Before I upgraded the firmware (black box, not masso), I could program a 3d or area clear with multiple tools (with different tool numbers) on a single toolpath. The carve would pause between tools, prompt me to change and then re-probe Z then run the next tool.
Since firmware upgrade, carveco now tells me the controller won’t allow multiple tools in a toolpath. Did I miss something?
you did. the BB controller does not support changing tools and resuming. You need separate files for roughing and finishing (not really a big deal, you just load the roughing and once complete, load the finishing). It won’t prompt the tool change, you could modify the post processor, but why bother.
1 Like
The original BB controller could not make tool changes from a single file. But since you say you used to be able to do multiple tools in a single file on the BB controller you must have had one of the tool change routines installed that can be found on this forum. Like this one - but there are others.
Do you remember installing such a thing? Perhaps the firmware upgrade un installed it.
This is curious. Is it Carveco’s post that is telling you that? Have you updated Carveco or it’s post? Where do you see the warning message?
1 Like
I never did any upgrades to the BB controller until just a few weeks ago. Up until that point, If I programmed an .stl 3d file with a roughing bit as tool 1 and finishing tbn as tool 2, it would save the gcode and run just fine. First purchased in 2021 and have run that way for 3+ years. Like I said, after the roughing pass, it would pause, ask for the tool change, re-Z and then continue when all those steps were complete. Now when saving, Carveco says my controller won’t support. But it once did, so I’m confused as to why that changed.
I understand it is confusing, we are trying to help.
As Aiph5u showed in the link I posted there was a very limited toolchange routine on the original BB controllers. You must have been using that then. I too have had my machine since 2021 and I know that rooutine was there (though I never used it).
I have upgraded to 1.4.1 serveral months ago so I will start up my machine and see if it is still there or gone.
While I am doing that - please let me know how Carveco is telling you this? Is it a warning box on your computer? or is it a warning on the Onefinity conrorller?
First off I should apologize for saying in my first post the controller could not make toolchanges. The routine shipped with them is limited and so problematic for most people that the recommendation has always been don’t us it. Since I never used it I forgot it was there.
And it is still there in 1.4.1
It is the exact same as was in that post I linked to back in 2021.
If you want to verify on your machine go to settings and scroll down to “On Tool Change”.
If it looks like this below then the controller must still be able to do what you were used to.
(Runs on M6, tool change)
M70
G21
S0
M0 M6 (MSG, Change tool and attach probe)
F100
(probe to minimum z soft limit, which is -10)
G38.2 Z-10
G92 Z15.4
g0 Z30
M0 (MSG, Remove probe, start spindle)
M72
But the question still remains - how is Carveco telling you this? Is it a warning box on your computer? or is it a warning on the Onefinity controller? That will help us determine where to look for answers.
Hey Mike,
on the buildbotics-derived Onefinity Controller of the Original/X-50/PRO Series, G-code files with multiple tools including correct prompts for tool changes are only expected to work if you insert a working tool-change routine into the ‘tool-change’ field on the SETTINGS page. Such a routine is here: Aiph5u’s tool change routine (posting also contains instructions on how to install it) (honors tool numbers if provided by the CAM program).
Note that reverting to the default settings on the ADMIN page will delete the new tool-change routine.
1 Like
Sorry for the delay, the “day job” got in the way. Appreciate folks jumping in to help.
I uploaded the error CarveCo gives. I can create the toolpath and simulate, but once I go to save I get the error.
To be clear, I never changed any code in previous carves. I could do this same function, name the tools separately (tool 1 and tool 2), and save without issue. Once running, it would prompt for the tool change. I didn’t add or modify the code. Once I upgraded, this stopped working. Had I specifically added the code I’d understand, but frankly had never CNC’d before I bought this one and despite being an IT guy in my real life, wouldn’t have know back then how to modify g-code to make it happen. If the upgrade removed this capability, I guess it is what it is, and could look at adding it back in. Just seems weird that it did work for 3+ years.
There different post processors for tool change in carveco maker. Make sure you have the one for tool change selected and not just the onefinity inch or mm post processor.
Hey Mike,
Carveco cannot know that you updated your machine. That’s why I wanted to know where the error was coming from. So rule out the update on the Onefinity. And besides I checked - onefinity still has the same code it had 3 years ago for tool changes.
So it must be a different post processor file that you used before in Carveco. Or maybe there was an update in Carveco that changed something.
Do you have an old toolpath file with 2 tools from back when it did work?
Would you be able to post it here or DM it to me. That would tell me what it used to do and how it did it.
1 Like
Thanks team. I was wrong/you were right…it wasn’t the journeyman and firmware update, apparently it was in a careveo update. The post processor for tool change was no longer an option, so I had to go searching through this forum for that .con file and downloaded it. Toolpath saved, so now I’ll need to find time to run it again.
Appreciate the help!
1 Like