Z Axis Travel Exceeded- Confusion about Work/Tool Offset <self resolved>

[carboncymbal]

zAll,

This will be a series of dumb questions that show my ignorance about work and tool offsets. My previous CNC experience using a tool library with offsets and toolholders comes from using Tormach Path Pilot. I am using the great Probe App and Swissi's recent ATC option as well. That said, I am having the same fundamental issue with another machine using my own ATC implementation, so the issue seems to be my understanding of the offsets. I am also using a fixed tool touch off device with my Z home position as my reference. I do not currently have a probe installed, but will shortly.

I am running an Avid Benchtop Pro CNC router.

What I expected

SETUP- 2 tools are measured, showing a Z height offset in the range of -4.5" (as I understand it, this the measurement of the machine Z coordinate at the time the Tool Touchoff is triggered).

With tool 1 loaded, G54 active, I jog the machine over to the cut area and put the tip of the tool in the position of the origin of my cam model (in this case, the rear, lower, left corner of the stock, on top of the vise). I then select "Set WCS XY0" and "Set WCS Z0". When I do this on my Tormach, it sets G54 origin point. As I change tools, the tip of all tools is in the same location.

What happens (I think)
When I do this on my machine, the machine tries to cut below the table, which results in a "Z Axis Travel Exceeded" error. After I rehome the machine from my frantic E-stop, I see that when the machine is at Machine 0,0,0, the Z position in G54 is -(G54 Z offset + T1 Z offset), in my case -1*(-3.7615+ (-4.5572)=8.3187.

Can someone please point me in the right direction for this? It seems I have a fundamental misunderstanding of the relations of the tool and work offsets, and how to correctly set a WCS origin to cut a part.

Thanks!

I have attached a current report and the test Gcode file I was using (using Swissi's Fusion 360 Post Processor)

[carboncymbal]

Well..... That is embarrassing. I didn't have G43 active when establishing Z0 for my G54 work offset. I just tested it and don't have any issues now and the program runs where I would expect.

[Muzzer]

Yes, it's the G43 Hx command that catches people out. Swissi's probe app takes care of that for you but if you are changing tools manually and want to set heights etc manually, the controller won't know what tool length to activate unless you tell it.

If I'm feeling particularly paranoid, I will load the tools I'm about to use, one after the other, activate each tool length offset (G43 T1H1, G43 T2H2 etc), then jog down to 8-9mm above the work origin (where WCS Z0 is etc) before raising the tool slowly until I can roll a 10mm cutter shank under the tool. If I have the offsets right, the indicated Z coordinate should say 10mm when it does. This has saved me a few crashes for sure.

The Z axis travel check may have saved your tool, as the offset error would have required more Z axis movement than the machine could manage.

If you have limited Z axis travel, there's benefit in trying to minimise the range of tool length offsets (ie the range of different tool stickouts). The sum of that range plus the required machining heights needs to be less than the available Z axis travel - including the final retract move. Getting all that within the available travel can be a problem. Yours is a router, so likely less of an issue due to the more 2D nature of the work but for turret mills (Bridgeport etc), some careful adjustment of the table height may be required. I had to resort to a spreadsheet at one point, to tell me the appropriate table height so I could avoid the "Z axis travel exceeded" warning.

[CNCMaryland]

Another way to do this is to go to Setup -> Part - go to the Z Axis, select the tool that you are using to zero, and then set it to 0.