Modeling with Fusion 360 (Model Mania Example)

hey one good way to improve your modeling and improve your design practice grow with fusion 360 is to go follow along with other tutorials like on this channel so i've been going back through the model mania it's a solidworks event it's this competition it takes three minutes whatever they give you a model and then some design changes at the end and so you effectively have to make one model and then kind of modify it and all do it within time and you know you win prizes if you're the fastest speed not really important but it's cool to go through some of these models where someone's gone through and efficiently modeled it with design change in mind so it's been really helpful for me to go back through because some of them are actually kind of tricky all right so here's the finished model at least for phase one and a few of the challenges that i when i'm first looking at this is this kind of rounded and angled slope this face that actually looks kind of confusing to me this shape when i look up from the top view that's not too challenging that looks like a pattern right looks like one of these so this isn't too bad and then i think you would pattern it and then this hole that's also a pattern that one actually does look tricky because it's a counter bore that's sitting low strategies number one definitely use pattern number two we're gonna do a rounded surface that we're gonna extrude up to that's huge sometimes i forget you can just create a rounded surface kind of like this one so i can use this rounded surface and then extrude up to that to create a more complex shape very cool i like that and then modifying whole wizard or tricking it to be able to drop a counter counterbore hole down low that'll be interesting and then going into the second part of the design let's look at how to model this in fusion 360. starting on the top plane i sketch a couple circles look for some circles sketch those out i'm in millimeter i want to make sure that my document settings look good hit d for smart dimension and 22 22 millimeter and 16. so nothing nothing crazy and then a circle off to the left and hit d for dimension 12 and dimension from point to point and that is 35 and now it starts to get interesting now remember that that dimension doesn't anchor this down it just shows the distance i'm going to select the two points and do horizontal now that's locked in space and i'm going to sketch kind of from this quadrant up and i don't know where it goes do another line now these are going to be equal i know that so i can make them equal and i know the angle select both lines and 22. okay that's not quite there yet right because you can see it's pretty crazy so undo that those movements 22 now we want to extend that with a line hey if you like these tutorials hit that like button and leave a comment youtube really likes that and it'll help me grow the channel thanks so i can do a line coming up from the center going vertical and i'll do another line going down and we can extend this until it hits and i do want tangency so that's the other thing so i'll do line to arc tangent same thing there we go that's better it's gonna be better behavior cool now we could do just an extent do s for search extend and we don't have to do this to clean it up but sometimes mentally it's nice just for um you know a nice clean sketch is easier to read easier to look at easier to modify sometimes okay so how about you know how do we get this symmetric a couple ways you can do that um we can do a center line and just align it so i'll hit x for construction and i think it's the construction line first and then these two lines and select all three in that order and then do symmetry and are we not quite yet equal and these two lines should be equal there we go cool all right so this sketch looks pretty good and then we'll start to extrude it just extrude that going up at extrude that cylinder at 22 perfect and now this is where it gets interesting you're going to sketch a line off in space and this sketch line is going to be a revolve or a surface okay so let's there we go this line out in space and a few things we know about the line is it's at 112 degrees to this angle and it's six millimeters off from that edge and it needs to be extended to reach the other sketch that's what i have i've aligned it so whenever you need to reference another sketch hit p for project and select the edge or you know this edge and then you can reuse that for as a reference so if i'm going to do a line so i can do p do it again there you go it projects it awesome and then we'll sketch a line coming up we'll do construction and it's connected at that point so if we were to test it this if this circle ever gets longer then this line should extend out a little bit or adjust anyways okay so we have this line that looks good and we're going to do a surface revolve great and it will select the surface and we'll do this angled line excuse me this axis in the center and we can see this nice new surface body and we're using this as a guide pretty cool something to keep in mind you don't have to achieve something in one feature sometimes just extrude it up okay so now for the tricky part of extruding up to hit this now there is a gacha with fusion 360. you cannot just extrude what you want to hit by default