UCCNC manual tool change

In the macros there is two forms of asking the coordinates, one gives you the current position relative to zeroed location, other gives you the current coordinates in the machine space:

See the UCCNCDocumentationMacro_capability_detailed.htm file:

 Function: double Get[XYZABC]machpos(void)
Description: The function returns the actual machine position of an axis, this is the abosulte position excluding any offsets.
Example: double Xmachposvariable = exec.GetXmachpos();
Notes: [XYZABC] means a character of X, Y, Z, A, B or C
 
Function: double Get[XYZABC]pos(void)
Description: The function returns the actual position of an axis including the selected offset and the tool offset.
Example: double Xposvariable = exec.GetXpos();
Notes: [XYZABC] means a character of X, Y, Z, A, B or C

Also in the Gcode there is several ways to move the head, i.e. if you add G53 to move command then it moves to absolute machine coordinates instead of zeroed coordinates.

This is explained in the page 43 on the UCCNC_usersmanual.pdf found in the same directory. If you use following command

  exec.Code("G00 G53 Z"+ parkZ); 

where the parkZ is the height you want to move in absolute machine coordinates the head will move up to that location. You might want to add check that it will never move down, i.e. write the code like this:

if (exec.GetZmachpos() < parkZ) {
  exec.Code("G00 G53 Z"+ parkZ); // Move Z up first to park Z position
  while(exec.IsMoving()){}
  exec.Wait(200);
}

In this case it will only move head if it moves up. It will not move the head at all, if your parkZ is lower than what the current head position is.

You might also want to check that softlimits of when doing those operations. To get softlimits you can use following code:

double XMin = exec.mainform.UCsetup.UCset.Axis[0].UC100axis.SoftLimitN;
double XMax = exec.mainform.UCsetup.UCset.Axis[0].UC100axis.SoftLimitP;
double YMin = exec.mainform.UCsetup.UCset.Axis[1].UC100axis.SoftLimitN;
double YMax = exec.mainform.UCsetup.UCset.Axis[1].UC100axis.SoftLimitP;

This would allow you to move the head closer to you before starting to do work, but only if it is not too close to the edge already.

I was planning to do the tool change macros myself too, but I have not had time to do it yet, and it I remember right it was hard to get the UCCNC to both run the M6 macro and pause operations. Perhaps the M6 macro can press the cyclestop button to pause the g-code run to allow the tool to be changed, and or something.

I think it's easier to avoid changing your tools while inside a routine.

Just save the toolpaths that use a single tool in one file and toolpaths that use another tool in other file.

I had trouble with that on wincnc as exporting different paths from the same setup as different jobs made the seconds assume different zeros.
In other previous experiences with different machines with no automatic tool changer I done it like that and it was ok.
Fusion360CAM and Winpcnc was not good.
I'm trying the same technique with Unccnc right now.
any trick to take into account?
thanks in advance.