Fusion 360 Tutorial - Timeline in 3 Levels of Difficulty | Season 3

how are you doing my name is lars christensen and i hope that you're ready for another fusion 360 video today we're going to talk about the timeline in fusion 360. we're going to talk about it on three different levels we'll talk about as a beginner as a professional and as an expert i'll let you pick what level you're on let's go [Music] alright so as a beginner i'm hoping that you have already noticed that there is a timeline down here by default insider fusion and the way that timeline normally works is that if i go up here and create a sketch on a plane you will see that we get that sketch icon there if i select a circle and finish up that sketch and i extrude that out then i will i will get the feature and hopefully most of you have kind of gotten through this this timeline down here is recording every single step that is that you're doing inside of fusion and you can always go back and you can right click one of these icons you can edit the feature or you can actually from right here also edit the profile sketch that'll be the same as right-clicking this gets here one thing to know is you can actually also just move that little cursor back and forth but this timeline doesn't actually have to be default and and some people choose not to i would say i always have it on and it is the default but be aware of that if you go up to your settings so we go click your name go to preferences and if you go ahead and go into the design space there is in here um an option to have the default what is parametric modeling but there is also a direct modeling and i'll show you just in a second what that means or you can have the software to prompt you so if you're jumping between different workspaces or between direct or parametric you can actually have the software asking you what you want to do the only time where the direct editing normally kind of appears to you is that if you go and you decide to open up a file of another format so here i'm going to open up a step file what is a neutral iso format and uh as i'm bringing this file in so this file was created in another piece of software could be in vendor could be solid could be something else but what you will see when i'm bringing it in that it actually does not turn on the timeline down here there is no timeline and that is what we call direct editing now the reason for that is that if you're bringing in some software or some part from another piece of software this plastic part here we need to create a plastic injection mold for example then we might need to do some edits to this part and we can use the direct editing tools inside of fusion and make some changes without have to record all those steps in the timeline mainly because the timeline down here can as many of you maybe have noticed can get a little long so just to show you in case you didn't know if i go in here in direct editing mode and uh i'm just like this the inner circle i'm going to select to fill it on top and there's also i filled it at the bottom if i hold down control and select those two and hit delete on my keyboard then you will see that fusion actually heal up that it um it kind of takes the hole and says all right i delete the hole let me then glue everything up the way i want it to be and this can happen when you're bringing in imported files that you want to make some corrections so we could go in here and select these fillets around here select that one that one that one that one that one oops and this is um fairly i would say complex geometry somebody probably spent some time modeling that up let's go ahead and take the other side of it that that all right so now we selected all those different fillets and again if we hit delete on the keyboard fusion will go ahead and delete all those fillets and it actually it's not so much about what you delete it's more about the surroundings can confusion figure out to heal it up but all these different changes that we just made we might don't want those to be recorded in a timeline that's why you you do that in indirect editing so just so you understand that's one of the the powers of direct editing now taking it a step further now where we have a mold and a cavity and you can see that the timeline now they have gotten some more features so this is actually done with surfacing you have the surface toolbar up here be aware of that having this timeline can actually be a very good learning tool issue if you're new to fusion so you can grab this little cursor and you can move it uh back and forth you can also use these buttons down here so if i go all the way back to the beginning we can actually click on next steps and if i just uh turn this on some of these things might be hidden you can see here that this was the part that you just saw before was brought in if i click on the next one here then and we hover over it excels that we scale the model up because in in um if you're doing a mold there's some shrinkage now i'm just going to grab uh the time bar here and i'm just going to drag it out a little bit uh you can see that there's some different um surface bodies being created and probably to plot some of these different holes in this body you will also see that some sketches were created we can probably go in and turn those on and you can see some different sketches was created in here that turned into some lofts and sweeps and we can go ahead here select all these and you can kind of see those different surface bodies here then there was some trimming to do so know that this timeline can be extremely well uh to kind of go back and look at uh what somebody did and try to figure out how the heck what was the steps