I am attempting to use fusion to create continuous fourth axis toolpaths without paying for the $2k mutli axis extension.
I can definitely achieve the shape I am currently aiming for using multiple tool orientations(using the A-axis as an indexer), but I would like to see if it is possible to get fusion to create a continuous toolpath that could save some machining time.
I wrote a grasshopper script that does some coordinate transformation and unrolls my vase shape, shown here:
It doesnât appear to do the Y to A transformation that I was expecting. There is only one line in the g-code that calls out an A rotation, at the very start. Furthermore I am not sure if my input surface length is correct. I am currently using the max circumference of the vase, shown here:
Does anyone have any advice on why fusion is not posting g-code that wraps the y-axis of the file around the a-axis, or what to use for the input surface length?
The wrap toolpath is a very specific functionality. It only works with a small set of toolpaths on geometry that is on a cylinder. See this video:
There might be a way to let Fusion do the carving toolpath and wrap it yourself. You would have to load the G-code and transform the Y moves to A moves, possibly with inverse-time feeds. This might introduce an error because your transformation deforms the surface without a corresponding change in the cutter shape. If your cutter is small, that shouldnât matter.
Another option would be to do the indexing on a small slice and then write a script to rotate and repeat. This would work if your pattern repeats, which I think it does but canât quite tell. You could use Fusionâs stock bound feature to choose a slice thatâs off-center to get better cutter engagement.
I was hoping that the post processor for fusion from avid called âAvid CNC Wrap Y to A.cpsâ would do exactly that, transform the Y moves to A moves. Is this not the case?
Yes, there could be some cutter shape issues if the pocket is too small.
The âWrap to Aâ posts will do basically what they say⌠They take X or Y (depending on how you have your rotary mounted) and wrap those moves to rotary moves.
Using these posts essentially makes your 4 axis machine work like a 3 axis machine with one of those axes being swapped to a rotary.
To put another way: âTurkey on a spitâ.
I believe you can do this type of toolpath in Fusion, although I donât know how to set them up because itâs been a while.
What I did in some of my other posts here is to find another true 4 axis post, create code with that and then just massage it to work with Mach 4.
It should be noted that Mach 4 CAN do all 4 axes at the same time, our post doesnât do that.
For the model above, the âturkey on a spitâ approach with a ball nose would yield great results, and you might be best off using Vectric Aspire or Vcarve as that toolpath would be pretty easy to make in one of those.
@Eric That was what I was trying to achieve, the turkey on a spit 2+1 using an unrolled version of my vase. As you can see, despite using the Y to A post my g-code still has Y moves, and only references A once at the start of the file to zero it:
(PARALLEL1)
M5
T41 M6
S18000 M3
G54
G0 A0.
G0 X9.8532 Y-0.2305
G43 Z5.2259 H41
Z2.3372
I know you can do this the ârightâ way by buying the multi-axis extension for fusion or by using the fourth axis as an indexer which seems to post just fine after enabling the A axis in the default fusion post, although I havenât tried it on my machine. Not sure why the g-code still has y-axis moves, they should be A axis moves if the post truly translates y axis moves into a-axis moves. I may be missing something fundamental, I am new to fourth axis g-code.
Made a little progress, I made the part in fusion 360 inches long, then made a parallel finish with a 1" stepover. I posted the g-code, and used find and replace to swap all âYâ to âAâ. Nc viewer now shows this, which is what I was looking for:
I think this method will not work because the tool contact point calculations will be off. Could work for cylindrical parts but I think anything concave will be off due to how I had to stretch the part to trick fusion into outputting the correct A angle.
Back in 2010 I built my first 4 axis machine. It was a Sieg X3 conversion. I used a Sherline rotary table for the 4th axis and a Probotix custom controller. Cost me about $4,500.
Long story short, the CAM to drive that 4th axis was $50,000 per seat.
Consider yourself lucky. $33 a day is still peanuts compared to any other provider.
PS. For the record I still use the X3, original PC but the latest LinuxCNC build.
My neuron isnât firing this weekend and Iâm having a hard time getting the machine setup right for 4th axis rotary turning in Fusion 360. It was a piece of cake in Vectric Aspire, but Fusion and I have issues.
