Assembly performance below level shelled body

[thijs_976]

Hi, 

since I'm working on an assembly of a machine part which contains shelled components, my daily schedule is becoming a mess.

The assy contains between 50-100parts, and even when i turn of 90% of the parts, making an edit on whatever component in it will give me a good coffee break. Which is nice, but after 2 coffees and 2 minor chamfer changes later I would like a faster workflow in order to make it home in time.

I would like to share the file in confidence, so you can take a look at improvements i can make on editing the design. 

I'm working on a HP Z-Book 15u, with i7 and 16gb of ram, solid state disk... etc. so not an under-designed machine for this kind of assembly. 

Most of the components are related to each other. although not always that much.. but a minor change on something irrelevant can blow op the entire machine/part. How to prevent this sensitivity? 

Right now, it is like fixing thing again and again, and after 2 weeks of making changes... there are a ton of unclear changes, added extrusions, removed faces... not really beautiful of I would have to share this with a co-worker. 

By the way, I have the impression Fusion is continuously making me wait for an Auto-save action, while he should do this once every 5 minutes. maybe it's because he's making me wait 4 minutes for every feature edit, but this starts to be annoying as well. Still I don't want to risk putting it at larger time intervals since fusion is crashing from the moment it starts turtelling and I have the balls to click the mouse again.. I'm a bit in a dilemma over here 🙂 

[kate.raskauskas]

Hi @thijs_976,

If you'd like to PM me the share link for your design, I'd be happy to take a look at it!

[TrippyLighting]

It is unlikely that the problem is hardware related. A 100 component assembly is not a large assembly by any means.

If you can share your design that would be very helpful. The best way to do this with assemblies is to create a public link from the design in the data panel.

Do you have any T-Splines or Contact sets in your design ?

If you have contact sets, delete them!

[thijs_976]

Hi Kate, 

did you have the chance to take a look at it? 

thanks

[thijs_976]

Hi, 

thanks for your reply in PM. 

The handle is made by a sculpt,combined with a sketched part which has multiple operations. 

fe, take a look at the red "lenshouder 2D". You'll see the holes are misalligned, while they were designed perfectly 2 weeks ago. 

To use this part and make iterations, I am forced to use the exported stp. file I sent to the manufacturing department and make my changes on the "dumb" stl. There 's just no way I can recuperate this "lenshouder". one reason is I don't understand how it has lost the dependencies, another reason is the extreme slowliness of fusion taking 10 minutes for every trail and error step I make to solve the faulty drawings in the part. 

Another thing, take a look at this picture: 

there is clearly something wrong with this cut-out. It should look like the second picture. 

How this changed, I have no clue. it had nothing to do with all the changes I made on the handle or lensring.

It's making me frustrated these things happen, since I have to check every tiny aspect of my part (all the parts) after making a change to whatever. This is stressful, since sometimes it's just a small detail you don't even notice. 

[TrippyLighting]

I've looked at your design and frankly If you sent this to manufacturing now would be a time to be worried!

Have you ever run a Modify->Compute all" on any of the models you designed for this project ?

I just did and this is the result:

Your model is severely broken. The 43 warnings indicate yellow icons in the timeline that went long with a waring message in the lower right corner of the Fusion 360 viewport. Yellow means Fusion can proceed but only with cached/old geometry, meaning that changes you make in the timeline before these warnings occurred ate possibly not calculated and propagated through the timeline.

The red icon indicate errors on feature Fusion 360 cannot find a solution for.

Any of these warnings errors should have been observed and properly responded to at the first occurrence!

It is a dangerous practice to continue working with such an amount of warnings and errors in the timeline. 

That is most certainly one of the reasons your model computes so slowly as Fusion has to try to find a solution for all these broken features in the timeline just to find that it cannot. That simply takes valuable calculation time.

As I've mentioned in my reply to your private message, having a T-Spline in the timeline and than edit it and shelling it is a really bad idea from a performance standpoint. I am aware that Autodesk marketing views promote that rubbish but that also is a dangerous practice! 

[thijs_976]

Hi,


thanks for observing this assembly.

I do realise this is a very bad situation. my problem with these warnings is that if I'm trying to go back and "heal" the sketches by changing the references etc. it is just impossible to do so because of the low performance. In fact, from the moment it goes wrong and 10 of these errors pop up, I have no chance in correcting them since it's a hopeless amount of time being lost.


What bothers me about this, is that fusion does not warn you if you finish a sketch with sufficient links or constraints.

Then, when making a slight change to fe. the T-spline which is a freeform and is not used as reference for many things, or just by dragging or turning the model, these sketches get messed up. As you know, when changing things in the beginning of the timeline, with a complex model, a bunch of errors will occur. I believe it was the low responsiveness of fusion which kept me from correcting these yellow sketches.


Any advise for me what to do? Run through the entire modeling tree from beginning till end?

Even when I did not have errors, Fusion was freaking me out...

What would your advise be if you have to make a freeform? Do this in a seperate file and import the part as a STP. file?

[TrippyLighting · Accepted solution]

In order to give you any advise I'd have to have much more information and advise would have to be an interactive 1-on-1 coaching session.

I've gone through your design and you create many sketches to create geometry, then you create new sketches on that new geometry to create more geometry. You create dependency upon dependency and in many cases that is unnecessary and would slow your design dow,

You split of bodies, that linger around in the component, but are not used anymore, so they should be removed.

You have a good number of suppressed features so far back in the timeline that there is no hope of un suppressing those without breaking more stuff.

My first steps would be to figure out what parts are complete, or complete enough, so they could be exported into there own files and export  them and see what breaks an fix it.

[thijs_976]

Hi Peter, 

You are right about the dependencies. In the past I used to create every component in a seperate file, and make an assembly in the final stage by joining all seperate files.

Now I must say I was amazed by the ease of workflow fusion 360 offered with creating components inside assemblies. The dependencies are a great help, but they can turn out to be a b*tch as well if you did something only 95% right. 

In my next design, I'll try to keep my focus on avoiding dependencies by just dimensioning sketches I can create myself. Or the parts which are dependent and not possible to create without dependencies, I can make them in separate files and join them later on. So if something goes wrong, It's just a part of the assembly which gets messed up. 

This sounds easy and a straight forward best-practice. But it is quite difficult if you're in the "creation process" and you want to have to complete picture of what you're designing from the beginning. Like the handle.. I cannot make this in a separate file since it is extremely dependent from the machined parts inside... 

This approach is easy from the moment you know exactly how your assembly will look like, how the components more or less will look like and which ones are related to each other, but how do you achieve this workflow from the first move you make? I always seem to mess up the model-tree after some inspirational inputs and new creations. then I have to start over and create structure. Are there some good and specific tutorials on this how to create structure, even when you don't know how many parts you'll have to create? 

Thanks already for pointing me on the failing model tree, you're absolutely right about that.