they took um to um to do that and then we ended up with um with kind of the core and the cavity done uh here so as a beginner uh that timeline running down there um is um is super useful now do be aware of if you go back to our plastic part here that you can turn that timeline on if you want to all you have to do is going up and right click up here and you can say capture the sign history and then it's on and now anything we're creating for this partner will be recorded and just as we can turn around we can also turn it off so we can right click here and we say turn it off now be aware of you get a warning that if you do that these things will will get lost so if i said okay to that then they are now gone and if i turn it back on again it just comes on as a base feature that doesn't have the sketches i've literally lost those sketches right now i don't have to use some of the other direct editing tools to modify uh this part now as a professional i want to talk a little bit about what happens in this timeline when things start breaking because if you have modeled a few times in fusion there's a chance that you kind of start breaking things down in in this timeline and it's extremely important that you actually go back and fixing those now i want to show you it's actually pretty basic things that happens but just some of the ways you can find out so if i go ahead here on this end and i open up a sketch and i'm just going to go ahead here and draw a square and let's make it 50 by 50 millimeters like that and hit q for press pull and and we can make a um a cut through there so we have a sketch and we we have a feature now this sketch if you're going to edit that this sketch here it's coincident to that corner because that's what i where i started my sketch and to this face and you should be aware of that in the background of a solid modeling tool the software itself is just keeping track on points edges and faces and they're all assigned with like ids so if any of those breaks that's when you can can run into two problems so if i we we put in our square we extrude it all the way down the ads but if i draw this one back and i for example decided to open now another sketch here and this is going to happen this sketch i'm creating right now is happening before those two other ones and if i just cut this face away let's go ahead here a little just cutting all this away that means that i'm stealing that corner and that face id when i'm now moving forward you will see that this we still get the feature so fusion is is powerful enough that it sees there's an issue it's yellow and if i right click on and hit review warning it would tell me that this sketch plane is lost it's using its cache to actually be able to do this um and also there's a project source is lost cast is used again so it's doing two different things here um if we go in and we edit that sketch um you will see that everything looks somewhat normal but of course that sketch is sitting where that sketch is sitting out in space it's having a warning you should always go in and fixing these and again the idea is when when fusion is solving it's solving from the first base feature every time it's recalculating it's calculating every single steps so you can imagine when it comes to this point that now is using cash now it's trying to recalculate things that's extra resources no need to it in this case we could right click and we could say redefine the sketch plane and we could select that face there and hit ok and you will see that that fixed it it went away so all it needed was it just needed to uh to find that sketch pane that's extremely important that you go and fix those another thing you might see is if i go ahead here and there to fill it here let's add a i fill it something like this uh to this part this is all good well i could create another sketch on the opposite corner let's make that 50 by 50. and just as i redefined our our sketch to the right plane i could go ahead here and say i want to edit that feature that was the original cut and instead of selecting that sketch if i i could select that sketch right there instead right so let's go ahead here actually there we go it needs to be before that let's move that to there edit that we could select that square there that's going to make that extrude satisfied but it's not going to make that phillip satisfied because that fillet is looking at some place in here now this one here gives us a red because it literally there's no chance for it to display before when the sketch was broken it could still fusion could still solve it but in this case here it cannot it it's missing literally that that area um and again if you don't fix these then that's going to be broken and you know you will never remember where they were broken right so if we go ahead here and select this edge instead and give that some kind of affiliate then the feature is now satisfied and it's fixed so as a professional you definitely are not allowed to leave all kinds of yellow and red things down here you need to solve these as you're working through them all right so for our experts you always got to keep in mind that as you're adding more and more things into the timeline the the more the computer simply have to calculate and that gives you a couple of different options if you watch the video i did under the rest toolbox i kind of talked about how i had modeled up the toolbox here part of the toolbox and then i started to lay things out with some different commands uh the the move command the line tool and then i i added some some different joints and just remember that you can actually clean some of these things up these two commands here uh the move their line and the