Fusion
Some processes are multi-threaded, some are not. So for some calculations, Fusion will only be able to utilize one processor at a time which is why you only are using 16 percent. Try running a local simulation solve and see how many cores light up on the computer.
I'm guessing you are using one of those features that is not multi-threaded.
It might help to elaborate on what you're doing or were doing when the Fusion starts chugging away. There may be another way to achieve what you're trying to do. Sharing a design or screenshot could be helpful. I'm happy to look and make recommendations.
Thanks,
Nathan Chandler
Principal Specialist
Can you share a screenshot of a design that requires 350k quad polygons ?
A fairly detailed quad mesh can have a couple 10k faces, but 350k sounds like an unreasonably high poly count.
A T-Spline in Fusion 360 might model similar to a polygon mesh, but a T-Spline is mathematically and thus computationally much more involved than a polygon-mesh.
NURBS related geometry creation is handled by he geometric modeling kernel and is not easily broken up into parallelizable tasks.
With what tool will you cut the seriously fine detail that is represented by his seriously one mesh ?
Have you done some back-of-the-envelope calculations to see what level of detail you can machine (tool radius) and what mesh resolution you need to represent that level of detail ?
You did not answer my question. Have you done some back of the envelop calculations to see what mesh density is needed to re-create the geometry with the machining tools at hand ?
The aim would obviously be to reduce the mesh count to the need, not keep it as hight as one possibly can and then wonder why the software slows down. Thus what you have produced could possibly overkill in terms of mesh density.
The question is how to do more with less.
So first of all, you should have created a separate thread. While you might feel you see the same symptoms, the root cause is completely different.
Your design has one sketch. You created a polygon and hen I assume you used the move command to multiply that sketch geometry.
The 1st mistake here is that you did not fully constrain and dimensions the 1st polygon.
The 2nd mistake is that you try to pattern the polygon by using the move command. A hex pattern can be read using 1 polygon and 2 feature patterns. No pattern should be created in the sketch at all.
The third mistake is that instead of dimensioning the location of the 1st polygon to lock it into place you used the fix constrained on the copy-pasted pattern of 8 polygons.
The 4rth mistake is that then you must have used the copy/paste command about 20-30 times to create more instances but you could not move these instances because of the applied fix constraint.
So now what looks like 6 polygons is really 6 x 30 (or so) unconstrained polygons.
And THAT absolutely kills the performance of the sketch solver. It is also compelt3ely avoidable bt using proper techniques. Create a polygon or two in the sketch. Extrude and then pattern the feature or faces.
Edit: MIstake #5 the design has no timeline! Not at all recommended for beginners!
That quad mesh looks like a mess. What software did you use for re-meshing ?
In essence the edge flow is very bad resulting on very many poles (star points in t-Spline lingo). This will create a very complex T-Spline, which is not needed for this relatively simple geometry.
A manual re-topology workflow would likely create a much better outcome.
Can you share the original (triangulated) mesh file ? (zip and attach)