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geekhack Projects => Making Stuff Together! => Topic started by: GSV-CargoCult on Tue, 07 January 2020, 06:46:18
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Can someone help workout why Fusion 360s performance drops off a cliff with my plate model? I get freezes and black areas in the component browser every time I try to add a new horizontal construction lines or add a sketch dimensions. Initially tried using Swill's plate builder and importing as a DXF into F360, but ended up with similar performance issues.
FWIW I've tried this on a couple of different PCs: My laptop i7 8650 2.11Ghz w 32 GB ram, SSD but inbuilt intel GFX and my home machine with a mid 2017 i5 16GB RAM, SSD and a GeForce GT 710 2GB
I presume it's something to do with the keys with stabilizer holes. Any help is MUCH appreciated!
https://a360.co/36yxUTs (https://a360.co/36yxUTs)
Edit: Sorry just realised the model hadn't uploaded, all sorted now!
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I've used multiple CAD software packages including Fusion, Solidworks 2013-2018, Siemens NX 11, etc. etc. and the one thing they all had in common was their inability to cope with plate sketches. All of them had severe lag, stuttering or freezing issues beyond a certain number of lines. I've heard other people make the same complaint as well, so you're definitely not alone.
I was never able to fix the problem fully, but upgrading my GPU certainly helped. That could be your issue since your GPUs are relatively low spec; the viewport will usually be rendered via DirectX or OpenGL.
If it's really unworkable then my best recommendation would be to do as much of the plate design as possible outside of Fusion, for instance in a 2D CAD package or even in a vector editor, then export as DXF/DWG. Import that and extrude. Once you're out of the sketch you shouldn't have an issue.
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Thanks, appreciate the response. *sigh* that's a shame. I suppose I was worried about the sizes on SwillKBs DXFs not being round eg 13.9999999999 so started adding some constraints to force it.
Maybe I'll go back to just using them. I know the Toad used SwillKB to design the plate so I suppose it should be fine given machine tolerances.
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Been using LibreCad for my plate stuff recently. Very lightweight and fast for 2d work so far. Also, free free free.
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I suppose I was worried about the sizes on SwillKBs DXFs not being round eg 13.9999999999 so started adding some constraints to force it.
Try ai03's plate generator (https://kbplate.ai03.me/). I haven't used it myself but I've heard it fixes issues of rounding.
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I've had success improving Fusion performance on defining sketches by employing a good few "best practices". Note these definitely won't fix anything lol. Fusions not well optimized for this it crashes/buckles under the pressure of some sketches.
Here's my tips:
- Avoid defining objects using too many dependencies. Dependencies meaning like X is perpendicular to Y, which is also parallel to A, B, and D. These are what the system has to mathematically work through when you define new dimensions or dependencies.
- Avoid defining new dependencies that already depend on a lot of other dependencies. Said another way, define dependencies in small batches. For example if you have a group of 6 rectangles (like in a plate) that you then define as being colinear to another group of 6, fusion will hate that and usually crash/stall. Define it in two batches of 3, that makes it easier on the system.
- Employ a conservative amount of fixed parts. I really try and not fix anything in CAD, it's bad practice, but it can help with improving performance/minimizing crashes.
Also, +1 for AI's plate generator. It fixes the issues of rounding!
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Have had great success with both swill and aio3. Aio3s does indeed make the prep machining easier as you can choose to add those corner fillets instead of having to do them manually with swill.
I have found(on my surface book) that fusion performs MUCH better in general when it’s using the nvidia gpu vs the integrated gpu.
So I echo the advice about gpu.
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avoid putting ALL your key openings in one sketch,
My workaround is before I do anything, I put common dimensions in the User Parameters like:
MX_opening = 14.00mm, U_spacing = 19.05mm, etc...
then pick a specific spot and constrain it to the origin, upper left corner of the ESC key, for example, and start the sketch, and put your only necessary keys dimension-ed in terms of multiples of U_Spacing (e.g. 2*U_Spacing) to that spot.
