Solution: Working with Onefinity support they have found a bug in the firmware where the stepper values are not updating when the Rotary button is changed. This makes the “steps wrong”.
Here is the temporary solution from Onefinity support:
—————-
The Y2 axis values are not changed to the A axis values. We’re working with the Dev team to correct this issue.
The settings should be as follows:
Microsteps = 16
Max-Velocity = 6.696
Max-Accel = 500
Max-Jerk = 1000
Step-Angle = 0.25714 degrees
Travel-Per-Rev = 360
Manually enter these values into the Motor 2 settings page (Be sure the drop down is set to “A” and not Y or Y2) then be sure to press save in the top left corener.
————
My “fix” made it work, but it was not correct. As support mentions, make sure you go to motor 2 in settings after rotary has been selected. If it doesn’t say A at the top, click motor one and then click motor 2 again. It should now say A at the top. Enter the values as directed by support.
Many thanks to Support.
EDIT: I have a rotary axis on my metal CNC mill, the rotary axis reads in degrees. The Onefinity BB rotary reads in inches. I thought it might just how it reads on the screen, but when Vcarve puts out the toolpath, (in degrees) and you run it, the rotary takes those measurements in inches. Not a good time when A180 makes it spin like 30 times.
Anybody know what I am missing? I can’t see any place to adjust the rotary to degrees and I can’t find a post processor that will output rotation in inches?
Thoughts?
Possible solution: When the rotary is engaged in the BB controller, I went to the motor 2 settings. They are labeled A in this configuration. I adjusted the “travel per rev” so that a G0 A360 command made the rotary turn one full turn. I continued to adjust based on trial and error, (no real math here). I think I have it pretty close at 51.4 mm. This may not be the final required number, but now a 1 mm move is equal to 1 degree. At least now it’s close when Vcarve gives an output in degrees it matches up.
I have asked onefinity support to look at my numbers.
A180 gives you 30 rotations? Wuh? Output rotary in inches? Wuh?? 1mm equals 1 degree…WUH??? What do you do to mill a taper then?
There are 2 other people here with me reading your post…and all 3 of us are scratching our heads. Could you maybe try to rephrase
@WC_CUSTOMS
EDIT: For clarity, I am talking about the Buildbotics rotary, not the Elite rotary.
Sorry everyone, I obviously have not done a good job explaining here. The current settings for the BB rotary seem to be off. We want our rotary to work in degrees, not in linear movement. Vcarve and other cam software output the toolpath in degrees. So a gcode of say G1 A180 means to move the rotary 1/2 a full revolution. With the current settings that gcode will spin the rotary a number of full turns. ( not sure how many, my 30 might be an exaggeration. )
I have adjusted the travel per rev setting to attempt to fix.
Maybe I am the only one that is seeing this problem, if so sorry for the confusion everyone.
Would love to hear from other BB rotary users. There is not a lot of users with the BB rotary as it just shipped for the first orders. How is it going for you?
1 Like
Sorry friend, I’ve got nothing of value for ya. I can’t get past the “travel per rev” you’re talking about. That would change with every diameter. I’ve never seen or heard of a post that outputs a rotary in inches. I don’t know how a 180 command could result in more than 180 degrees unless you’re switching from incremental to absolute. What happens if you zero a axis, then go to MDI and type in G90G0A180?
Thanks @WC_CUSTOMS
I know, it’s weird. In MDI I entered your code just like that and it spun many rotations. The travel per rev is not a setting I am used to seeing either, but it is the only setting in the BB that I could adjust. It does seem to work.
Appreciate your help though. As this BB rotary is brand new we will see if others have a better solution than I have come up with.
Thanks again.
Note: once set so that the rotary makes one full turn for a command of 360, it wouldn’t have to be adjusted for different diameters of stock. The software would make appropriate changes in the number of degrees required for the movement.
1 Like
Did you ever find a solution for this? I am Currently troubleshooting mine. It seems to run along the x just fine but when it comes time to rotate it completes many rotations before stopping to make another pass on the X. If running a rounding toolpath this creates a real mess as the edges of the square ram into the bit.
I tried the settings that you have posted up top but those are not feasible, it turns a 30 minute job into a 6 hour job. Although I do believe it is probably a settings issue I have yet to find the solution. I should add that I am not sure why this is so difficult
We’re finding a few bugs with the software and post processors. It will take us a bit to sort them out. The pains of a early adopter 
One bug is when you push the rotary button, the A axis values aren’t changing to what they should be. We attached them here, so you can manually input them (then make sure you hit save at the top left after changes) until we find and fix this bug in the next release.
2 Likes
@shadowop30
The settings change for the A axis are a must as Vcarve will output A axis in degrees. A gcode command of say G0 A360 must turn the rotary one full rotation. If your A axis is turning multiple revolutions it is not set correctly. Make sure when you go to motor 2 settings that it says A at the top. If not, push motor 1 and then motor 2 again and it will say A. You must be in rotary mode to change this settings.
My two cents worth: The A axis will be slower, but appropriate.
To decrease carve time you want your carving to be mostly along the x axis, not around the A axis. Raster direction will affect this. Make sure you see your tool paths run down the length of the stock, not around the stock.
1 Like
