i am trying to understand the principals of tool manual changing (using vcarve desktop). my cnc is a generic, using fanuc inch (*.tap) post processor. mach 4 is installed.

for instance, if i want to use a roughing tool and a finishing tool:

1) is it better to save the two toolpaths to a different file or together? why?
2) if i save together, when the roughing is finished, does the spindle pull away from the surface and wait for the tool to be changed? or does it reposition itself to the original home? if not, can i jog to a more convenient place to change the tool?
3) once the tool is changed, how does the spindle know EXACTLY where to go to start the finishing?
4) do i have to zero the xy axis after every tool change? if so, how do i zero it to the EXACT same place as was used for the first tool?

lumberjacques

in mach4 ,for all that question, you will write the answer(the answer are writen by lua in m6 in yours case or any other m function that you can imagine

1. This is a matter of personal choice. I generally save different operations in different files for version control reasons, but there is no compelling mechanical difference between the two;

2. Only if you tell it to. Depending on your CAM package, it may issue a G28 or G30 to go home or to a pre-defined "tool change" point, or you can (depending on your CAM package) tell it to go to a specific position on a per-toolpath basis. On my XCarve (which uses GRBL, not Mach) I have a point defined at the centre front of the machine as the "tool change" point, and another one at the centre back as the "cleanup" point., where on the lathe, I tend to use a per-toolpath safe point. Note that it is on you to make sure you set up the toolpath constraints so you avoid fixtures if you use this functionality;

3. Assuming you haven't changed the workpiece zero point, all the CAM calculations are done to this zero. On mills/routers, it is common for the Z zero to change with toolchanges, but the X and Y zeroes will stay the same, so everything lines up; and

4. No - in fact, you shouldn't - but assuming the fixture touchoff points remain unchanged and/or the workpiece touchoff points are unchanged (e.g. you haven't machined those surfaces away during the last op) re-touching ot re-probing zero should get you back to the same zero point to within less than a thou.

Generally my mill/router sequence is this:

1. Home machine;

2. Touch off fixture or workpiece X and Y, zero X and Y;

3. Probe Z (which sets Z zero)

4. Load file for Op 1;

5. With Z all the way up, jog to the X and Y extents of the toolpath and ensure that I am in the boundaries of the workpiece (which is a check to make sure the zero was properly set in CAM - if I touched off the lower left corner of the stock, but CAM zero is set to the centre of the stock, this will show up here;

6. When I am happy the setup is correct, run op 1;

7. Manually change tool for Op 2;

8. If the tool for Op 2 has a different Z height, probe Z to set Z zero (my router doesn't have toolholders so I'm changing tools in the collet, which means for tools that don't have a height setting ring, tool length is undetermined and must be probed. For a mill/lathe with tool holders and a fixed tool length, this step is unneeded);

9. Load file for Op 2. Sanity check extents in the visualizer;

10. Run op 2;

11. Etc until done.