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Are you selecting a face when you create a sketch? If you are all the edges of that face are auto projected in so you could end up with hundreds of curves in the sketch before you start. There are 2 workarounds, create a plane on the face then select for your sketch or turn autoproject off in preferences. You might want to turn off Auto project on reference as well. With auto project off you will need to project in anything you need as a reference but it does keep your sketches a lot cleaner.
Mark Hughes
Owner, Hughes Tooling
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I think it comes down to the sketcher is constantly looking for and trying to add constraints as you draw. @innovatenate can you help?
Thanks Mark
Mark Hughes
Owner, Hughes Tooling
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For the sketch you showed in the Screencast, it looks like there is a lot of model symmetry that you may be able to take advantage of. Instead of projecting everything into the sketch, might it be possible to simplify the sketch and then mirror whatever features or geometry you need to create in 3D?
Contributing factors for the performance of Sketches are the options at the top of the sketch palette:
Disabling 3D, snap, grid, profile, constraint and point display will help since all of these little features requires some computation.
Another thing I'm wondering about is does the sketch need to maintain the associativity to the source geometry? If not, then you could right click on the sketch figures, select break link to break the associativity. Creating associativity between 3D geometry and sketch entities is another thing that might lead to the sketch performance.
In the design that was imported, how many bodies do you have per component in the design? I'm wondering if the issue is that you have like 1000 bodies in a single component somewhere in the browser.
It might be worth a test to use activate a component to see if it can help to filter down some of the design. If you activate a component (maybe one with only a single body in it) and then try to project a sketch, is it any faster?
Another helpful trick is to select all the sketch geometry and select Fix. This should help to "lock down" and reduce the computational overhead of creating new sketch constraints.
I hope that helps!
Nathan Chandler
Principal Specialist
Hi Norbert,
yes it's painful to watch Fusion taking so much time when this really should not be the case.
Would you be willing to (or able to) share you design with us so we can have our sketch development team take a look at and figure out what is slowing you down?
you can private message me here or email me at jamie.gilchrist@autodesk.com.
hope this helps,
Jamie Gilchrist
Principal Experience Designer
Jamie Gilchrist
Principal Experience Designer
Hey Nathan!
First of all thank you for the reply and the input you gave.
For the sketch you showed in the Screencast, it looks like there is a lot of model symmetry that you may be able to take advantage of. Instead of projecting everything into the sketch, might it be possible to simplify the sketch and then mirror whatever features or geometry you need to create in 3D?
-> The sketch is by far not complex, see the screenshot of a construction with a much more complex sketch were I'm experiencing no performance problems. I still do not understand what's the problem with complex sketches - it is a line drawing and with current computational power (talking of over 2,5GHz and 16GB RAM) it shouldn't be a performance restricting factor!
Disabling 3D, snap, grid, profile, constraint and point display will help since all of these little features requires some computation.
-> No improvement at all!
Another thing I'm wondering about is does the sketch need to maintain the associativity to the source geometry? If not, then you could right click on the sketch figures, select break link to break the associativity. Creating associativity between 3D geometry and sketch entities is another thing that might lead to the sketch performance.
-> Yes, i need the association to the source geometry. And I do not like the idea that i have to draw my sketch all over again when i change something in the source geometry.
In the design that was imported, how many bodies do you have per component in the design? I'm wondering if the issue is that you have like 1000 bodies in a single component somewhere in the browser.
->The imported design is a plastic case enclosing two sandwiched PCBs. The PCBs components exported from Altium Designer and they together contain about 3900 bodies. There are also 650 Unstiched geometries in one component. I tried to delete them (selected like in the screenshot), suspecting them being the cause for the bad performance, but it was not possible without loosing all other bodies too.
It might be worth a test to use activate a component to see if it can help to filter down some of the design. If you activate a component (maybe one with only a single body in it) and then try to project a sketch, is it any faster?
-> Here is a screenshot of the construction tree. Can you please give an example. "B150_SIP_Modul" is the imported design, it was an NX assembly. Every component has only few bodies, max. 3, except "SMV01-V21" and "SMP01.V21", which are the PCBs (~3900 bodies + 650 unstiched)
@JamieGilchrist: Thanks for the reply. Unfortunately I'm not allowed to share the design, as it contains customer data which we signed a NDA with.
Thank you for your help!!!
With all those unstitched bodies have you tried switching to the patch workspace and trying to stitch them. If they should form more than one body stitching could be tricky though.
Mark
Mark Hughes
Owner, Hughes Tooling
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@n.ebner wrote:
It might be worth a test to use activate a component to see if it can help to filter down some of the design. If you activate a component (maybe one with only a single body in it) and then try to project a sketch, is it any faster?
-> Here is a screenshot of the construction tree. Can you please give an example. "B150_SIP_Modul" is the imported design, it was an NX assembly. Every component has only few bodies, max. 3, except "SMV01-V21" and "SMP01.V21", which are the PCBs (~3900 bodies + 650 unstiched)
Thank you for the detailed response.
The below screencast clarifies what I'm trying to suggest with activating a component. I'm not 100% that it will help, but I thought it might be worth a try.
It sounds like the root of the issue may be simply the number of bodies in the design. 3900 is a lot of bodies, especially for an imported file. My guess is that there is something you're doing that is causing Fusion to have to run through all of the bodies loaded in memory. If you imported something and it didn't stitch into a solid, try starting by solving the interoperability issues, first.
If you could simplify 650 bodies into a fewer number of bodies (~10), that might be a huge win. Without being able to see the design and toy around, I can only guess. I would check out the previously recommended Stitch command. There is also a Validate command located under the Inspect menu in the Patch work space. This can be used to heal and generate solids.
In a previous case. I found I could do the following procedure to generate a nice solid from 1000's of surface bodies when the upload/import process failed me
1. Perform a Save As of the problem component to save it to its own design (right click on the component in the browser and select Save As.
2. Export this design as a SAT file
3. Use the File > New Design from File command to import the SAT file.
You could then insert this back into your main design assuming that it work, or possibly share just that SAT file so we could help you repair the geometry (assuming there is an issue with it not stitching to a solid).
The elephant in the room for me is, do you need every body in that 3900 bodies? How many of these bodies are little circuit board components that have no bearing on what you are designing? It may help to simplify the model and remove bodies/ and components that have no impact on the design. The reality is that there are performance limitations that impact the amount of geometry you can have in any given design. It's hard to say anything about a design that I'm not able to look at, but it my help to just simplify this down to a smaller number of bodies.
You could leave the tallest or critical components in-place and remove the rest.
I hope that helps.
Thanks,
Nathan Chandler
Principal Specialist
Hey Nathan,
thanks for the explanation! As my work progressed, yesterday I did just that what you've described in your screencast - converted one body into a component, acitvated it and drew a sketch. But I could not see any improvement.
Next thing I will try is to export into a SAT-file...
I was able to stich those unstiched bodies together - there are two connectors which were missing a patch to be fully closed. Now the 654 unstiched objects merged into two normal bodies. But i still see this:
You suggested to use the validate command under inspect in the patch workspace... unfortunately there is no such command.
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