Second Time File Dives Deeper

[CA Glue]

Hello All, looking for any input.

Context - Laguna IQ 2x3, single vcarve file of text, Richauto A11 HHC

So I ran this file with the intention of running it twice, consecutively, on an oversized blank that would be cut down to size later.

First execution - perfect 0.1" depth 60° bit
flipped stock
Second execution - bit dove to 0.6" depth and it caused the X stepper driver to fail (confirmed by switching wiring internally).

I did not home between file executions. I did not go to origin between file executions.

Can someone please explain what is going on here? thanks

[FabLab Wageningen]

mmmm

'My' generated Gcode does include a 'go to origin' by default as far as I know. Only it does that at a safe Z-height.

The last 4 lines would be:
- G0 to Z safe height (to be seen in Toolpath Tab)
- M5 (spindle off)
- G0 to Z home height (to be seen in Toolpath Tab)
- G0 to X0.000 and Y0.000
What are your last lines ? Looks like something going wrong at the Z axis.
The Z height parameters on the Toolpaths tab look like screenprint attached.

Alternative: static or other interference. Always a headache.

Marcel.

[FabLab Wageningen]

As follow up on my earlier post:

When you started the job the second time, you also would have had a homing move, I realise.
Your first lines of Gcode should be comparable to this:

- T1 tool number 1
- G17 coordinates involved are X and Y respectively
- G21 units are mm (you might have a different value here (G20) if imperial)
- G90 coordinate modus is absolute (as opposed to relative (G91))
- G0Z20.000 move to Z home height
- G0X0.000Y0.000 move to X and Y home coordinates
- M3S18000 spindle on, 18.000 RPM (will be generated even if you set your spindle on manually)
- G0X0.001Y30.000Z6.350 move to the start X and Y coordinates of the CNC job, safe Z height
- G0Z1.001 move to just above the material surface
- G1Z-1.333F275.0 plunge in and go to work
then a lot of G1's or G2 / G3 if you are into circular things....

If this resembles your code, it is not a Vectric software issue, I fear.


Marcel

[CA Glue]

Correct, When I started the second operation, there was a homing move and it went to the correct position for x and y, and that is when the z went wonky.

Can you tell me how to generate the gcode, I have yet to find that.

Thanks for your responses.

[CA Glue]

Here is part of the gcode

(Filename: g code test)
N10M03S10000
N20G00X63.557Y49.426Z5.080
N30G1Z-4.745F558.8
N40G1X63.281Y49.515Z-4.452F1778.0
N50G1X63.140Y49.543Z-4.317
N60G1X62.815Y49.838Z-3.619
N70G1X62.774Y49.867Z-3.533
N80G1X62.957Y49.710Z-3.933
N90G1X63.140Y49.543Z-4.317
N100G1X62.760Y49.406Z-3.717
N110G1X62.432Y49.277Z-3.166
N120G1X62.760Y49.406Z-3.717
N130G1X63.140Y49.543Z-4.317
N140G1X63.281Y49.515Z-4.452
N150G1X63.557Y49.426Z-4.745
N160G1X63.499Y49.158Z-4.451
N170G1X63.437Y48.895Z-4.234
N180G1X63.403Y48.752Z-4.161
N190G1X63.346Y48.562Z-4.105
N200G1X63.250Y48.340Z-4.088
N210G1X62.799Y47.447Z-4.117
N220G1X61.601Y44.965Z-4.121
N230G1X61.393Y44.493Z-4.178
N240G1X61.242Y44.083Z-4.275
N250G1X61.118Y43.674Z-4.419

[FabLab Wageningen]

You have a different machine, so a different post-processor. I see no parameters for metric vs. imperial or absolute vs relative coordinates, so I have to guesstimate here. But what I read:


N10M03S10000 - spindle on, speed 10.000 RPM

N20G00X63.557Y49.426Z5.080 - non CNC working move (above material) to safe Z-height (is the value in the toolpath tab) interestingly, you set these as .2" (imperial) and the machine is receiving them in mm (metric).

N30G1Z-4.745F558.8 - straight line CNC work move; only to Z-coordinate, thus plunge into material, Feedrate 558.8 (units is mm. given this amount ?) NOTICE DEPTH: you are at -4.75 already... (this is mm, given the previous line command). Plunge runs at lower Feedrate than 'real' work moves (see Feedrate at next line command) which looks good to me.

N40G1X63.281Y49.515Z-4.452F1778.0 - straight line CNC move to X, Y and Z coordinate; Feedrate 1778.0 (I sincerely hope these are mm which is higher than plunge and number looks realistic NOTICE DEPTH: you are at 4.45.

