Tool offsets issue, cannot start program[video question]

More
16 Sep 2023 19:27 - 16 Sep 2023 19:59 #280947 by petmakris
I am having the issue I speak in the video about. 

Let's say I have tool T1 loaded on the machine and I want to run a program that uses tools T4 and T5.

If I try to start the program while T1 is loaded on the machine, I get an error, maximum Z will be reached. 
The first strange symptom in this case is that there is enough height available on Z.
But the super spooky part is that it complains about Z height before asking me to change the tool from T1 to T4. 

More strangerest, If I swap T1 with T4, the program starts and works as expected. How is this even possible?



 
Last edit: 16 Sep 2023 19:59 by petmakris.

Please Log in or Create an account to join the conversation.

More
16 Sep 2023 22:43 #280951 by tommylight
Upload hal and ini files at least.

Please Log in or Create an account to join the conversation.

More
16 Sep 2023 22:58 #280955 by petmakris

Upload hal and ini files at least.
 

The config files, including everything are located here, it's github link.
Pressing the dot key once loaded should start an in-browser studio code environment.

github.com/petmakris/maho-mh500w/tree/main/config

 But here are some links as well:

HAL files

github.com/petmakris/maho-mh500w/tree/main/config/hal

INI and Expanded INI

github.com/petmakris/maho-mh500w/blob/main/config/maho.ini
github.com/petmakris/maho-mh500w/blob/ma...ig/maho.ini.expanded

INC files for INI

github.com/petmakris/maho-mh500w/tree/main/config/inc

TOOL TABLE

github.com/petmakris/maho-mh500w/blob/main/config/tool.tbl
The following user(s) said Thank You: tommylight

Please Log in or Create an account to join the conversation.

More
19 Sep 2023 11:21 - 19 Sep 2023 11:22 #281151 by petmakris
I am a bit suprised that nobody understands the issue I am facing. This should be a very beginner workflow/use case.

Is there missing information from my video question?
Can I explain better the issue? 

How could I improve my answer so i get some help?
Any hints appreciated.
 
Last edit: 19 Sep 2023 11:22 by petmakris.

Please Log in or Create an account to join the conversation.

More
19 Sep 2023 12:44 - 19 Sep 2023 17:05 #281160 by Aciera
Have you tried running the program anyway?  I'm pretty sure that message is not relevant and the program would run just fine.


Also, I think if you use gmoccapy instead of axis gui this message does not appear at all.
Last edit: 19 Sep 2023 17:05 by Aciera.

Please Log in or Create an account to join the conversation.

More
19 Sep 2023 18:28 #281182 by petmakris
Hey thanks.

I haven't tried to skip the warning, I don't feel safe doing so actually     
But I don't know how the machine will behave. Will it try to travel outside of machine boundaries?

 

Please Log in or Create an account to join the conversation.

More
19 Sep 2023 20:00 #281188 by Aciera
That error message comes from the Axis GUI and, as far as I am aware, no other GUI checks for limit violations. In my opinion it is one of the very few bugs in the AxisGUI and should probably just be removed because checking for limit violations is done elsewhere in the code.
So, no, the machine will not violate limits even if you ignore that message.
The following user(s) said Thank You: petmakris

Please Log in or Create an account to join the conversation.

More
21 Sep 2023 11:28 #281293 by petmakris
I skipped the warning and everything went fine.
Thanks.

I might try a different UI though now I've seen this.

Please Log in or Create an account to join the conversation.

More
21 Sep 2023 18:22 #281324 by Henk
Hi. Are you running a cam generated program? I didn't see any gcode above.

I noticed that your z axis max limit is 0. In my experience, when this is 0, and your program contains lines like "G53 G0 Z0" as a retract move, it causes errors similar to these.

Replacing those lines with G53 G0 Z-5 for example eliminates these errors (in my case at least)

For this reason, I always set the maximum limit for z in the ini file to something slightly larger than 0. Even 0.1 usually prevents this issue.
The following user(s) said Thank You: petmakris

Please Log in or Create an account to join the conversation.

More
22 Sep 2023 13:54 - 22 Sep 2023 13:58 #281377 by Aciera
This is caused by a bug in Axis' limit checking. The method used calculates the maximum and minimum gcode movements and then adds the tool offset values that are active at the time when the 'RUN' or 'STEP' command is issued.
It has no knowledge of any tool changes in the gcode and thus it uses the same tool offset values for the entire gcode in the program. If the tool offset values of the tools do not vary much then you may not see an error message from Axis although you may get one from the interpreter/trajectory planner anyway. On the other hand, if you use a long tool (like a probe here) and start the gcode with that offset active you will very likely get a false warning and the code will actually run just fine when you ignore the message by clicking on the 'Run anyway' button.

I have filed a pull request to remove separate limit violation checking in AXIS.
github.com/LinuxCNC/linuxcnc/pull/2652
Last edit: 22 Sep 2023 13:58 by Aciera.
The following user(s) said Thank You: petmakris

Please Log in or Create an account to join the conversation.

Time to create page: 0.337 seconds
Powered by Kunena Forum