What do you mean you “set machine coordinates”? The only thing that changes machine coordinates is homing or restarting the controller?
You set the work coordinate offsets. What specifically did you do to do that?
I home the machine
Goto G90 x4 y17 z-25
I then set G10 L2 P1 X7 Y20 Z-22 (Machine Location for corner of table)
Home and zero
goto G90 X450
Set G10 L2 P2 X453 Y3 Z3 (Machine Location for Tool change)
Home and zero
goto G90 X596 Y281 Z-14
Set G10 L2 P3 X599 Y284 Z-21 (Machine Location for current work location)
All are set….
You’re losing me here.
Are you doing all that from G54?
I assume your offsets for G54 and G55 are always the same but G56 changes?
Why are you jogging to a location in between? Also, not sure why you need to home and zero multiple times.
What’s the significance of the 3mm offset?
No
G54 Is the corner of the table
G55 Is for tool changes
G56 is the current work location
None of the locations are the same….
3mm offset is the offset from the Zero switches….
Maybe I do not understand what your asking but I know the machine locations are correct. I do not understand why some or all of them get reset even thou I did not run a cutting gcode… Just moving around and Homing.
Because the Post Processor will not put the locations from Fusion into the gcode and I want to Zero the work at G54 (table height), when done have it to to G56 to run the job, when finished, go to G55 for a tool change.
Here is the literal meaning and function of each part of the command:
G10 — The “Data Setting” Command
By itself, G10 tells the controller: “Stop moving the motors. We are not cutting right now. Instead, open up the internal settings registry because I am about to change a saved configuration value.”
L2 — The “Work Coordinate System” Mode
The L parameter tells the controller which setting registry you want to open.
-
L2specifically unlocks the Work Coordinate System (WCS) Offset Table. -
It tells FluidNC that you want to calculate and save a physical distance offset between the machine’s absolute home switches and your workpiece zero point.
P1 — The “G54” Target Slot
Your controller has multiple coordinate storage slots so you can save different fixtures. The P number chooses the exact slot you want to modify:
-
P1= G54 (Default Workspace Slot 1) -
P2= G55 (Workspace Slot 2) -
P3= G56 (Workspace Slot 3) -
…up to
P6(G59)
When you type G10 L2 P1 X4.0 Y17.0 Z-25.0, you are saying to FluidNC:
“Hey controller (G10), open up the coordinate offset memory table (L2), and modify the G54 workspace slot (P1). Look at where the spindle is physically standing right now, and calculate the math so that this exact spot is registered as X = 4.0, Y = 17.0, and Z = -25.0.”
The goal is to be able to have 3 or for work piece locations so as to make multiple of the same part.
Home from the table corner (G54)
Move to the first part (g56), then the second (G57) and then the third (G58)
Once done, move to G55 for the tool change, and start the process over.
As it stands right now, I cannot keep the locations set on the esp.
When I setup the G54 offset for my pen plotter, where I want G54 0,0,0 to be G53 90,0,0, I used this:
G90 G53 X90 Y0 Z0
G54
G10 L20 P0 X0 Y0 Z0
Alternatively, I could have used this. G54 is default but I’m being explicit since I’m using P0.
G54
G10 L2 P0 X90 Y0 Z0
Or I could have used P1 so it’s explicitly saying make G54 0,0,0 = G53 90,0,0
G10 L2 P1 X0 Y0 Z0
I’ve never had to reset that. It’s currently on FluidNC v4.0.2.
There is no 4.0.4 yet. Did you build the latest from source?
Sorry, fat finger… 4.0.X what ever the latest is….
I would double check but the machine is in the middle of a cut.
I have been setting them according to the documentation and I have been adding the G5X and G0 X0 Y0 Z0 into my gcode. Problem is sometimes it goes to the location, other times not because the esp as lost the settings.
Sorry, I meant that those individual positions never change. So, G54 is always the same position. G55 is always the same (but different from G55). And G56, since that’s based on your workpiece, that will differ between jobs.
I’m not sure what’s going on but if you’re using the Home and Zero buttons in the WebUI, that is going to reset the offsets for the current coordinate system.
Sorry but I do not understand….
If G10 L2 Px is to set the locations in the eprom, then they should not be re-written or reset just moving around the workspace…
The documentation indicates the eprom on the esp is a Non-volatile location.
Try homing your CNC. Don’t zero XYZ. Then set your G54, G55, G56 offsets.
Turn off the power to the Jackpot.
Power back up and home the machine. Don’t zero XYZ. Move around and then go to G54, G55, G56. They should all be saved. I think you are resetting them over and over by zeroing your XYZ AFTER you set your offsets in G54, G55, and G56.
I hope this solves the problem.
@Britt Thank You!!
So far this morning I have 4 set for the locations I wanted. After setting and verifying, I power cycled the CNC.
I have been randomly going from one G5x to another with No Issues! Thank you and will report back after doing some cuts I need to complete.
That’s great news @breese! I’m glad it’s working. Looking forward to see what you are making with it.
