Z diving problem?

[gilles_vigneron]

Hello, I was able to make my first cut this afternoon, I was pretty stressed!
There was a problem at the beginning, and I can’t find the solution. The M4.1’s first “action” was to dive in completely, then get up, then start the gcode instructions. I drew via F360, designed the toolpath on F360, and this first action clearly doesn’t seem to appear in the simulation… So, I guess I misset something on the M4.1, but I don’t know what. And, I confess, I don’t quite understand the z-stop’s z-home. I saw the video “how to set the z-stop on the M4,” and I can’t find a solution there. Can someone point me in the right direction? Thanks in advance

[ian_ab]

@gilles_vigneron

I don’t quite understand the z-stop’s z-home

Z stop is the value you set when the M4 is all the way down, i.e. Z lowered right down (no bit) Z-home is where the bit is just clearing the work surface, not quite cutting. When you are cutting the depth goes to minus values. Z-stop should have been set when you did your calibration. You can reset it by lowing the Z access all the way and setting it under the settings menu.
I set my Z-home by placing a metal plate under the M4 and connecting a multimeter, one side to the plate and the other to the bit in the router, then lowering the z until it makes contact, raising it resetting the Zstep to a lower value and lowering again, gradually creping down until I just make contact. then raise it 0.1 mm and set the z-home. I then raise it 4mm.

@gilles_vigneron

The M4.1’s first “action” was to dive in completely, then get up, then start the gcode instructions

Can you put a copy of your .nc code or .gcode here to have a look at.

[bar]

I believe that there is a known bug in Fusion 360 that is causing this, and someone posted a solution in the forums, but I forget what it is. Let me see if I can find it.

[bar]

Fusion360 and G28 G-Code

Hello friends Not sure if others have experienced this and I don’t haven’t tried too many other products but this might be an issue with how Maslow handles G Code so I’ll ask about it: Fusion 360 adds a line in the G Code each time I post process a bit like this: G28 G91 Z0 This a kill the panel instruction basically as it plunges the bit right into the sheet and then, with router all the way down, returns to home. If the machine is already at home it will drop the bit and leave it down whil…

First Cuts and Lessons Learned......so far

Finally finished enough “around the house” projects to build a frame and get my Maslow put together. I was able to overcome each issue encountered through the forum posts, so thank you to the community for all of it. Assembly and Calibration: Had to up the current limit a bit to get consistent full retraction. This was the first thing I learned in the forums and I wished I had looked sooner as I partially disassemble the unit looking for issues first. Was very frustrated with the overall expe…

I’m not a fusion user so I’m not an expert, but these sound like the same issue, right?

[ian_ab]

@bar

I’m not a fusion user so I’m not an expert

could it be this:

@jemmer798

So since I posted, and after reading @dlang 's mention of the Z commands, I looked into changing the default Post Processing settings. I changed the “Safe Retract Height” from the default (G53 I believe) to Clearance Height, and haven’t had any more issues thus far (>15 cuts all unique .nc files). The .nc files also have a bit of a disclaimer about the change: (-Attention- Property Safe Retracts is set to Clearance Height. Ensure the clearance height will clear the part and or fixtures. Raise the Z-axis to a safe height before starting the program.) I don’t now if this is the answer, but it has worked for me so far.

Also: From Supported Gcodes | Wiki.js

G28 Predefined Position

G28 is a machine coordinate location stored in non volatile memory. It will go to the same location regardless of the coordinate system or G92 offsets. You can view the current setting via the $# command.

• G28 This does a rapid move to the location.
• G28 axes If you specify axis values it will first do a rapid move to that location in your current work coordinate system. Then it will do a rapid to the stored G28 location. It will only move on axes specified.
  • G28 Z10 will move to work Z10 then move to the Z location stored in G28. No motion on X or Y.
  • G28 X10 Y20 will move to work X10 Y20 then to the G28 location for X and Y. There will be no motion on Z or any other axes you have defined.
  • G28 G91 X0 This is a way to move only to the X stored in G28. G91 X0 is a relative move of 0 so there will be no move before the G28 move. Again, only the X axis will move. Note: You will remain in G91 after the move. If you were in G90 before the move, you may want to send a G90 to return to that mode.
• G28.1 Use this to set the G28 offset to the current location in machine coordinates.

[gilles_vigneron]

Thanks for your explanations, they enlighten me. I need to do this z-stop setting… I’m adding the .nc, but reading @bar’s later posts, it seems likely (the symptoms match and the g28g91z0 line appears) that it’s the G28 G91 Z0 bug that is incriminated. I confess that, from afar, my reflex is to say to myself “what did I screw up again?!” rather than considering bugs.
1 cadre pied cornhole 5mm.nc (30.0 KB)

[gilles_vigneron]

@bar, thanks for the tip, I’ll study that!

[gilles_vigneron]

I’ve been poking around the sites in question. It appears that the @ian_ab solution generates a gcode for me where the cursed G28 G91 Z0 instruction no longer appears. I’ll test it later and come back with the result. Thanks again to those who took the time to point me in the right direction.