Machine is looking for probe after probing

@onefinitycnc @MyersWoodshop So after i worked through the setting XY zero problem, I then put my workpiece down and use the XYZ probe to find the corner and Z height. That worked great.

As soon as probing is done, the machine moves up and away slightly.

However, when i then run the program the first thing it does is say to connect the probe and then it plunges down to find the touch plate. Problem is, it moved away so when it plunges straight down it is beyond where the probe is on the corner.

I believe this is a function of the G90 code that is listed in the setting- g-code program start menu.

I deleted the G90 from my actual .ngc file but since it is defaulted in the program it still goes through them motion.

My question is, why is the machine looking for a second height check right after being probed and also, is there any issue with me deleting that G90 line from the settings menu?

Which program are you using for probing?

@onefinitycnc I generated the .nc file in Carbide Create. I am using the Onefinity branded probe I ordered with the machine. I just hit the probe XYZ button on the display. It goes through the probing cycle just fine. Then i hit the play button and the first thing it does is ask to connect the probe. it then does a Z height probing cycle, which is what the G90 code is telling it to do.

Can you upload the first few lines of code in your carving file. I suspect there is something it it that is causing your issue. If so it should be easy to remove and resolve your problem. It will most likely be in the first 20 lines of code.

1 Like

@charleyntexas Here is a snippet of the code.

(Design File: K:/XXXXXXX/Battlefield Woodworks/CNC/CNC Setup Projects/myers_woodshop_wasteboard_v3_ONEFINITY.c2d)
(stockMin:0.00mm, 0.00mm, -19.05mm)
(stockMax:819.15mm, 819.15mm, 0.00mm)
(STOCK/BLOCK,819.15, 819.15, 19.05,0.00, 0.00, 19.05)
G90
G21
(Move to safe Z to avoid workholding)
G53G0Z-5.000
(Large Holes For T Nut Bottom)
M05
(TOOL/MILL,6.35, 0.00, 0.00, 0.00)
M6T201
M03S20000
(PREPOSITION FOR RAPID PLUNGE)
G0X158.22Y761.56
Z10.00
G1Z-2.03F635.0
X158.14Y761.65F2540.0
X158.11Y761.71
X158.08Y761.77
X158.05Y761.87
X158.04Y762.01

I thought the G90 was causing the issue so i deleted it which left me with the below code

(Design File: K:/XXXXXXX/Battlefield Woodworks/CNC/CNC Setup Projects/myers_woodshop_wasteboard_v3_ONEFINITY.c2d)
(stockMin:0.00mm, 0.00mm, -19.05mm)
(stockMax:819.15mm, 819.15mm, 0.00mm)
(STOCK/BLOCK,819.15, 819.15, 19.05,0.00, 0.00, 19.05)
G21
(Move to safe Z to avoid workholding)
G53G0Z-5.000
(Large Holes For T Nut Bottom)
M05
(TOOL/MILL,6.35, 0.00, 0.00, 0.00)
M6T201
M03S20000
(PREPOSITION FOR RAPID PLUNGE)
G0X158.22Y761.56
Z10.00
G1Z-2.03F635.0
X158.14Y761.65F2540.0
X158.11Y761.71
X158.08Y761.77
X158.05Y761.87
X158.04Y762.01

BUT then the action still happened. That is when I noticed in the setup screen for the machine, there is a pre-programed ( i think) G90 code. My question was can i just delete that? But also, why is it doing it. When i generate a new g-code from from Carbide Create it includes that G90 code as the first move.

I appreciate all your help

which post processor are you choosing in carbide create?

Thanks for letting me look at the code snippet. I don’t see anything in it that would indicate that a probe is being called for. You probably should not remove that G90 though. It determines how the machine moves and removing it can definitely have a unpredictable results. Well there is one prediction, and that is you won’t get the finished product you were expecting.

I am not 100% sure but from what I have heard just now, it sounds like your post processor is what is automatically calling for the probe when you start a carving file. If you change to a different post processor then you can prevent that. I used a X Carve post processor file with Vetric Software to create a carving file and it does not call for a probe. You can still probe before you start the carve and your X Y Z zero location that is set during probing will remain as set.

I hope this helps.

