Hi All, I will upload one of the files when I get home tonight, thank you for the offers of help!
Attached are three files. If they don’t work let me know and I’ll post the public links.
These are three slices of the mesh from the engine of the overall model. For most of the mesh layers the carve will only be on the outside since I repair the slice to have a solid face on top (the exception being the engine inner cone and outer cone slices).
But you can see the plunges (something I didn’t really pay attention to before carving I guess) in two of the files. In the other you can see how it does the “corners” even though all the parts are round/oval shaped (and I have no idea why it chooses to do it this way).
Slices.zip (1.2 MB)
Appreciate your help!
One more update!
I think I found a way to make it helix in the corners every time. That’s by setting the boundary to boundary box with tool outside. Seems to be working on the test I have running right now.
If anyone thinks of or finds a better way let me know!
I had a quick look at your files. First question that pops up with regard to the head plunging down. I do see in your toolpath that you’re going straight down when moving to the next layer with the expected stepdown. But that doesn’t seem terribly wrong.
However, the stock material that you’re carving this out from, is that the exact size that you have defined in Fusion, e.g. width and length are already cut to size? Or are you using a bigger piece and are you cutting from that? Because if you’re cutting from a bigger piece than what’s in Fusion, it will indeed have some unexpected behavior as currently fusion believes it can come in from the side of the material and start cutting from there. If the actual stock is bigger, you’ll indeed have some more “unpleasant” contact with the material…
If you make that bigger, you’ll see that the result of doing an operation will be different because now Fusion knows that it needs to take into account the extra material when generating toolpaths, In this case I chose silhouette, in the attached file I ended up using bounding box.:
(Note that in this particular case I also assumed that the stock is 1mm higher than what you need, so you’ll flatten your piece in the same process.
slice-test v1.zip (851.2 KB)
The project file contains your original setup + two setups with larger stock material.
In both I’ve added first a roughing pass and next a pass to clean it up further on the sides.
THe first extra setup uses a 6mm end mill for the roughing pass and next the ball nose for cleanup, the second one does it all with the same ball nose to avoid the tool change. Then you can have it run as a single job which is also fine.
In the setup I didn’t just enlarge the stock, but also added a bit of extra height (1mm) to “flatten” the stock in case it’s not perfect. I wouldn’t recommend that if you only use a ball end, because you won’t get it really flat or you’ll need a lot of extra passes with minimal step-over. So in that case remove the extra height.
By no means the setup in the attached file is an optimal solution, but it should give you an idea on possible approaches.
Hope this helps
2 Likes
Hi Brvd,
Thank you for the detailed reply! I didn’t consider Fusion thinking about the side approach and I agree that more than likely has to be what happened.
The stock I’m using is 4 x 3.5 inch cuts of red cedar board. A few of the boards do have a slight cup but I haven’t been too concerned with it (at least not enough to add extra material to it). If time were not the factor it is for me I would definitely add the material as you suggested.
I’ll take a look at the file you re-uploaded and become that little bit wiser 
Thank you!!
In that case just set the stock top offset of the setup you want to change to 0.
And/or increase the stock on the side from your original setup. You’ll see that the results you had aren’t that different from what you had.
Another thing I like to do when you’re cutting out something like this is to use an additional offset in the geometry box (no matter if you choose silhouette or bounding box or whatever)
It’s not strictly necessary, but it will avoid that your cutting a full path in stead of having some extra space for your mill to pass along the sides. Especially for deeper cuts and some wiggling around of the cutter, this might create more resistance than what the SM can comfortably handle (you’ll get some kind of chatter and the end mill bouncing against your material on both sides.) This avoids that somewhat, this at the cost of some extra time. (you only need to do that for the roughing pass obviously, although Fusion will not cut into the air if you selected “rest machining” anyway.
PS: I do expect a post with the end result 
1 Like
Nothing really to add to what @brvdboss has said.
I assume your different setups are just various tests and you’re not trying to run them all.
-S