move are actually kind of overwritten later on by these joints so there is actually no sense of of keeping these in here they are they're really just um you know they were moves i used to to lay this thing out to get it kind of close to where i wanted it and then i tied it down with these uh four joints so you can go ahead and you can select uh these items these three moves and you can actually in our case here we could actually delete them and get them out of the timeline and that would um that would save it up now another thing i think is an expert moves when you're working with timelines is to utilize something like grouping things together that can that can help so in this case here there's a grouping here that was used for the layout for the mill and if i just select those here and i just suppress them for a second and there was also um some joints used here later on for for the assembly so this one kind of have two different type of configurations and you could group these together so if we select these and we right click we can create a group and that group we can rename so it gets a name so this could be you know as assembled we could call that group that uh and then we could go ahead let me just go ahead here and suppress that let's go ahead and take this other group here we can right click we can unsuppress it and then we could create this into a group and we could right click and we could rename that group to be manufactured now um manufactured now we have two different group we've grouped things together here one is assembled and one is as manufactured and we could just right click we can suppress uh that feature and we can right click we can unsuppress that feature and activate that so that's just a way to kind of um pack every thing together now the last tip i'm going to show you here as an expert and this is a simple model but i think it shows it very well is when you start working with bigger assemblies how can you possibly assure that you put as little down in the timeline as possible and one of the ways you can do that is actually by placing your components and model your components where they're going to be in in the final assembly so you can look over here and you can see that this stool and you can watch the video where i did it is a bunch of link components which means that it's a bunch of different components being put together now if you're looking at this footrest right here uh what you see in the final assembly here uh that footrest was i think one of the first components that was brought in here here you can see that it was brought in and then it was there was use a join to place that so again if i move back you can see it's sitting there if you move it down then you can see that it's placed in place now in this uh final assembly we're in right now if i turn the origin on you can see that that origin of this part is here and this this does take an expert to start thinking about this but where you're placing that audience could be absolutely critical and i'm not saying that this is a very good place for this stool but what we could is if we open up the foot rest itself and i turn that audio on you will see that well like most people do i model this one up right on on the origin there well if we go back into our assembly and let's just go ahead here and and delete it out of here um if i insert this footrest into this current design where does it come in well it comes in here right now we do get a free move in here but at some point uh here we will have to to use a joint um to lock it in that maybe have to use two or three different uh connections what we could do instead uh let's just leave it out of here was in if we had thought ahead we would model this part where it gonna be placed in the final assemblies and this is the way that uh people have worked with cat systems um you know going back to to the late 90s i think where if you put if you're putting a big assembly together then you actually start thinking about these things ahead of time so when you started to to to draw this one up i'm just going to sit here and use the the move icon um if you started well let's let me just let's do something else here let's save ass just so i don't mess everything up here all right um so when you start modeling something like this up you would actually have in your sketches you would have thought this through and and you would have modeled up um this part here i don't know something like like this um so you had kept that origin in cons in relationships where it should be so when if we go in now and we insert this new last version two in here and is that updating it actually comes in where we want it and now instead of have to activate a joint it all it takes as you probably have figured out is to um to take this part and just ground it right here and that will be a lot lighter than trying to use joints with different commands so i hope that this is useful i hope that you found this video helpful if you did give it a thumbs up if it was a completely waste of your time if it was stupid it was dumb give it that thumbs down leave me a comment and don't forget that down in the description there's a new way that you and i can connect via email until next time i hope you have an awesome awesome day take care folks

Channel: Lars Christensen

Views: 15,513

Keywords: Autodesk, Autodesk Fusion 360, Fusion 360, Design, Manufacturing, Tip, Beginner, Lars Christensen, #LarsLive, Best Practice, Modeling, cam, cad, tutorial, How to, 3d printing, free software, software, Product design, Mechanical engineering, fusion 360 tutorial, fusion, autocad, design, inventor

Id: vSZPcqUB3lA

Length: 22min 12sec (1332 seconds)

Published: Wed Dec 09 2020