

We've been chasing the problem with the Laguna post processor. Here you mention Syntec. We actually have a Syntec post and the code it produces is this:

%
O1001
(T5 D=6.35 CR=3.175 - ZMIN=76.2 - BALL END MILL)
N10 G90 G94 G17 G49 G40 G80
N15 G71
N20 G28 G91 Z0.
N25 G90

(2D CONTOUR1)
N30 T5 M06
N35 S5000 M03
N40 G54
N45 G00 X-4.065 Y620.508
N50 G43 Z91.44 H05
N55 M08
N60 G00 Z81.28
N65 G01 Z77.2 F1693.
N70 Z76.2
N75 X-3.43 Y620.507 F5080.
N80 G03 X-2.794 Y621.141 I0.001 J0.635

Pretty darn close to what your V-Carve is giving you...

I've linked the post above, give that one a try. There may be some changes needed (it looks like the XY is going home when the job is complete)

[Vintagetunes]

SUCCESS!!!🙌🙌🙌

It worked!!  The only thing I had to change was "Preload Tool".

Thank you SO MUCH for helping me sort this out!  You've been a lifesaver!

Now for the larger test cut!😎