How to create a circular mesh like a speaker with holes

[Anonymous]

Hello I am a nube to fusion360 but loving it:)

I want to create a circular speaker with lots of holes in it like perforated mesh. I did it one way with a cylinder and then sketched a small circle and then did a vertical pattern followed by a circular pattern. The problem was it became very unresponsive very quickly and therefore a nightmare to work with.

My question is what is the best way to achieve this. I am assuming that there must be a better ay as I am sure this is something that is always needed in product development.

I have attached a screenshot of something I am trying to achieve.

Thanks in advance 🙂

[HughesTooling]

I experimented with something similar a while ago, one tip is make a sketch with a line that matches the profile of the outside cone to use as a path for the pattern.

File's attaches step along the timeline to see how it works, any questions just ask.

Mark

[Anonymous]

Thanks mark,

How do I open that as the demo version I have only seems to save in the cloud and no local files that I can see??? Told you I was a newbie 🙂

[HughesTooling]

Use the option New Design From File on the file menu.

Mark

[Anonymous]

Thanks Mark

I got that working so thanks but I still get the spinning wheel of death when I try and process lots of holes. For instance I just made the holes down into 40 and now its been thinking about it for 5 minutes and still not finished. If you are doing a speaker mesh then you can be talking about a few thousand little holes, especially the little bluetooth cylindrical speakers. Obviously this method doesn't seem to be good for that many. Is there something I might be doing wrong? I am on a mac pro top spec machine so I cant imagine my machine is not fast enough??

Thanks.

[HughesTooling]

I tried a couple of other ways like sketching a vertical column then extrude and pattern but it takes just as long to compute so I guess making a thousand holes is just going to take a long time. Only work around would be use parameters for the counts for each pattern, set them to a low number while you're modeling the initial design, when you're finished and happy change the parameters to the numbers you really need and leave any filleting until the very end of the design process.

Mark

[HughesTooling]

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@Anonymous wrote:

Thanks Mark

I am on a mac pro top spec machine so I cant imagine my machine is not fast enough??

Thanks.

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Processor speed is the most important thing with something like this, number of processors will not help much as these sort of operations will not be multithreaded.

[PhilProcarioJr]

@Anonymous

This only took about 20 seconds to calculate on my 3 year old windows pc. 2400 holes....

[TMC.Engineering]

I looked at patterning a few ways too and it looks @PhilProcarioJr is the best for this problem.

normally I like to pattern features but it was a lot slower. 

Phil patterned bodies then did a combine.  It seems much more stable and faster.

The only thing I would note is Phil used 80 instances over 360 but the body was two sided.  would it be better to only go one sided, or maybe 2 sided and only pattern over 180 degs?

[HughesTooling]

One small difference with Phil's version is the holes are perpendicular with the origin planes not with the surface of the cone. My first try with the extrusion rotated 5° slowed the process drastically about 3 minutes to do a compute all and after a few edits Fusion really slowed. What I found sped it back up was to use a 2 sided extrusion and move the end away from the centre.

Doing this to Phil's original version speeds it up as well. Version with holes perpendicular with the cone surface attached.

Mark