I'm back. It was a good idea to test it first...
I have good and bad news. The good news is that you can do the whole job with the probe screen. The bad news is that you first need to update to 1.2113, because Manual probe mode was not implemented in 1.2111.
Setup: you have to do it once. Home the machine first!
On the Probe / Setup page
Set Safe Z just below the Z home position in machine coordinates. The machine will move in this height.
Check Greater Z is safer in G17.
Check Save mobile probe pos. on exit.
Check Override probe dia. and set the diameter of your edge finder.
For the first tests check Limit traverse speed and set feed rate. It will slow down the quick movements. When all works fine, you can uncheck this.
Check Separate settings per mode.
On Probe / Page 1
Select Probe tool.
Select Mobile probe.
Move your machine above the tool probe, high enough for the longest tool.
Press Set as mobile probe pos and confirm with Start probing.
Set P1 to a negative value which is enough for the shortest tool to reach the probe. (Z will probe in negative.)
Turn on Zero probed axes.
Set Fine distance. (1 mm or equivalent in inches.)
Set Fast feed and Fine feed. (100-200 and 25 in mm/min.)
On Probe / Page 2
Select outer corner.
Select the corner you want to probe.
Select X and Y for Axis 1 and 2.
Set P1 and P2 distance as positive number (see the drawing on the button).
Turn on Zero probed axes.
Set Fine distance.
Set Fast feed and Fine feed.
Turn on Axis 1 count dia. and Axis 2 count dia.
Turn on Manual probe mode. You will probe the edges manually.
Exit UCCNC and
after UCCNC closed open your profile with a text editor. (E.g. Notepad, but not Word.) Find the following line (the numbers will not be the same):
- Code: Select all
MobileProbePos=True,0,True,15,True,190,True,-25,False,0,False,0,False,0,-39.7,True,7.236
Change the 3rd True to False. This will tell the probe screen to move only in X and Z to the probe. You are ready with the setup.
Use these steps after you homed the machine
Workpiece setup
Select Outer corner.
Move the edge finder to the corner of the workpiece.
Press Start probing: the edge finder will move to the first side of the workpiece then informs you to touch the workpiece. If you touced press Start probing to continue. The edge finder will retract and return to the start position. Then the same will happen on the other side of the corner. X and Y will be zeroed to the corner counting with the diameter of the edge finder.
Insert the tool which you need for the job.
Select Probe tool.
Touch the workpiece with the tool in Z then press Reference current as workpiece. The machine will go to probe the tool and save the offset for later use. (The machine will not move in Y, only X and Z.)
Start the job.
When you change to the next tool
Just press Start probing (Probe tool is still selected!). The tool will be measured and Z will be set.
Start the job.