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Multiple freezes and crashes on quite simple files...

Message 1 of 12
399 Views, 11 Replies

Multiple freezes and crashes on quite simple files...



For a few days, I experience a very important degradation of Fusion's behaviour. I asked it to put a 50mm dimension between 2 straight lines, and I have the time to open the forum, see if anyone already reported such issues, decide to post something and write it. As I finish this sentence, Fusion is still crashed. A Windows message popped up to ask me if - since the program is not responding - I want to close it or wait. I chose wait, and I still wait. Screen is all "transparent white":




This drawing is based on an imported DXF file. There's no body, no other component,... just 2 horizontal/vertical constraints and 2 (almost 3...) dimensions. Not sure it can get any simpler.


I was working on another design yesterday (one that I designed myself from scratch, without importing anything) a bit more complex but still, I'm an amateur hobbyist so all my designs are laughably simple, and Fusion totally crashed 3 times. In between, it froze, then recovered, then froze again before crashing.


Since it was working flawlessly before on the same computer, same OS, same everything, no major Windows update, it seems to be linked to Fusion, not to my setup. Other programs work fine, so I doubt there's any hardware issue.


Is anyone experiencing the same kind of issues?


Thanks in advance for your support


Edit: While I was finishing typing this message, Fusion recovered. I started a screen recording, then changed the - finally computed - 50mm value to 45mm, which caused a new freeze. I waited for more than 7 minutes before deciding to stop this very boring recording. 8-9 minutes later, Fusion is still frozen.


Tags (2)
Message 2 of 12

Can you share such a design?

Fully undefined (not constrained or dimensioned) sketches are always slow in Fusion.


Message 3 of 12

Here you go. As a reference, I also designed the second file for our bathroom (meuble_sdb_v2_splines1 v5.f3z) a while back, and even though it is full of undefined unconstrained splines everywhere, I never experienced such performances issues, not to mention full crashes


A few minutes ago, I had a warning from Fusion stating that the performance was degraded with a message I could copy to clipboard: here it is:


DISCLAIMER: Yes, I know, I work on a beast of a machine you're probably very jealous of,... 😄


[GPU Information]
GPU Device: Intel(R) HD Graphics 520
GPU RAM: 128 MB (Integrated card)
GPU Driver API: DirectX 9.0
GPU Driver Version:
GPU Driver Date: Unknown

[Graphics Effects Settings]
Anti Aliasing: On
Ambient Occlusion: On
Object Shadow: Off
Ground Shadow: On
Ground Reflection: Off
Selection Display Style: Normal
Transparency Effect: Better Performance

[Limit effects to optimize performance]


Message 4 of 12

"quite simple" is in the eye of the beholder, to misquote that famous saying.  This is a common problem with DXF and SVG imported designs.  This sketch contains 6518 very small line segments.  That is a lot of lines for the sketch solver to solve, especially if they are under-constrained. Here is a zoomed in view of one of the small closed regions (leaves?), with every other line selected in a small region:

Screenshot 2024-06-03 at 1.48.17 PM.png


If it were me, I would use this as a guide, create a separate sketch, and re-draw the curves using Fusion native curves.  You could probably get by with Arcs for most of those curves.  I suspect it would take 10-15 mins to do, and you would save yourself a LOT of waiting and frustration that would almost certainly add up to more than that 10-15 mins.


Jeff Strater
Engineering Director
Message 5 of 12

Isn't it weird to see "GPU Driver API: DirectX 9.0" even though dxdiag states that the installed DirectX version is DirectX 12?




Message 6 of 12

Well, this is good news (in the sense that it doesn't mean I have to buy a new computer just yet...), but I'm still wondering why this is happening on multiple design, including the one I include in this post


This one has basicaly no curves at all, no splines, and a lot of constraints. From what you say, I think that - as it  is often the case - the problem is in front of the computer, so I'd like to know what I'm doing wrong.



Message 7 of 12

What particular operations are crashing or freezing for you on this design?


I see this sketch:

Screenshot 2024-06-04 at 12.54.55 PM.png


It is all the symmetry constraints that make this complex.  However, even with all this, I did not see any operation on this sketch that takes more than about a second to complete (which is what I would expect for this level of complexity).


In general, people tend to try to avoid adding the symmetry in the sketch, but, instead, will model half of the shape in the sketch, and use Mirror on the solid to get the symmetric result, especially if the sketch is at all complex.  There are valid uses for sketch symmetry, but usually those are mirroring a fairly small number of geometries.

