I was able to recreate this as well. that said, I am not sure that xyz probe is going to deep vs just x probe going to shallow. When I probed XYZ the bit cut the surface what I would say was approximately 0.0625" deep (fairly educated guess as I have been doing a ton of work at 0.0625"). When I probed just z (in the same corner of the touch plate in the same spot on the worksurface (offset by bit width so i could see if it cut) it was less than a paper thickness off the stock.
Now for the kicker and why I am thinking it is the inverse where x is not going to true 0. I measured my touch probe (with dial calipers) and realized that the configuration was set to 15.4mm when my probe in the circle corner is 15.2mm… low and behold that is 0.07". So when my touch probe thought it was 0.2mm thicker than it was, my z0 was below the surface about 0.2mm when probing XYZ. This does not explain the fact though that then when probing only Z I would now technically be 0.2mm above the surface after my adjustment.
Charley I have everything set up (probe on flat conductive surface) and I’m trying to run the code you provided in the MDI line but I’m not getting anything. The machine is not moving down and touching the plate as you said it would. Please advise.
So do you think it is a controller software issue?
charleyntexas
(Charley Thomas (Onefinity/Triquetra Touch Probe))
27
Try copying the following code and paste it into a TXT document (Windows Note Pad) Then load the file as though it were a carving file and run it.
TURN YOUR SPINDLE SWITCH OFF PRIOR TO RUNNING THE FILE
G21
G92 Z0
G38.2 Z-25 F25
G92 Z0
G91 G1 Z12 F700
M0 (MSG, Move the touch plate clear of the spindle but leave it in contact with the conductive surface then click continue)
G38.2 Z-50 F75
G91 G1 Z3.175 F50
G38.2 Z-50 F25
M0 (MSG, RECORD THE Z AXIS READING FROM THE DIGITIAL COORDINATE BOX. THIS IS IS YOUR TOUCH PLATE THICKNESS. CLICK CONTINUE TO EXIT)
M2
Quick update for @OnefinityCNC and anybody else following…I have tried the following with no luck in fixing my problem:
Rolling back the firmware to the previous one (Onefinity suggestion)
Resurfacing my waste board “with a bit in the router” (Onefinity suggestion)
Resetting XYZ setting in the controller settings (Onefinity suggestion)
Performed the probe fine-tuning again for XY & Z (With help from Charley)
I don’t know what else to do except wait for a solution with the next firmware update. It’s not a really big problem, however it is a little annoying. I still love the machine!
1 Like
charleyntexas
(Charley Thomas (Onefinity/Triquetra Touch Probe))
30
Just to confirm, Did your run the measuring gcode file with the gcode I posted to measure your touch plate thickness? If you did, did you update the thickness of your touch plate in the OneFinity controller software settings page?
If you answer yes to both questions do the following:
Create a new text file with Windows Note Pad and open it for editing.
Copy the contents of the below gcode into the text document
Change Line 5 in the code so that XX.XXX is replaced with the thickness of your touch plate as measured with the measuring gcode file from my previous post.
In the text document click the File/Save As menu
Look for the Encoding Drop Down Box . It should be near the Save Button. Change the drop down selection to ANSI then give the file a name and click save. Note: You do not need to change the default file extension from .txt to .gcode. It will run the same regardless of the extension.
Load the file just as though it were a carving file.
Turn off your spindle switch for safety
Position your bit over the target circle if you have a OneFinity touch plate or near the back right corder if you have a different touch plate.
Check to insure your wiring is all connected.
Run the file. Your machine should probe the Z axis and then lift up.
Remove your touch plate and ground wire before you click the OK button to continue.
When the file finishes your bit should be at Z 0
G21
G91
G92 Z0
G38.2 Z-50 F50
G92 ZXX.XXX
G91 G1 Z17.000 F700
M0 (MSG, REMOVE THE TOUCH PLATE AND MAGNETIC GROUND WIRE. CLICK OK TO CONTINUE)
G90 G1 Z0 F700
G91
M0 (MSG, YOU BIT SHOULD NOW BE LOCATED AT Z0. CLICK CONTINUE TO EXIT)
M2
If the code above results in your bit finishing at Z0 correctly but you still have an issue with the built in Z only zeroing function of the controller then please verify that the touch plate thickness has been correctly saved on the settings page of your controller touch plate measurements section. If the measurements saved are the same as you entered in the above code to replace the XX.XXX then I have to assume that the problem is with the controller coding.
We’ve identified a bug that was introduced with 1.0.6 Beta. Apparently, when the jerk is raised beyond a certain number (in this case up to 15000) it affects the z probe height. Reducing it back down to 1000 (but staying on 1.0.6 beta) will correct the z height. We’re working on a fix.
@OnefinityCNC , would this also apply to having multiple work coordinate offsets? When i have done that i noticed that each offset i needed to adjust my Z as well on the offset when my spoil board is flat\true.
I just ran a few XYZ probe tests with the jerk settings changed around and got the following results:
X-15k, Y-15k, Z-15k-----Z height was off
X-15k, Y-1k, Z-1k ------ Z height was good to go
X-1k, Y-15k, Z-1k--------Z height was off
X-1k, Y-1k, Z-15k -------Z height was good to go
X-5k, Y-5k, Z-5k----------Z height was off
X-1k, Y-1k, Z-1k----------Z was good to go
I’m going to keep all of my settings at 15k and continue to probe for Z after XYZ in order to keep my max jerk settings until the new update comes out hopefully soon.
(Onefinity suggestion)