Ahhh, that explains a lot. This is more than just a curvy thing that you can just do by spinning around…
So there are a couple of ways you could approach this…
A true 4 axis post would help you if you wanted to do this totally in Fusion. As you saw from my other thread this doesn’t exist right now. Like me you’d have to hack together code from another post.
I have a background in writing posts and coding G code, so for me this was something I was comfortable enough doing. I’m not great at it, but good enough to power through.
So that’s an option… Another one might be this:
All “tool orientation” in Fusion really amounts to is doing 3 axis stuff, rotating the rotary, doing more three axis stuff, rotating again, etc. since you have some pretty predictable angles in there you could just make regular old 3 axis tool paths for each angle, save them out and just run them one at a time, rotate the axis, and run the next one.
If you wanted to automate it a little more you could copy paste each separate tool path into a single text file and simple issue a rotate command after each toolpath, that command would be simply:
Yes it does make sense, I was hesitant to ask if I could do that at first. I tried it once and the A axis rotation was way off even with the correct degree value input and screwed the stock up so I moved on and purchased the machining extension for rotary tool paths. Does anything ring a bell for why G0 A90 command was off? I slowed down the motor 4 acceleration because the rapid movement was extremely fast but I haven’t tried it since I changed the acceleration. (I don’t remember if it was velocity or acceleration that I changed in Mach4 but it defiantly slowed down its rotation speed when I ran a rotary tool path)
Also, thank you for all the feed back and reply’s. This is the most insight I’ve gotten from anyone since I started and it’s really helping me out!
3+1 indexing in Fusion 360 using the Tool Orientation option works out of the box with the current Avid wrap-to-A post-processors. I use that pretty much exclusively when doing rotary axis work in Fusion.
Can we see what you’re doing a little more in detail? Maybe post these for a single simple small operation, like this:
Lucas, I use my rotary as an indexer and use the tool orientation function in the Fusion tool paths.
I would machine like this.
LH side 3D Adaptive
RH side 3D Adaptive
Both roughing with a square end mill, leaving .030 material. (Caution, with heavy cuts you can spin the rotary)
LH side Scallop
RH Side Scallop
Both with a ball nose end mill machining from the inside out on the paths.
If I have any areas on the side that Scallop doesn’t clean up I typically use a Flow path on those areas.
Top Inletting
3D Adaptive (sq end mill, leaving .030 material)
After that I use a Parallel path with a ball nose to finish the barrel channel and any other curved areas.
The rest of the inletting finish work is 3d Contours, 2D contours and Bores and anything else that is needed to get the geometry cut.
Rinse repeat for the bottom side inletting as needed.
Once you have the sides complete and are working on the inletting, the stock will have a fit of flex to it.
At that point, I support the stop with machinist screw jacks. (Caution with your A moves once you are supporting with screw jacks. Make sure you do not have any A moves while on the jacks)
This is huge! Thank you so much for this, did you use one of avids post processors for fusion when running tool orientation within your paths or did you have to alter another machines post to get rotation?
I am using UCCNC instead of Mach4 for machine control. The post for UCCNC for Fusion does the 4th axis rotations when using the tool orientation in Fusion.
No problem. For anyone that stumbles upon this I found this video explaining how to modify the post, I haven’t tested it in real life but it allowed me to post from fusion with the 4th axis as an indexer: https://www.youtube.com/watch?v=mbBkrYQ1AbM&list=WL&index=5
