Upgraded but now soft limits always hit - SOLVED

[ATS-Byron]

Hi All,

Here are some updates:
-A report after starting it up and the system asked for the TEST to be done.

-A report after homing, after the TEST was done.

-A report after wtb12-row4.ngc failed

-A report after bclb-r-wtb12.ngc failed

-A report after ptb.ngc failed

-A report after power down and reboot with homing

-A last report after trying wtb12-row4.ngc one more time

Also here are some updated pictures and added pictures https://tinyurl.com/2eb4r42r

[centroid467]

If you graph the wtb12-row4.ngc program in CNC12 (F8 graph job on the main screen), does it give the same 907 errors on the same lines?

[ATS-Byron]

If you graph the wtb12-row4.ngc program in CNC12 (F8 graph job on the main screen), does it give the same 907 errors on the same lines?

Hi centroid467, if I press F8 it goes to what I expect is the graph window, but there are no errors that pop up.

[cncsnw]

That suggests that the problem relates to your tool-change macro, since it includes lots of axis movement, but skips nearly all of its code during the F8/Graph preview.

You could try changing Machine Parameter 46 from 1 to 0, so that the active G codes display is present while running a CNC job; then running the job in single block mode (this takes some patience, of course).

Single-block mode prevents lookahead, so the control will not report the 907 error until it actually reaches the line that would exceed limits.

In the mean time, you could check to see whether the G21 mode is correctly restored after the M6 tool change is complete; or whether the M6 tool change leaves the control in G20 mode, even as you proceed to moves that have large millimeter dimensions.

[ATS-Byron]

cncsnw, when I run the wtb12-row4.ngc in single block mode it stops on the error at line 21. See attached picture.

I am not sure how to check the G21 or the G20 mode?

Thanks.

[ATS-Byron]

Actually it fails at line 12 first. See attached picture.

Does that mean in the G-Code there should be a G21 before those lines?

[ATS-Byron]

Ok, never mind my last post. It only failed on that line 12 because I didn't restart the program. When restarting it goes to line 21 and fails.

[tblough]

You are in G20 inch mode (the line of codes just above the F5 key), and trying to move a little over 2,380 inches in X. That would be quite a large machine to be able to do that.

It looks like you are missing a G21 in your program to switch it to metric positioning.

[ATS-Byron]

Also just noticed that I had meant to upload those job files and didn't.
Attached are the 3 jobs that I ran to go with the reports attached earlier.

Thanks.

[cncsnw]

All three job files include "G21" at the top of the file.

It appears that your M6 macro is switching to G20 mode, and failing to switch back.

You should contact the support technician at Centroid who helped you with the tool-change macros, and see if he can locate the problem.