I run the program, get to the change, change bits and continue, the tool probes down and touch the plate and picks up, remove the plate hit continue and the machine is cutting in the air pretty much at tool plate height. My probe plate is 15mm thick and it’s set correctly in the fluidnc dashboard, it works correctly for the 1st cut but not after the tool change.
I assumed the p0.5 was telling the machine that the plate was .5mm as that was the default when I first activated the probe tab. But setting that to 15 tries to drive the tool through the bed.
This is the copy/paste from the ecam as is. Changing the .5 to 15 is whare I first did when it was cutting air but it just drives the tool straight down into the touch plate and holds firm so no cutting is an option. The touch plate is pinned to the bed by the tool.
I’m using the probe button on the fluidnc dashboard, I don’t use the in gcode script.
So you get a successful probe with the +10 lift off when the 0.5 mm is listed, but don’t get a successful probe when the plate thickness is changed to 15?
The code you posted here still seems to be the code before editing. Can you post the edited code?
Any chance the wiring connection for the probe is not solid? Intermittent?
Hmm. Well, the P15 looks right. I mean you don’t have a minus in front of the 15 or anything.
Next up is, the target distance of -80.
In your config.yaml file…
Do you have “max_travel_mm” (or however its spelled) inputed for Z? If so, do you have soft_limit (or however its spelled) enabled for Z?
If so…
That would likely mean: this is a LowRider, with the regular YZ plate, not the “Dan’s Extra Tall YZ plate” version, and … this part is key … it would mean your Z needs to be all the way up before attempting a probe operation, or else your script is calling for a target distance lower than your max travel would allow.
When you try the probe after tool change, do you get any alarm or warning messages in the Command area (feedback/info box)?
Does it work if you type this in directly in the terminal?
I had mine act this way like 50% of the time, but worked out that the wiring was loose at the end of the probe
That’s a max distance. The Z doesn’t need to be all the way up, that’s just the max it will travel before erroring out if it doesn’t read the probe signal before then.
For all of us less experienced, let me explain…
because I had to read Dan’s post 5 times before I figured out what he was getting at lol
(This is not a criticism of Dan, but of my reading comprehension with things I’m not super familiar reading)
So he can correct me if I tag this wrong
M63 P1 ( turn off pin 27)
G91 ( -- set Relative distance mode)
G0 Z10 ( -- move 10mm in +Z direction)
G90 ( -- set Absolute distance mode)
G0 X0 Y10 F2520
M0 (MSG change tool, probe)
G38.2 Z-80 F200 P0.5 ( Probe set thickness)
G00 Z10.0000 F500 ( --- still in absolute mode, move to Z10, -5mm from top of 15mm thick probe)
M0 (MSG remove probe)
M62 P1 ( turn on pin27 )
There’s no good way to Bold something in preformatted text mode, but he was pointing out the need to change the Clearance line to this
Which I kept misunderstanding because I didn’t notice the difference between his and Nathans
I was mistaking his machine for being a LowRider, based solely on the 80. I was explaining that, if it’s a LR3, and if it’s got regular size YZ plates, and if he has max travel inputted and soft limits enabled, the probe target distance cannot be more than the available travel.
Based on the video, it’s MPCNC, not LR3, and all the above become moot.
The problem was that he set the probe height to 15mm then because it was in absolute mode, telling it to go to Z10 was basically telling it to dive another 5mm.
It gets your #1. It throws an alarm and won’t attempt the probe operation.
Why jogging to the top helps (when max travel is set and soft limits are enabled):
If your max travel is 80, and you tell it to probe -80, you can accomplish that if you start the probe while you are the top, because the firmware first asks, “do we have an available 80 to down within the max travel?” and the answer is “yes.” But if you are down a few mm’s into your available max travel, then the 80 would require going further down than you have available to go. It would alarm.
Why MPCNC likely different: My understanding (I could be wrong) is that MPCNC does not have Z end stop. If I am wrong on that, then there would be no difference between it and LR3.
Z end stop, though, only matters for homing, correct? So I don’t think it matters for probing.
As far as jogging up, I guess I could see this scenario if the probe operation errors out instead of just stopping motion:
Lets say you have soft limits enabled and you can’t travel beyond -20 to 80 mm.
If you were current sitting at Z20, you would only have -40mm available to travel, so I can see that moving to the top would help in that scenario, but I’m honestly not sure what a proper soft limit on Z should look like, and whether that’s a likely scenario that would get hit often.
If so, I guess I would be unlikely to enable soft limits on Z and have to worry about making sure I start at a certain point, or making sure my tool change scripts don’t error out in the middle of a job
