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 doesn’t 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 shouldn’t 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 can’t quite tell. You could use Fusion’s stock bound feature to choose a slice that’s off-center to get better cutter engagement.
I was hoping that the post processor for fusion from avid called “Avid CNC Wrap Y to A.cps” 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 “Wrap to A” 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: “Turkey on a spit”.
I believe you can do this type of toolpath in Fusion, although I don’t know how to set them up because it’s 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 doesn’t do that.
For the model above, the “turkey on a spit” 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 “right” 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 haven’t 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 “Y” to “A”. 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.