For your layout I would only include 1U openings for:
ESC
Tab
Caps
LShift
LCtrl
(Split)Space(s)
The few keys right of Space
BS
Enter
backslash
RShift
Arrows
Column on the far right end and the 2 upper right keys
A second sketch of the stabs, hit P to reference the locations of the first sketch and snap the stabs to them.
And a third Sketch consist 1U openings of:
F1 F2 F3 F4 (or F1 only)
1
Q
A
Z
Then a forth sketch for the plate outline
Make the plate, extrude all the openings from first and second sketches except LCtrl.
Extrude again for Ctrl and use Pattern Features
Direction to the right
Count: 3
Spacing: 1.25*U_Spacing
Repeat the same for F1/1/Q/A/Z
THEN you can make a new sketch, project the actual shape of your plate and export your DXF if you need to.
Yes it's freaking tedious.
No don't do pattern in sketches, or at least avoid if possible.
Same as above, leave corners sharp and do the fillet to the solids as editable features, not sketches.
It's actually good to fully constrain your sketches.
Plan your "operations" beforehand and try to do it wisely.
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Thanks again everyone.
+1 for using user parameters for MX_Opening and U_Spacing
I tried using AIs plate gen for rounding, but haven't had any luck with it supporting multiple layouts (i.e. both ANSI and ISO)
@katotaka- I'll give that a try and see how it goes
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That’s odd. A keyboard plate should be easy for fusion to handle. It’s hard to help without seeing what you’re doing. Autodesk allows you to share a model using a public link:
https://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/sfdcarticles/sfdcarticles/How-to-share-a-Fusion-360-design.html
That said, there are tons of things that can slow it down. A common one is the rendering mode. If you turn off the shading, for instance, the speed can often double. Try minimizing the number of features. If you’re cutting 120 switch cutout, it is much faster to select all the cutout sketches and perform a single cut. Inversely, you can select everything that’s not a cutout and perform a single extrusion. Finally, make sure you have you’re video drivers up to date. Fusion offloads a lot of the rendering to the graphics card. Don’t even thing about running it under a Virtual environment, since the virtualized drivers are much slower.
Hope that helps.
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Hi there,
I design my plates with fusion sometimes. When I have started I was having a lot of issue in term of perf. I have tweaked my fusion a little bit but the most important thing for me was to understand a bug on the copy / paste sketch section feature. Maybe you use the same process, maybe not.
Basically, when you make copy / paste, even if you cancel the paste modale the copy of the sketch isn't cancelled so you need to ctrl + z manually. If you don't : It result of many duplicate dot / lines / contraints that break the perf of F360.
Here is a topic that show the bug in video : https://forums.autodesk.com/t5/fusion-360-support/how-to-remove-thousand-duplicate-comportement-of-the-c-p-cancel/m-p/8645322#M48925
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Hi there,
I design my plates with fusion sometimes. When I have started I was having a lot of issue in term of perf. I have tweaked my fusion a little bit but the most important thing for me was to understand a bug on the copy / paste sketch section feature. Maybe you use the same process, maybe not.
Basically, when you make copy / paste, even if you cancel the paste modale the copy of the sketch isn't cancelled so you need to ctrl + z manually. If you don't : It result of many duplicate dot / lines / contraints that break the perf of F360.
Here is a topic that show the bug in video : https://forums.autodesk.com/t5/fusion-360-support/how-to-remove-thousand-duplicate-comportement-of-the-c-p-cancel/m-p/8645322#M48925
Bug or not, every time you use paste in fusion it does a two-part operation:
1. actual pasting your thing in the same space as the original
2. a free move operation that doesn't register capture position afterwards
so make sure you undo TWICE if you feel the need
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Without looking at how you constructed the model, the less features you use, the faster it will render. Also modeling flexibility is counterbalanced by performance. The more you opt for having Fusion360 calculate coordinates and sizes, etc. the slower it will perform. Finally, some features are more calculation intensive than others.
Check you model and make sure all of the holes and cuts are done in as few feature operations as possible. The simplest way is to sketch all of them in a single sketch and then extruding only the plate area. Such operations are less taxing to the renderer than extruding the entire plate and then performing the hole and cut operations separately.
Finally, you can dramatically increase Fusion360's speed by keeping turning off as much of the rendering as possible such as shadows and detail level.