N50G1X63.140Y49.543Z-4.317 - etc. depth again more than 4 mm

Looks like you use imperial units in your work, but the machine is values in metric (mm). That should work painlessly, though. But there is serious Gcode telling your machine to dive at least 4,7 mm. into the material., that's for sure.


Marcel.

[FabLab Wageningen]

I had a busy Friday and am at the point where I have a glass of decent wine(*) and I suddenly realise:

Can you post us the .CRV file ? Then we can check your settings and generate our own Gcode to see what happens.

I will NOT try to re-run your job. I do not want to put our CNC at risk. But comparing GCode might help a lot.

happy weekend,

Marcel.
(*) a 2018 Barolo - top of the range at my local supermarket - actually pretty good

[RickW3DS]

You get to drink wine in the middle of the day?
Wait, what time is it there?
Yes, a file would help.

[CA Glue]

Here is the file.

Thanks for your input. I am definitely learning something here about gcode.

This sign was made for a student who introduced me to "Duck Shit" tea. https://teapedia.org/en/Ya_Shi_Xiang

I think I would choose wine next time.

Thanks again

[FabLab Wageningen]

Thanks for the sign CRV, I'' see and investigate. Definitely not a 'relax' moment, then.

My dearest wife, an otherwise perfect woman, is hooked on oolong tea, as it happens. Me, I rather go for wine indeed, but never before driving or operating heavy machinery. And Rick can rest assured: I live in a different timezone indeed.

Marcel.

[Adrian]

I had a look at your file. With the start depth you have and the depth the actual v-carve is the depths your code is saying (nearly 5mm) is correct.

As the issue is only occurring the 2nd time you run a file that has run perfectly the 1st time that would indicate to me that the issue is outside of VCarve. I would try it again and make note of where the z physically is and where your control software says it is at at the start end of the 1st attempt.

[FabLab Wageningen]

There you have it: More confusion after Adrian's answer - which I actually support. But look at this:

I took the .CRV en re-did the toolpath, using a 60_degrees V-bit and - for safety's sake - a maximum cut depth of 8mm.

YOUR ORIGINAL TOOLPATH - DIVING DEEP
(VECTRIC POST REVISION)
(0CE8B0E204A506FA63017255C468991C)
T1
G17
G21
G90
G0Z20.320
G0X0.000Y0.000
M3S10000
G0X63.557Y49.426Z5.080
G1Z-4.745F558.8
G1X63.281Y49.515Z-4.452F1778.0
G1X63.140Y49.543Z-4.317
G1X62.815Y49.838Z-3.619

MY GENERATED TOOLPATH - LOOK AT THE DIFFERENCE IN Z:
(VECTRIC POST REVISION)
(0CE8B0E204A506FA63017255C468991C)
T1
G17
G21
G90
G0Z20.320
G0X0.000Y0.000
M3S18000
G0X63.557Y49.426Z5.080
G1Z-2.205F250.0 (my feedrate is questionably low - I have to check my parameters here)
G1X63.281Y49.515Z-1.912F1000.0
G1X63.140Y49.543Z-1.777
G1X62.815Y49.838Z-1.079

X and Y parameters look allright, proving we talk the same file at same coordinates indeed.

If your first try was a correct cut and the second too deep, it almost looks like you ran 2 different toolpaths ? Could that be ?

Marcel.

[CA Glue]

Hmmm.

I suppose nothing is impossible. I will have to go back and look through my files. I don't think that I ever would have created the deeper file, given it a near identical name, and put it on the usb for transfer but I may bee trying to do too many things at once.

As per Adrian's response, we seems to be having issues with the Laguna and some people seem to indicate electromagnetic interference may be causing the "ghost in the machine" incidences.. This is something I do not understand either.

Thanks for all your help.

Jim

[FabLab Wageningen]

Actually, that is much easier than you think.... I did it.

I opened your .CRV - obviously already including a toolpath. I created 'my own' toolpath and that was generated with almost exactly the same file name as your toolpath and then I exported both into the same directory. And than it's very easy to confuse the 2 submitting to the CNC.

Marcel.

[Adrian]

I took the .CRV en re-did the toolpath, using a 60_degrees V-bit and - for safety's sake - a maximum cut depth of 8mm.

When you redid the toolpath did you put the 0.1" start depth in for the v-carve toolpath? The depths your second snippet of code show are all 2.54mm out which equates to 0.1".