First time with my Atrump. I'm stuck with an error message.

[kenmwallace]

The hardware all seems to be working great. I am really impressed with the Atrump E216/Centroid machine. I know I will love it after I learn my way around the controls better.
I am used to Hurco, so there are some things I have to get used to in this new environment.
The first part I am trying to make simply needs a 5.5 inch diameter hole milled into it.
In the following photos I show the very simple Intercon program that I created to do this.
Another photo shows that when I try to run it, there is a message that tells my have Z axis overtravel.
But I am nowhere near the end of travel in Z.
I looked at the work envelope in the WCS. It is all zeros. But, I understand from the CNC10 manual that work envelope is only in play if there is a G22 in the program.
The next photo shows the G-code. There is no G22.
Any suggestions? Report file attached.
Sorry for dumb questions... This probably won't be the last, but it sure is good to have someone to ask!

[tblough]

It's trying to add the length offset for H1 and that will cause it to exceed the Z axis travel. What is the value of H1 in your tool table?

[cncsnw]

Hmm. That is a good question.

First, a "907 Z axis travel exceeded" message relates to the overall software travel limits (set on the Machine Configuration -> Jog Parameters table). The G22 work envelope is not relevant here.

You will get the same "907 Z axis travel exceeded" message, whether your program tries to move Z above the plus software limit, or below the minus software limit.

Your screen picture above does not show what coordinate system is active, but at the time you made the report, WCS #1 (G54) was active. I will assume it was the same when you tried to start running the job.

If the job were to run, then at the start of line 24 Z might either be at the carousel level (if a tool change were needed, and the M6 macro were run) or it might be all the way up at home (if a tool change were not needed and the M6 macro was skipped). In either case, though, the positioning mode should be G90 (absolute).

The Z zero point for WCS #1 (G54) is -13.0138 (down from home).
The height offset H1 has a value of -0.5144.
There is no G52 offset in use.
Therefore the move on line 24, assuming G90 absolute positioning, should be trying to go to -13.4282: -13.0138 - 0.5144 + 0.1000
Your minus travel limit for the Z axis is -19.8800.
Therefore there should not be a problem doing that move, assuming the WCS is G54 and the positioning mode is absolute.

If, on the other hand, the positioning mode was somehow switched to incremental (G91), and T1 was already active (so the M6 macro is skipped), then at the start of line 24 Z would be at home (because that is where your G28 return point is set), and line 24 would attempt to move Z another 0.100" higher than that. That would exceed the plus travel limit.

1) Change Machine Parameter 10 to a value of 3.0; turn on Single Block mode; and run the program.

This will be a little tedious, because you will have to press Cycle Start for every single line of the program, and every line of every macro it calls. But it will show you every line, including lines in the macros, and it will not read ahead, so it will actually run all the way to where the error occurs.

2) Try changing the Z level of the G28 return point from 0.0000 to -4.9780 (same as the G30 return point) and see if the program runs without errors, and whether it cuts the first pass of the Frame cycle at the correct Z level.

[kenmwallace]

Thanks very much for your thoughtful analysis.
I did have the offset wrong for the tool I was trying to run.
When I set the offset to zero, all was good and my part is made.

[kenmwallace]

I think I will learn a lot from a careful study your suggestions.