General Help

I have fixed it in the master (development) docs. 2.7 is so different with the joints/axes split that it doesn't make sense to fix it in the 2.7 docs.

TOOL_CHANGE_QUILL_UP means that the Z-axis moves to the G53 Z=0 position.

It sounds like you might have configured with the home/limit switch at zero and home at -(small number)

Try setting the home switch to be at +(small number) and home at zero.

tjd wrote:

For example, a job/part needs 4 tools to machine it, where in AXIS GUI can I set up each tool relative to part zero??
I can't see if this is done from the tool table or somewhere else in AXIS.

You use the tool table, but you can populate the table from the Axis GUI.

You do this using the "tool touch-off" button.

Here is one way to work.

Choose one tool to be your "master" tool, this should always have a zero-offset in the tool table.
Then use this tool to "touch off" the workpiece (using the normal "Touch Off" button)
Then change tools (M6 Tnn G43) to load another tool, and touch that off to the same point, but this time use "Tool Touch Off".
The result of this is to populate the tool table with the difference in length between the master tool and the other tool.

The G43 is very important.

If you have a probe then it is best to make that the master tool.

One way to touch-off is to use an accurate dowel (I use one of my many broken 6mm carbide milling cutters). Lower the tool to be close to the work and then jog _up_ until the dowel just slips through the gap. This is far safer than jogging _down_ to something.

Once you have set up your tools like this then you can use any tool to touch-off the work, as long as it is loaded with M6 and G43 has been applied.



An alternative way to do this is to actually measure the length of each tool and populate the table either directly or using the G10 commands.

tjd wrote:

Great, I had managed to work out some of that with trial and error since posting but had omitted the G43.
What does the G43 do to the touch off/tool touch off process?

It applies the tool-table offsets. With those not applied, or with the wrong offsets applied, the G10 calculations (which is what "Touch off does" will be incorrect.

Also, I select spindle speeds manually on the HURCO, consequently I haven't made any configurations for spindle encoder/pwm values.
I was expecting LinuxCNC to show me some kind of dialogue box (like for when changing tools) to indicate the spindle speed to set manually but it doesn't. How do I set this up? or is it not a feature of LinuxCNC?

As far as I know there isn't anything existing that does this.
I would strongly advise arranging for LinuxCNC to have control of the spindle. But if you can't then a Python userspace module (just like hal_manualtoolchange) shouldn't be hard to create.