@charleyntexas I used F360 and generated another G-code. I used the gbrl post processor in their library. When i open that file i am still seeing the lines of code. I haven’t tried to run this file yet to see what happens on the machine though. Here is a snippet of the code.

(1001)
(T2 D=0.25 CR=0 - ZMIN=-1.001 - flat end mill)
(T3 D=0.06 CR=0.03 - ZMIN=-0.8112 - ball end mill)
G90 G94
G17
G20
G28 G91 Z0
G90

(Face3)
T2 M6
S18000 M3
G54
G0 X18.025 Y0.371
Z0.6
Z0.2
G1 Z-0.09 F39.37
G18 G3 X18 Z-0.115 I-0.025 K0
G1 X0 F75

I would try to run it and see. If you still get the probe request when you run the file let me know and I will upload the X Carve post processor I use and you can try that. If you want to give me a call my cell phone number is 903-436-0675.

2 Likes

I just ran a test in Carbide Create.
If you save the gcode with default settings it will add the probing code ( G6 command) that will ask to probe before every toolpath.

You need to select either the basic gcode or grbl post processor in Carbide Create (these do not add the probing command of G6) by choosing edit at the top left, then select Post Processor. The default is set to ‘Shapeoko with limit switches’ which adds the probing code. Make sure to have the most updated Carbide Create. The post processor choices are a relatively new setting for Carbide.
I’ve attached a picture below.

This is one reason we uploaded TWO post processors for Vectric. One does NOT have the call for probing before each toolpath, the other (it says with probe) DOES have the call.

1 Like

@onefinitycnc

I downloaded 505, which is the newest, unreleased version. I set post processor as Basic. I turned on the machine, homed it, ran the XYZ zero. Then loaded the file and hit play. I got the below errors. (note i tried the GBRL post as well and got the same errors)

Level Source Location Repeat Message
debug API RequestHandler.py:63 1 Traceback (most recent call last): File “/usr/local/lib/python3.5/dist-packages/tornado/web.py”, line 1509, in _execute result = method(*self.path_args, **self.path_kwargs) File “/usr/local/lib/python3.5/dist-packages/bbctrl-1.0.2-py3.5.egg/bbctrl/APIHandler.py”, line 46, in put self.put_ok(*args, **kwargs) File “/usr/local/lib/python3.5/dist-packages/bbctrl-1.0.2-py3.5.egg/bbctrl/Web.py”, line 342, in put_ok def put_ok(self): self.get_ctrl().mach.start() File “/usr/local/lib/python3.5/dist-packages/bbctrl-1.0.2-py3.5.egg/bbctrl/Mach.py”, line 295, in start self._begin_cycle(‘running’) File “/usr/local/lib/python3.5/dist-packages/bbctrl-1.0.2-py3.5.egg/bbctrl/Mach.py”, line 118, in _begin_cycle (cycle, current)) Exception: Cannot enter running cycle while in mdi cycle

|error|API|RequestHandler.py:61|1|Cannot enter running cycle while in mdi cycle|

send the file to support@onefinitycnc.com and we’ll take a look.

Ok, sent the file. Thanks for taking a look

1 Like

It opened on my machine flawlessly. I suspect something is running or loaded in the MDI tab on your controller.

Ah, the old “it works fine on my machine” routine :wink:

Man, I don’t envy you guys - with more and more machines in the wild, a dedicated teams of help desk professional is warranted.

But, once I have my machine (<- hint), I’ll be happy to help.

-Tom

1 Like

Our staff continued this support via email. A reboot of the controller cleared the code and worked.

5 Likes

@cyberreefguru

I should have come back and closed this thread out. I emailed the test file and we worked through it together to find a solution. It did turn out that deleting and re-adding the files after a power cycle fixed the weird error I was getting.

Onefinity support is top notch. Im sure they had better things to do on a Saturday than help me troubleshoot my file. But none the less, there they were bright and early helping me out.

4 Likes

@cyberreefguru It’s great you found the solution, and thanks for adding a bit more detail. If you had this issue, I bet someone else may at some point and having the solution listed here for future reference is helpful!

1 Like

Will there be 2 post processors for fusion 360 like for vectric? The current buildbotics post processor does the secondary (most of the time unnecessary) z probe.