I’m trying to do a double sided job on my rotary, using my rotary as an indexer. I’ve used Fusion 360 and using “tool orientation” to flip the material. I did the same with with Vcarve and doing a double sided job. Both times my alignment is off. I can’t for the life of me figure out why. I thought maybe it’s a calibration issue or something but whenever I do a vcarve wrap job the prints turn out fine. I’ve also tried a 4 sided job and it seems the sides R and L are reversed and backwards.
4th axis work is extremely sensitive to misalignment of the axis of rotation with the machine as well as alignment of the center of rotation with the work offset/zero. Those things I would check first.
I calibrate my rotary using cuts like these. It’s possible to eliminate most of the offset, but it’s not easy. Someday I might figure out how to add set screws for finer adjustments at each end of the rotary.
Do you have the latest Mach4 install? There was a previous version that had errors in the rotary calibration scripts.
@ThinkboxTech That’s what I thought to. I ran the calibration tests and made sure I’m fully calibrated. I used the avid cnc calibration test in mach 4. Is there another way to test it? Maybe check the steps on my rotatory?
@Stephen I totally forgot to run an update. Silly mistake. I ran and update on all the applications, did another calibration test and then ran all the code again. Still the same issues.
I tried to run two separate jobs and manually rotating the rotary from 0 to 180 on the second job. Still the same issue.
How about a simple through-hole, half drilled from either side? Eliminate all of the potential for software wrapping errors and disparate design/coordinate spaces.
@Christopher Here is it bored out on both sides. I used fusion 360. It was one done in one job. The circles don’t aligned. I measured the width and diameter of the circles and they seen accurate.
I was just talking to avid support about this yesterday, I am trying to be able to keep parts indexed for a 3-axis double op then onto the fourth axis for the third operation. For the 3-axis double op I am using alignment pins in the bed and holes cut in the first operation, and for the fourth I am planning to cut an inverse of the rotary chuck jaws into the base of the piece.
Getting the jaws to be truly square to the spindle has been a challenge. I have gotten it pretty close by putting a dial indicator in the spindle and backing the proximity sensor in and out until the horizontal jaws are close to level on the dial indicator after homing the A-axis.
If I can’t get that method close enough after zeroing, Liere from avid also suggested that I could measure what the angle of the jaws is after homing, and use that angle in my setup in fusion, or simply modify the angle of zero in the MDI before each cut.
Sounds like your issue might be a bit different if cuts dont line up after a 180 degree rotation – it seems like you should check if your XY axes are zeroed properly when doing A-axis cuts.
I homed everything and did a Y X diagonal square test to make sure the calibration is correct. It seems like everything is. I then did the bore hole test and still the same results.
Your rotary work offset is good enough for VCarve wrap jobs
Small to medium misalignment for drilling a hole from both sides with Fusion, most likely from rotary work offset X0 error (X because you have a tabletop installation)
Larger misalignment for VCarve box
Even larger misalignment for Fusion box. Very large.
Here is what I recommend
Take @greg.obj’s suggestion – check your rotary centerline directly. I suggest visually comparing alignment between the point of a narrow V-bit and the point of your tailstock when at X0 and Z0. It’s a quick and direct check.
Use a tailstock if you aren’t already. It helps keep your workpiece from shifting, and it helps overcome misalignment between the chuck rotation axis and the rotary (chuck-to-tailstock) axis.
Rerun the rotary calibration. That process stores values for the offsets between the touchplate and the rotary centerline. My guess is that these values need to be regenerated. You can skip the physical adjustment steps if you want. This might help with the holes drilled from both sides and the VCarve misalignment, but the Fusion misalignment looks larger.
Export a .f3d file for your Fusion box and upload it here so we can review it.
Once you work through these, if you’re still unhappy with the performance, we can figure it out from there.
Okay I figured it out. With all your guys help. I’m not sure what I did or how I did it but whenever I was zeroing out x on the rotary it was offset. For some reason it was adding an offset of about +5mm. This was even after I did the rotary calibration. It wouldn’t change no matter what calibration I did or how many times I did it. I ended up deleting mach 4 and all avid cnc apps, and then reinstalled them. Ran the calibration again. It works fine now.
I was having issues, when running the rotary as an index in fusion 360, with the sides being reversed/flipped. All I had to do is was click reverse A axis in the post process. I’m just adding this here in case someone runs into the reversing problem and can find the solution here.
Glad you got it figured out. I do a lot of four sided 4th axis work . For finding the center axis of the rotary and checking the the tail stock is true to the chuck, I use a piece of heavy wall extruded alum tube in the chuck and supported with the tail stock center. Touch off each side of the tube at the chuck to find the center. Use a dial indicator mounted on the spindle and run the length to check tail stock alignment to the chuck. Spending some time doing this really pays off when doing multi-side work .
I also use a small lathe face plate screwed to the stock then hold onto the face plate hub in the rotary chuck. On the tail stock end I have an aluminum plate with a center hole drilled in it, that I screw to my wood stock.
