Fusion 360 not using all available system resources

[tsitalon1]

Hello !

I'm having an issue with some of my projects requiring 1-3 minutes to compute sketches and extrudes, even though Fusion 360 is only using 10-30% of system resources of my Windows 11 PC.

The concern I have is Fusion 360 is not using all available resources, so I feel regardless how simple or complex the model is, I think Fusion should be able to use more than 30% of my system resources.

Using an AMD 12/24 core CPU with a 3060ti and 32gb of ram.

I've searched and cannot find any setting that tells Fusion to use all CPU cores and all GPU cores to process models,  any way to do that?

[g-andresen]

Hi,

Like almost all CAD applications, Fusion uses only one kernel for most processes. This is perhaps understandable if you imagine that a fillet on an extrusion based on a profile created in a sketch cannot be processed in parallel like the basic profile sketch.

Günther

[tsitalon1]

I'm not a programmer, so I'm not sure i understand why Fusion cannot use more CPU/GPS cores.

I have a model of a double sided drink coaster that only has 31 items in the timeline, but does contain multiple SVG's imported and many sketches and it's choking on them, the program has crashed multiple times and when it doesn't crash it takes 1-3 minutes for every change I make.

I don't claim to be a Fusion expert, but if your users can crash you application or make it slow to a crawl, that is not a good thing on machine that has 10x the resources they state are the minimum.

Super frustrated.

[lance.carocci]

Some operations currently happen in the same thread as the UI, causing the appearance of a deadlock, which is likely what you're experiencing. We have refactored many of these over the years, but some remain. The result is that some operations will hang the UI until they complete - it's the equivalent of Fusion 360 thinking so hard that doesn't realize it's making an ugly face in the process and everyone can see it.

Modeling operations tend to be single-threaded calculations that benefit from clock speed; simulation and toolpath generation workflows tend to be multi-threaded and benefit from extra cores.

The current behavior will eventually be replaced. We know how much it annoys folks when the UI fades white or black and goes unresponsive under load - it's not an easy fix, but one we're working on.

Ultimately, our goal is not to consume more of your resources - it's to do more processing with fewer resources.

[jeff_strater]

please share examples of the SVGs you are using.  My guess is that they contain a very large number of short curves.  This workflow is not recommended in Fusion.  Fusion sketches are designed to use a relatively small number of curves.  You will have better luck with smaller sketches.  If you are interested in having a better experience, I'm sure we can help

[tsitalon1]

You are correct, the SVG's and sketches do contain a lot of small curves and circles, but I'm forced to work with these are they are customer requested design elements.

I cannot share the F3d file as it's a commercial product for a customer, but can you tell me what options I have to resolve it now that these sketches are on place and contain all these small curves ?

[jeff_strater]

There is only so much you can do, to be honest.  First, you can try to separate geometry into as many sketches as you can.  For instance, if there is an outer boundary, and then a lot of interior cutouts, you can separate the interior cuts into one or more separate sketches.

You can also try importing the SVG, then editing the resulting sketch, selecting all the sketch curves, and use the Fix command to lock all the curves in that sketch.  This gets to one of the underlying cause of the slowness.  Fusion is a constraint-based sketch environment.  Every curve and point's position is computed with a solve of the sketch (which is also single-threaded), even if there are no constraints and dimensions.  Once you have thousands of curves, that can take a significant amount of time.  However, if you "Fix" those curves, that tells the solver that these curves are not going to move, so it can just ignore them in the solve.

Another possible cause of slowness in sketch is profile recognition.  In the sketch palette, there is a "show profile" option.  See what happens if you uncheck that.  It can sometimes take a lot of time to determine the number of regions in the sketch.  Leave it off until you need those profiles for Extrude, etc.

You can also use the SVG as a guide, and create native curves in Fusion by tracing over the SVG.  Depending on how complex it is, that can be a surprisingly effective method.  If it takes you 10 minutes to trace over a design, but you are seeing 3 minutes per operation, it only takes 4 operations for the time to trace the geometry to more than pay for itself.

Finally, ask the customer about their process - where did the SVG come from?  I know that some drawing packages such as Adobe Illustrator have options, both on the creation side, and on the export side, to generate fewer, bigger curves, instead of lots of tiny curves.  If a drawing is being used for display purposes only, it doesn't matter so much, but if it is intended for a CAD package like Fusion or any other "precise" CAD modeler, fewer curves is better.

[tsitalon1]

Thank you for your detailed explanation, I will try "Fixing" all the sketches to see if that helps!

Once last thing, my latest changes broken something and I cannot tell what, nothing looks wrong in Fusion, and a compute all command does not list any errors in the timeline at all, however now when I export the model to Step format and import into my slicer (bambu studio) I'm getting manifold errors.

Any way to find these in Fusion ?