Manual tool change problem

MaHa beat me to it

JohnnyCNC wrote: if create a part in Fusion 360 and used 10 different tools for the job I will have 10 files and must have room for 10 tools in the tool table.

Just a note that the Fusion360 postprocessor inserts a G53 Z0 before every toolchange. This is a move to absolute Z zero, and that pretty much _requires_ that the Z axis is configured with top at Z=0 and bottom at Z = -5

Finally - nearly there.
I thought you guys may have cracked it, but unfortunately ....
It was still going low on the tool change.
When I try to home the Z axis it always changes the DRO and backplot to Z0, regardless of where it was previously, and rewgardless of where the mill is.
I finally decided to give in and accept that Z0 had to be the top of the Z-axis column.
Set the toolchange position in the .ini back to 0, 0, 0 and subtracted 4 from all the Z and R values in the test file.
It now works almost perfectly - just one small niggle - it is not going back to true Z0 for the toolchanges - it is going to Z0 minus TLO.
I guess it is something to do with the G53X0Y0Z0 command preceding each tool change - is there another G code that takes it back to absolute zero?
The resulting backplot display is a little counter intuitive as my material is now down at Z-4, but I can live with that.
Thanks again for all your help.

G53 Z0 wil take the axis right to the top.
But the actual tool tip (in the physical world) and the tool tip and DRO on the monitor will show a z position that takes in to account the Z length.

You can switch to showing absolute coordinates in the display, if you want. That should definitely show zero at top of travel.

Just to expand on what andypugh has mentioned, if returning to absolute zero (G53 Z0) Axis also takes into account any G43 offsets present at the time G53 G0 Z0 was executed, so the tool in the backplot will appear to be at TLO units lower than the expected Z position.

When I try to home the Z axis it always changes the DRO and backplot to Z0, regardless of where it was previously, and rewgardless of where the mill is.

Then I suspect you will also need to redfine your Z-axis max and min limits on your INI file to be max = 0 and min = -5. When you home in Axis it is assuming that you want the current position of the cutter to be re-referenced to Z=0 as defined by the range of motion specified in your INI file.

After you get this straightened out you shouldn't need to go back and manually rejig your G-codes. It should all just work