MakerFr.com

Hello,

The CNC has been running great and I even made some clamps on it. To find zero on a part, I use an edge finder and it probes all axis.One problem I have is when an operation is done and I want to change tools, the machine doesn't remember what the zero position is after the operation is complete or if I cancel the operation. I use Fusion 360 to create different setups for each tool because the manual tool change command doesn't work. I've tried looking through the forum and other forums but I can't find a solution. I launch operations from an SD card.

Hello Albertotron,

I can't explain you the tool change procedure, because I still didn't try to use it. mstrens will be better to explain it.
I am not an expert in the domain, but I am pretty sure you can use your edge finder on condition that you define personalized X-probe, Y-probe and Z-probe command buttons. mstrens will confirm or not. Did you do it? In this case, please let us know the Gcode you programmed for these 3 buttons ?

See ya

Hello,

I do probe after the operation has been done but sometimes I can't do that because material has been removed and there is no square edge. Right now I'm cutting carbon fiber in water and I can't probe unless I remove water and that gets tedious. I have one command for probing XYZ axis and one for just the Z axis. I forgot to mention that the edge finder is a touch plate.

Here is the G-code for the edge finder:

G91 G21 ; (Relative position in mm.)
G38.2 Z-30 F100 ;(Search of the probe on 30 mm. speed 100, if not found after 30 mm. Alarm GRBL)
G0 Z1 ; (back 1mm.)
G38.2 Z-1 F10 ; (Searching the probe for 1 mm, slower, speed 10)
G92 Z3.85 ; (Adjustment of the Z offset according to the thickness of the probe, 20 mm in this case)
G0 Z3 ; (Up 3mm.)
G91 ; (Start of X probing)
G0 X-15
G0 Z-5
G38.2 X30 F100 ; (Search for probe)
G0 X-1 ; (Back 1mm)
G38.2 X1 F10 ; (Search for probe at slower speed)
G92 X-11.05 ; (Side thickness)
G0 X-3
G91 ; (Start of Y probing)
G0 Y-45
G0 X12
G38.2 Y50 F100
G0 Y-1
G38.2 Y1 F10
G92 Y-11.05
G0 Z3

The probe tools available in ESP32 (TFT) is foreseen only for the Z axis.
It is made in order to be used with a probe set on a fix position.
The principle is :
- to define once a Change tool position (= where the CNC must go to let you easily change the tool)
- to define once a Probe position = (where the CNC must go to start the probing= XY of the fix probe, Z not to high so that it is fast enough)

then when you want to mill with several tools, you apply the following process:
- you install the first tool
- you move to the origin of you piece and you set XYZ to 0 ; you can do it in the same way you do it currently using a mobile probe.
- once Set XYZ done, you select the calibrate menu. CNC should go to the fix probe position and perform a Z probe. The result of the probe does not change the Z offset already defined but the Z position is stored in memory (an will be use later)
- you can then mill with the first tool
- at the end, you can select Go Change in order to move to the Change position and change the tool.
- then you select Probe and the CNC will move over the fix probe, will perform a probe and adjust the Z offset in order to take care of the diffirence of height with the previous tool.
- you can now mill with the second tool having the same origin (in G54 offset)
You can repeat the 2 last steps for a third (4th...) tool if needed.

I was having trouble at first finding the calibrate button and it turns out I had a very old version of the software. I updated to the new one and I was able to find it. On startup I get an error about a CMD; can't remember the exact name but it doesn't seem to affect anything. Do I have to change anything in the code so that Z probe knows the thickness of the probe plate or does it remember it from the original XYZ probing? I'm assuming that executing the calibration sets the zero position of XY to where the probe position was originally set?

The calibration does not change any offsets. I t only perform a Z probe (over the fix probe position) and keep in memory the difference between the Z position of this probe and the Z offset(defined when you set the origin of the workpiece). This value, will only be used when you use the Tool button that perform a new Z probe (over the fix probe position) in order to calculate the new Z offset to apply in order to keep the same origin workpiece). So during the Tool, the XY offset are not changed.

The error that you get at power on can just be discarded. It is a kind of bug that I did not solved.

Just to make sure I understand and do everything correctly.

I'm going to:

-Set tool change position
-Probe XYZ with custom command
-Set probe position at origin
-Do operation and wait for it to finish
-Change tool
-Do calibration, not Z probe
-Set XY zero
-Start new operation with tool

Albertotron a écrit : 17 mai 2020 22:26 Just to make sure I understand and do everything correctly.

I'm going to:

-Set tool change position
-Probe XYZ with custom command
-Set probe position at origin
-Do operation and wait for it to finish
-Change tool
-Do calibration, not Z probe
-Set XY zero
-Start new operation with tool

No.
Please note that this tool is foreseen to use a probe at a fix position (and not at workpiece origine) to perform change tool.
You can also use a "mobile" probe to set up the origin of workpiece.
The sequence is:
- Home
- set tool change position
- set (fix) probe position

- define the origine of workpiece with a first tool (use set XYZ to 0 or use a mobile probe system.
- do calibration (cnc wil move over the fix probe and perform a probe but will not change offset)
-Do first operation and wait for it to finish
- go to Change tool & change tool
- execute "probe" (from menu tool); cnc will move to the fix probe, perform a probe and adjust Z offset
-Start new operation with tool

Hi im having the same issue, cant find the calibrate menu, do you have a link to latest software please.

Many thanks

Hi Craig81,

Craig81 a écrit : 18 mai 2020 23:33Hi im having the same issue, cant find the calibrate menu, do you have a link to latest software please.

https://github.com/mstrens

You will find there the last firmware of the ESP32 and the STM32. By the way, I still didn't received the touch screens. You can now follow their status of delivery here, column "Order status".

See ya.