In my tool change script I have an M00 command with a short instruction, followed by another M00 command with another message. Basically, two steps in the tool change process, the first message telling me which bit to install, and the second telling me that the Z-axis homing is about to start.
I find that the first message flashes by and the run pauses at the second message only.
My understanding is that M00 is an unconditional stop, and that I should have to press the main button to move past the message.
My code looks like this:
M00 Chg to Click when changed
M00 Home the Z-axis first
Am I doing something wrong?
Tech: MPCNC Primo with Rambo 1.4 board and āFull Graphic Smart Controller, bigā. Fusion360 with Estlcam to generate the gcode.
Strange. Your understanding matches mine, and I just copied and pasted your two lines into a file and ran it off the SD card, and the MPCNC stopped at both lines. Maybe you can attach the g-code file that is messing up to this topic so we could take a look. Maybe there is a non-printing character in the line or some other issue.
Hereās my start up code. I added the M400ās today to see if it made a difference, but it still reacts the same. āConsole2 4 v6 - frontā is the name of the gcode file (for where you see that in the code).
So I get a pause on the first message: āConsole2 4 v6 - front Click to startā
It briefly shows āChg to S1R 1/8" 2 flute 24000 Click when changedā
And then it pauses on āHome the Z-axis firstā.
It skips the pause for the second message.
Any help is appreciated.
G90
M00 Console2 4 v6 - front Click to start
M107 P2 ; Stop spindle
M400 ; wait for move to finish
G00 Z40 F500 ; Raise Z probe off of surface
M400 ; wait for move to finish
M00 Chg to S1R 1/8" 2 flute 24000 Click when changed
M400 ; wait for move to finish
M00 Home the Z-axis first
G28 Z ; Home in order, w/zprobe
G92 Z0.5 ; Account for probe thickness (set your thickness)
G00 Z5.0000 F500 ; Raise Z probe off off of surface
I donāt know what is going on. Brainstorming I see possible sources: something in the g-code generation is inserting non-printing characters that is confusing Marlin, a bug in Marlin, a bug or issue in the g-code sender, or a minor hardware issue. So gather a bit of info:
What program are you using to generate your g-code?
What program are you using to send your g-code to the control board?
If you are using a g-code sender like Repetier-Host, does the problem occur if you run that same program from the SD card.?
What version of the Marlin firmware are you running?
Please attach the exact file that is causing the problem. You can use the upload button:
There is one thing you can try. Put some g-code command(s) that take a bit of time just before the M00 that is failing. Maybe something like this:
G00 Z65 F100
G00 Z40 F100
If this āsolvesā the problem, there the issue is most likely Marlin or the rotary encoder button on your display. Iām running Marlin 509D on a Rambo 1.4 board like yours, and I tested multiple M00 commands yesterday in response to your question. I did not have an issue.
Edit: I just copy and pasted your code above, put it on an SD card and ran it off the SD card. The machine stopped at all the M00 commands.
I removed the " from the bit name in Estlcam, but never thought to remove the /. Iāll try that tomorrow.
Hereās the code generated by Estlcam for a really simple piece. The tool change code is defaulted in at the beginning of the fileā¦
As I said in the original post: Tech: MPCNC Primo with Rambo 1.4 board and āFull Graphic Smart Controller, bigā. Fusion360 with Estlcam to generate the gcode.
Additional info: running straight off SD card. The Marlin version is whatever V1 shipped, 509D sounds right ā I can check that tomorrow as well.
As another thought: The M00 command has a [P] and an [S] parameter. Is there any chance that Marlin is seeing the bit name (āS1R blah blah blahā) and interpretting the S1 as a one second time out on the pause???
I took a look, and there is no non-printing characters besides in the M00 areas of the file, so we can rule that possibility out. I like Darrellās idea.
So the answer is the āS1Rā in the prompt string of the M00 command.
Since S is āexpire time in secondsā, it was expiring the message in one second and moving on.
Once I changed the string from S1R to SIR, everything works correctly.
Something new to consider when creating prompt strings. Lol.
Robert - my Marlin pops up as 509 on the splash screen. No āDā at the end. I wonder if you have a slightly newer version? I got mine from the V1 site, so I assumed it was flashed with the most current firmware.