Jeff Strater
Engineering Director
Message 8 of 12



The specific action was trying to drag the left caster a bit more to the left. This led to a freeze and multiple "Finished computing" messages and the entire drawing going left and right (I clicked elsewhere to make sure I wasn't dragging it along with my mouse as I was waiting, as it already happened before).


I know that mirroring entities is not ideal, I ran into some issues with it already in the past, but here, I'm mirroring 2 drawers, 4 grooves and 4 sliders (well, rectangles that represent a slider),... I don't think it's something that should put Fusion in trouble... I would understand if I was mirroring half a car or building,... but it's not the case.


I do know that my computer is not  (by any means) a powerful machine, so I'd also be interested in knowing if upgrading to a faster CPU would help (something like "Unlikely - Maybe - Probably - definitely). CPU is an i7 6500U (2,5Ghz, turbo at 3,1 Ghz) and i run 8Gb of RAM but have no dedicated GPU (Intel HD520 - shared memory). From what I read about it, the GPU is not really involved in this kind of work, it's more about the CPU... WDYT?

Thanks for taking the time to try to troubleshoot anyway!

Message 9 of 12

@robertmarteau wrote:



I know that mirroring entities is not ideal, I ran into some issues with it already in the past, but here, I'm mirroring 2 drawers, 4 grooves and 4 sliders (well, rectangles that represent a slider),... I don't think it's something that should put Fusion in trouble... I would understand if I was mirroring half a car or building,... but it's not the case.


Many other CAD systems don't use their own sketch engine but license  the the D-Cubed Sketch engine from Siemens. Development of that sketch engine started 30(?) years ago and by now it is very fast and robust, but it is a pure 2D sketch engine.

All that speed and robustness has also lead to the undesirable effect that many, even experienced CAD operators have developed bad habits, of which many are apparent in this thread.


Fusions sketch engine is much younger and under the hood is a 3D sketch engine. That also means it isn't as robust or performant as D-Cubed. While that has some obviously undesirable effects, the lower performance requires folks to develop proper sketch habits.


These guidelines below are general sketch guidelines applicable to all parametric 3D CAD software, not only Fusion 360.


1. One sketch per feature.

Fusion allows to extrude more than one set of geometry from one sketch. Many other CAD systems don't. This can be very helpful, but often is overused and leads to performance degradation!


2. Fully constrain and dimension sketches.

Under dimensioned and under constrained sketches cause performance degradation as they have to be constantly re-evaluated for possible changes.


3. Limit mirroring and patterning in sketches.
Be aware of symmetries (before you even touch your computer mouse!!!). Design only half or quarter of stuff and then mirror, or pattern 3D geometry. This creates computationally more performant designs.


4. Limit fillets and chamfers in sketches and use the solid modeling features where possible.

Together with #3 this will result in simpler sketches that are faster to sketch, require less, or no debugging and as a result are much more robust.


Many folks get completely hung up on sketches because they don't understand what the purpose of a sketch in  a parametric CAD software is. 

The purpose of a sketch is not to create the full and final outlined of a discrete manufactured part.

The purpose is to create basic geometry to be further refined with 3D modeling features.  


Message 10 of 12

ah, drag...  Yeah, drag in that sketch is slow, even on my machine.  Drag is problematic.  First, it is compute intensive, second it queues up mouse movements, which end up with the behavior you saw, where it keeps reacting for a long time.  Not much I can add beyond what @TrippyLighting recommended.  I guess I would recommend, if you want to stay with this sketch, that you move things by editing parameters, not by dragging.  Not really acceptable, I realize, just what I would do.

Jeff Strater
Engineering Director
Message 11 of 12



Thanks for your input. I used to create more sketches in the past, like @TrippyLighting suggests as the best practice, but I ran into issues when modifying the design. 

If I create 2 sketches, when I come back to modify sketch1, Sketch2 doesn't exist (yet) in the timeline, so I can't use any of the geometry defined in it. That often causes issues, and I ended up solving it by trying to stick to "one sketch per axis". 


Any tip on how to work around this time travel issue? 😉

Actually, I think a big part of this is on me (not knowing/using best practices), but I would still expect Fusion to be able to drag a caster in a drawing that's still, IMO, quite basic (unless I'm mistaken here also). 

Message 12 of 12

@robertmarteau wrote:

Isn't it weird to see "GPU Driver API: DirectX 9.0" even though dxdiag states that the installed DirectX version is DirectX 12?


Have you gone into preferences and changed the driver Fusion is using? Default is Auto-Select and it should use the highest Dx available but you can force it to use one of the others.


Mark Hughes
Owner, Hughes Tooling
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