Understanding Fusion 360 Bottlenecks

[Anonymous]

So I've been having degraded performance in Fusion lately and I'm attributing this to improper design practices. The issues I've been having are as follow: constant crashes when making simple edits, for instance simply clicking on an edge will trigger the program to freeze and completely crash. I'm not sure why this happens.

I'm currently making a simple part with a cube shape framework, when I designed the cube features I had no problems. However this cube houses a very intricate piece inside of it with sketches that have more than 500-1000 elements (individual lines).

Once I started stacking sketches (I currently have about 8 sketches in this project) the performance dropped like crazy. Using basic features such as inspect/measure become very cumbersome (takes about 5 seconds for it to compute the length of a simple line) and often times the measure tool itself will result in a crash.

Can someone shine some insight on how and why this happens and if there are some best practices to avoid these issues in the future? Thanks in advance!

[PhilProcarioJr]

@Anonymous

Honestly, without seeing your project first hand it's hard to say how you can make this more responsive. But knowing what I do about sketches in fusion I have learned to make sure each of your parts and it's associated sketches are in their own component. I never use complex sketches in one sketch. I break them up so that my sketch only has what's needed for that one part or feature. The sketch engine in Fusion can not handle 500-1000 elements in one sketch right now. They are working on improving the sketch engine but still that's a lot of entities for one sketch or even a few sketches (Again I don't even know how many sketches contain this amount of elements). Use feature and body patterning instead of sketch patterning when ever you can. I'm sure there is more but this is all I can think of right now and without seeing your project.

[Anonymous]

That's great information, exactly what I was looking for. Thank you for clarifying the engine's capabilities.

I was advised by another member to begin using pattern profiles as well, I'll make this a regular part of my workflow from now on! I'll also do exactly as you suggested and keep sketches specifically for features (great idea).

Thanks again for the info!

[cekuhnen]

@Anonymous

I hope this video makes sense:

https://drive.google.com/file/d/0Byzv_NlyKp_2TnRFWDZveFduVFE/view

I follow the basic process:

1. keep sketches as basic as possible

2. add details like edge rounding/fillets via solid or patch modeling tools instead

this keeps sketches nice a slim and they react faster

in addition sketches are easy to read and manipulate

the more you add to a sketch the slower the solver will be because it has increasingly more to deal with.

Nice side effect is sketch only for example offers G1 fillet, patch and solid fillet tool also offers G2

[Anonymous]

Understood, thanks for the information.

Do you guys know if the number of sketches within a project will cause issues? For instance, I have 10 sketches (hypothetically) and I only have one visibly active. If I make edits to the model for any reason does the program also need to take into account the hidden sketches or are those outside of the computation queue?

[cekuhnen]

the sketch engine is rather slow with heavy sketches when editing them but not when just seeing them.

[Anonymous]

Interesting, my sketches have been consolidated and are hovering around 500-600 pieces (not currently seen or active) but when I use tools such as "measure" the delay is immense.

[cekuhnen]

@Anonymous Fusion's 360 UI is not the fastest one to be honest.

Can you show a screenshot of what you are looking at?

[Anonymous]

Sure, I just attached it. I'm sure you can notice the channels on the face of the interior block. That's where all the complex geometry is located. The sketch for that geometry contains about 600 pieces in its current state.

As an example I just tried measuring the corner on the exterior of the block and that took about 2-3 seconds to compute. 😕

[cekuhnen]

https://drive.google.com/file/d/0Byzv_NlyKp_2emxlNDV6Q0NqRms/view

did you build it this way? or do you sketches inlcude all the data for the boolean cuts?

[TrippyLighting]

Instead of pattening sketch items, you should create these feateurs as single 3D features and use "Create->Pattern" to create patterned 3D features.

this will keep the sketches light and Fusion 360 performs better.

[Anonymous]

Hi Trippy, I the intricate geometry was created this way. I only sketched out one of those channels and used the pattern tool to duplicate the negative extrusion.

[Anonymous]

cekuhnen, your upload is still loading so I'll be sure to check it out in a second but I did it like this:

One channel (the long horizontal channel) was made making one sketch and duplicating the extruded pattern.

The cross cuts (rectangular in shape) are in their own separate sketch file which are simply long rectangles. Besides that the only existing sketches left are those of the general shape (box).

[cekuhnen]

@Anonymous

could you share the file s I could load it here and test the speed?

info@ckbrd.de

obviously I will not share it

[changedsoul]

Just to toss out another reason for poor performance I recently came across. My Fusion was lagging big time making minor edits in a very simple project, it was also hanging when trying to rotate the design and look around at it.

What I found, my wifi was acting up, and after a while of fusion acting up, I noticed I was bouncing back and forth between online and off line and wasn't aware. This was causing all the issues (for me). So just a heads up if it happens so someone else, I went into offline mode until my internet connection got better.

I know this isn't related to what was happening here in the OP, but it did degrade performance and I wanted to toss it out there.

[Anonymous]

That's a great point as well, I might consider working in offline mode from now on. I've been having a lot of issues with updates being performed in the background interrupting my work.