Does someone have a file they could share that includes information in the CAM setup so I can see how this is supposed to be done?
Thank you,
Scott
Ah ok, if youâre running vanilla CNC12 you can likely use the âCentroidâ post thatâs included in Vectric, but thatâs not going to get you rotary support.
Our EX Rotary posts will get you that, but with some caveats:
Firstly there are a couple of nice added features:
Even though you âloseâ an X or Y axis on a rotary post (because youâre wrapping one of them) our rotary post will get you to XY zero BEFORE the wrap. This can help you if you forget (like me) to get into position before running a rotary job.
ONE BIG CAVEAT on our âAVID-ifiedâ version of CNC12 we allow placing the rotary along the X or Y axis, and we allow placing the chuck facing either direction. Depending on how you place it the direction of the rotary axis reverses.
An example: Letâs say you have your rotary along the X axis, and you chuck is close to X0 but itâs pointing towards X+, this would mean your rotary spins normally.
If you had your rotary along X with the chuck facing X- the rotary would spin backwards.
We do this to make it easier for the user, so essentially all you need to do is tell us if your rotary is along X or Y, and we take care of the motor direction for you.
I say all of this because this automation is in our version of CNC12, and wonât be in the vanilla version of Centroid. You can still do this, but youâd have to set things manually.
Sorry thatâs not a direct answer, but you should be able to use our posts with stock Centroid reasonably easy as long as youâre paying attention to settings.
Thank you Eric. Iâm sorry I wasnât clear about what I needed. Running the rotary on the Avid and post processor isnât a problem at all. Thatâs been working well. Iâve taken a Centroid post processor originally from Gary Campbell and made modifications to also use a laser on the rotary (thanks to Jim Neeb). That said, I am going to look carefully at the Avid PP because you guys are putting a lot of thought into making Centroid stuff more accessible. Love that!
The machine setup Iâm having a problem with is in the CAM part of Fusion 360. For example, I donât know what generic (or otherwise) version of a machine to use for setup and Iâm having a difficult time getting the âwrapâ functions to work as I set up the cutting paths in Fusion 360. I thought that since this was a thread on wrapping in Fusion 360, a user thatâs gone through it might have a file I can import into Fusion to look at what theyâve done.
Iâm going keep banging away in Fusion 360 regardless. Iâm making incremental gains, but itâs slow and frustrating. Thatâs not an Avid problem, for sure.
Rotary toolpaths in Fusion are very powerful, but are a bit tricky to setup. One thing that got me tripped up early on was not having a âmachineâ setup.
We require that now with our Fusion posts⌠or to say another way: You canât JUST use a Fusion post if you want to do rotary work, you ALSO need to pair it with a âmachine profileâ
Both of those are available on our website for download.
If you want you can check out this Fusion test file I made for rotary:
Hopefully this doesnât confuse more than help, but things to look for:
Check the Setup and look at the machine I have in there (Avid EX with rotary). I have that in there because the Machine Setup itself has a rotary axis configured. THAT is what tells the post âHey you can post A moves nowâ
Then dive into the toolpaths. Iâd ignore anything but the facing toolpaths just to learn how it works. If you look youâll see the âtool orientationâ set in each of those toolpaths.
Itâs also worth noting that this job is meant to have Z zero at the CENTER of the rotary axis, NOT on top of the stock.
At some point in the future I have on my list to make a video for rotary operations. Itâs not going to be out in the next few weeks though. Hopefully this helps you out a bit.
Please do keep posting questions in here. Iâll try to help as best as I can. (I do have a busy few weeks coming up)
However, questions from you (and anyone else whoâs got rotary questions) will be great in helping me figure out content for an upcoming video.
One thing I will say: If you want true 4th axis rotary Fusion/Centroid is the way to do it. Once you get your head around Fusion youâll be able to make great use of it.
What I did early on was make a reasonably simple shape. It was just a 4 sided box with a chamfer on one side. I practiced making facing toopaths on each side. Then I would air cut it. Once I got that down I saved that model and would keep it for reference when I made subsequent models.