it won't just work it wasn't for me so go up to object select the surface and it will fail and i tested a bunch of different things so it seems to solve much better when you use adjacent faces this seems to be the gotcha for me i test on a couple different parts um so this selected face i thought should work but it needs this adjacent faces okay now turn off that body great all right now for the whole wizard so this one's interesting because in the solidworks model mania they effectively just drop it in and then manipulate the sketch in which it derives which we can't do that we just have a feature that we're editing so what i did was i selected this top face as the reference and then drag this over until it referenced that center hole or an axis you could create some sort of reference that you connect to but that that was good but i then and i used the counter bore and clearance so i used the sizing so i went down and found m4 great and then click off of that so i click now to simple and it keeps that shape for me and then i can manipulate this until i come up to a distance so i know that when i came in and measured so when i measured this face or sorry in the saw work sketch i know that that's supposed to be four millimeters and so when i come in and find this extends here that this 39 gives me the four millimeters so i just adjusted that to hit so so not quite as easy as solidworks but it is possible it's doable next is the circular pattern so that one's pretty easy turn on the circular pattern circular pattern for features and what we want to do is pattern this whole feature and the whole feature so i'm doing both right the whole and the solid so i've got both and then this axis doing three of those so it's doing all of it at once and then we come in and start adding fillets easy fillet of 22 millimeters in these three corners then select the outer edge go all the way around at one millimeter do that again cool thing is the tangency does a nice job of finding everything just by selecting once so that's when it's pretty easy and then the final fill it up here of one millimeter at that edge great so this is phase one okay let's get into phase two okay so this is our end goal a few things that get modified we modify the angle distance so we go back and we change this to eight degrees instead of 22 so double click change your sketch from 22 down to 8 and then hit rebuild okay now the things that we have to come in and do we're here okay so now how do we create that kind of cut out part now there's several ways you can do it because it's uniform shell does work so i can do shell and i can do faces so i'll do these three faces and i believe it's three millimeter we shell that out great now here's where it gets interesting there's a face fillet in solidworks and it allows you to do a nice fillet between these two faces and not have to calculate everything but in fusion 360 we don't have that luxury we can't use that feature there is a rule fill it but it's not designed to be used for faces just yet from reading the forums okay so how do we as how do we create a 30 millimeter fillet that achieves the same thing if i don't have that special fill it that they have in solidworks so i created just a simple circle on the bottom i'm going to extrude that up now i extrude it up great but how do i get it to align nicely with that surface now luckily we have that same surface body it's that surface body that's perfect so um we'll do an extrusion up to the object again same challenge where you have to come in and do to the object but you do have to there we go two object and make sure you choose adjacent faces now we could come in and do all three areas at once because we have three fillets to fill in and hide that surface body once we're done join it together and so you can see it creates that similar effect to the fillet that they were doing and then adding the fillets as a finish the big one that i'd want to show you for sure is this i believe it's a one millimeter inside so if we do fill it face face we want to do all of the interior faces that it's gonna touch and we don't have to go around and do all three we can do those three and we'll do one millimeter great now how do you pat you can actually pattern that around so a circular pattern s for search i'm gonna do features i'm gonna do just the fill it and select the axis of this circle it brings it all the way around great optimize works but adjust does not solve in this case it fails so don't forget to look at your options here your compute options cool so then we can add these remaining fillets and we're done hey thanks for watching if you're looking for more of these model mania style tutorials be sure to check those out i'll put those in the link you

Channel: Tyler Beck of Tech & Espresso

Views: 2,568

Keywords: fusion 360, fusion 360 tutorial, tyler beck, fusion 360 tutorial beginner, autodesk, design, mechanical design, product design, cad, cad software, cloud based cad, cad in the cloud, free cad, autodesk cad, free cad program, autodesk fusion 360, fusion 360 tutorials, how to model in fusion 360, fusion 360 for beginners, model in fusion 360, fusion 360 from solidworks

Id: WfJv-rS9hu0

Length: 13min 16sec (796 seconds)

Published: Fri Oct 29 2021

Reddit Comments

[u/Galaxy3170]

I’ve been looking for more vids like this thanks.