Slooooow Sketch

[etfrench]

Fusion 360 is processing sketch actions extremely slowly in this sketch: http://a360.co/1WMXXvj

Here is the video: https://knowledge.autodesk.com/community/screencast/e40970f7-aafd-4a2d-b73e-2ad6bb489610

The machine has an Intel i7-6700 CPU @2.4Ghz and 16gb RAM.  Taskman shows memory and CPU usage are low.

Also note the second fillet is not created correctly.

This sketch was originally created in another model and was copied to this model to see if Fusion 360 would be more responsive.  Unfortunately, it was not.  The sketch was the only thing copied from the original.

[innovatenate]

One tip is to right click on the sketch and select Hide Profile. This will help with performance for large sketches, or sketches with complex boundaries (e.g. splines for outlines).

Another tip that will help is to split the sketch up into multiple smaller sketches. If you imported this sketch via a DWG file, you can use layers to help split up the sketch. Take a look at this version of the file where the sketch is done in smaller parts. Note that I created multiple layer sketches by adding sketch entities to different layers in AutoCAD and then importing the DWG into Fusion 360.

http://a360.co/1QB50qq

Fusion 360 is using a constraint based sketch environment. There is more than meets the eye when looking at a sketch. Each sketch entity can have many relationship governing its behavior.

What application did the design originate from? Was it a 3D design or always a 2D design?

I hope that helps.

Thanks,

[etfrench]

The original was imported from a dxf file, although very little is left from that.

Eventually, when it's fabricated it will look like this:

The individual components are from the manufacturers and the layout is my design.

I was able to get Fusion 360 to be responsive again by exporting the sketch as a dxf, then importing it back.  The one oddity was the imported dxf was a mirror image.

There does appear to be some artifacts from the original drawing in the sketch only model which may be contributing to the slow performance.  The Data pane appears to show other components instead of just the sketch.

[TrippyLighting]

What is the purpose of inserting the actual PCB copper layout in a more or less mechanical design?

Or did you use F360 to position the components and then developed the layout to match that ?

That looks like an Teensy 3.x if I am not mistaken(?)

[etfrench]

A little bit of both.  I used Fritzing to generate a schematic and general layout.  Since the Teensy 3.2 has pins on 3 of the 4 edges and also on the bottom, it's hard to get all of the pins exposed on a single layer board. Fritzing was showing errors for traces too close together and I haven't used it enough to determine how to eliminate the errors.  I took the layout from Fritzing and entered it into my 2D cad program.  After loading that into Fusion 360 to verify the components fit, I discovered the they weren't exactly the size I was expected, so I had to move a few (lots) of them around.  I also needed to make sure all of the traces were at least .009" wide and .010" apart.  I'm planning on etching the board, so I also wanted to keep the board covered with as much copper as possible.

After making three or four revisions, Fusion 360 started to take lots of time to do any actions even though memory and CPU usage was well below 50%.  I guess it shouldn't be surprising as there are 4600+ objects in the sketch 🙂

[joncolinleonard]

Excuse me for inserting myself into this conversation, but I was just struggling through creating a custom, graduated, voronoi pattern for a structural steel support. The app that generates voronoi patters wouldn't deliver the results that I wanted, so I set off to create my own using the sketch tool. The workflow is to create the spine of the pattern, then meticulously offset the interior shapes with the offset tool, then remove the spines, then extrude the positive shape.

The problem is that a short way into creating the spine shape, I began to experience 2-4 second wait times for Fusion to  calculate all of the relationships and place the lines. Since I am placing several hundred lines, this wait state became painful. I attempted to launch the "hide profile" state as suggested here, but this is not a function that is supported in my current release. What DOES work is to use the "Fix/Unfix" tool on groups of points as the performance slows down. Since I am only partway into the process, I have no idea what Fusion will do when I attempt to extrude a solid from such "complex" geometry, but I am keeping my fingers crossed. The images show the overall layout, and the "fixed" points which brings the sketch speed back to normal.

[jeff_strater]

Hi @joncolinleonard,

Your approach is a good one:  Fixing geometry when you are done with it will definitely speed up the solve.  The solver knows that it can just skip right over those.  Good tip for others to know.

You do have the "hide Profile" option, it's just named the other way around:  "show Profile":

If you uncheck "show Profile" it will hide all the profiles and suppress profile calculation.

Jeff

[joncolinleonard]

Thank You!

I also found the show/hide profile command in the sketch dialog console.

Best Regards,

Colin

J. Colin Leonard, IDSA Consulting
941-586-6701

Sent from my iPhone

[Anonymous]

Hi!

Lately, I am also experiencing major slowdowns even during simple sketch operation like the one You can see on the screenshot. It would perfectly understandable If my model would be complex, but it really isn't and it's a second time I am experiencing this kind of behavior during modeling. Last time was about two weeks ago when I was working on a model of not very different complexity. 

I believe it's a bug because all the rest runs very smoothly all the time, even when I am creating way more complex models. 

Please take this into consideration 🙂

P.S. - "Show Profile" trick do not solve the problem in a slightest. 

Cheers

Lukasz