The Ultimate Fusion 360 Sketch Video (44 Strategies & Tips)

44 sketch tips you got to learn in fusion 360 coming up okay so the first thing we're talking about right now is keeping our sketches simple you'll notice that this model although i could have actually done almost all of it in one sketch i'm going to fully define and sketch each shape extrude it give it a feature then do the next sketch now it's a circle i'll extrude that then next sketch extrude it why do we do it this way well i now have a sketch that can be edited for each one my performance increases because my sketches aren't too heavy so let's look at this a little bit closer here's the d-pad example and this is a good one i saw this in one of the au classes on sketching where if you take this model and you break it up by sketch feature sketch feature the performance is much better and the sketches are so much easier to manipulate maintain make changes to now so if we do the opposite and and we're going to do multiple offsets we could pattern that anytime there's a pattern that's a good giveaway you don't want to be doing sketch patterns for this much complexity so now so now we can extrude each profile that's a full extrude then we turn on the visibility of the sketch find the next one you can see it's it's a this one is going to be trickier to work with i can select through and find the right profile might want to hide the body find the next one hit extrude do the next join rule of thumb keep those sketches as simple as possible next one sketch on these three planes as much as possible the front top and right plane as well as use that origin strategically if you can keep the origin at the center of your design it's going to make your life a lot simpler and if i'm extruding this if i can keep it symmetric about the origin that even adds more value so in this case if i do symmetric extrude then that's going to keep my three planes right in the center so when we look at this in an example my planes if they were all in the center that makes my life so much easier so let's let's look at it when i first do this first extrude and do that right off the origin so i extrude this my next one when i want to do the cylinder coming from the middle where are my planes why look they're right there right in the center so i can easily select those planes and start sketching i don't have to do a brand new plane so i can do that next sketch and extrude going up extrude coming from the side extrude coming from the middle right so again rule of thumb keep that origin in the center as much as possible let's pause for just a second if you'd like to download all these tips in one friendly cheat sheet or grab a transcript of this video check out in the description down below the other thing when it comes to the origin it is critical as far as defining your sketch i'm going to talk about why defining the sketch is so important but even though i fully define this sketch with a bunch of dimensions you'll notice that it's going to stay blue even though i dropped on a bunch of different dimensions and why is that it'll move around because it doesn't know how it relates to the origin so i either have to dimension to the origin i got to do distance to the origin both vertically and horizontally then my sketch will be fully defined it's all black that's good or if i simply connect to the origin now it's fully defined things have to know how they relate to the origin to be fully defined the next thing constraints or dimensions so i had this friend and he would send me a cad model from time to time and it was always the same question you'd say tyler i'm going to add this dimension and when i do even though this sketch looks great when i try to scale it up or down it goes crazy right it does this okay that looks okay but if he makes this 150 how come it just went wonky like that right and i'd always ask the same thing without even looking at it did you fully define your sketch did you use constraints in this case it'd be really smart to do your constraints and think about how you would describe it to someone without a dimension you'd say well it's a rectangular plate i'd say okay so that means these two lines are parallel and are they equal yep these two are equal these should be that should be a horizontal line that should be a vertical line and what about the way the arc goes into the line well i want tangency i want that nice smooth transition from line to arc so i'll do tangency so that's going to keep that corner intact with the round the other thing we definitely need to do is connect it to the origin some point on this sketch should be connected to the origin or in this case we could do a sketch across the middle and make that construction line we can select the line in the origin to midpoint there we go so at least we know it's connected to the origin in the center okay so now i'll add a dimension of 60 and this one of 30 what are we missing what drags okay so it looks like i failed to put that at horizontal what about the arcs they should all be equal or we should put in a dimension for each arc okay so they so they're all equal and they're three great i already have that now what happens this is moving up and down so i haven't related it to the origin as far as maybe the height of the origin we could do a construction line or a distance now it's fully defined so great idea use constraints first and then dimensions the next one troubleshooting a sketch i always drag the blue points to figure out what's missing for constraints but when you go to hit extrude and it will not extrude it doesn't give you a profile and you can't seem to get it to work i learned this line method i love this this was from an au class as well and basically you just sketch a line through it and then when the profile wakes up that tells me this side of it's fine so you can start adding lines as you go okay so it's above let's go there okay so it's somewhere in that range and you don't have to keep these lines intact you can even drag them and you can start to kind of pinpoint where the problem is so it looks like it's somewhere in here if i zoom in on that that point was not connected and now it's coming through just fine so you can use that as a way to pinpoint what is missing in the sketch when dimensioning if you add a dimension to the sketch it's black and fully defined meaning it's going to behave with the design intent that i have in mind but when i place on one more dimension it gives you this message it's saying it's over constrained what does that even mean it means you're adding one too many variables to the mix right so if you hit okay it's now a reference dimension and it's a measurement try double clicking it doesn't do anything okay how do you toggle something i'm sorry and i know that that is duplicate i didn't actually mean to do duplicates let's add a new dimension this one over constrained it's a reference what if you'd rather have this one maybe than the radius or maybe then even this height right so what you can do is right click on one of your dimensions an option you can delete a dimension and then you can right click okay so i delete that dimension and now this drags up and down and this is reference up this reference updates but let's right click on it if you right click on the dimension and do it just right sometimes it's not there you can toggle this to driving now it's an intelligent smart dimension it's parametric and it drives it another really good rule of thumb is to name your sketches so if this is the main so if this is the base profile and this is the and this one is the vertical cylinder that's going to make it a lot easier to work with in the future if you saw my other video and i'll link to it of how you can build this whole model from one sketch what i did was i sketched a bunch of different profiles or sub-regions in one sketch and this is acceptable because this is a pretty simple model it's not that overwhelming there's not that many dimensions there's not that many constraints and so when we start extruding i'm effectively extruding let's do it together so i'm i'm going to extrude the base profile first right and then i'm going to extrude this upper profile a little bit and then i can reuse here's a little trick if you want to select something that's hidden by geometry you can hide the body or you can do a select other hold and click with the left click near it and it'll let you pick the face or the profile or the other face so that is what's called maybe a select other in other cad systems and in fusion it lets you select through things i love that one so now if i extrude and this is a new join and also we want to get this profile too there we go so we're using the same sketch over and over again and keep that other rule of thumb that it's better to do a sketch and then a profile and keep them simple it makes they can edit easier and perform better so the next one you don't really have to trim infusion if i add this circle and i want to trim that off whoops hit d for a dimension i trim that i can but what if you want to keep that as a reference you don't have to get rid of it you can just extrude that profile and use that sub-region and leave that there so it doesn't hurt anything but if it's bugging you there's a couple options you can hit search as key for search trim trim it out right you can do that but if you'd like to keep that reference there here's another option do the search and do a break if you break this it's now going to be two entities so it's been broken there and there and now when i select it and hit x on the keyboard for construction now it's just reference geometry over here but then geometry where i need it pretty cool how do you drive everything in a sketch with the same dimension so if i find this dimension hover over it it's d1 okay so if i go find my parameters do a search for parameters i can find all of my sketch dimensions right here in this first sketch and then the other features and their dimensions i could drive everything off of this let's rename it and call this our master dimension or offset dimension or whatever it is you want and now i can do everything is related to the master to mim so master dim times 1.3 we'll do this one this is the master dim divide by two master dem kind of get where i'm going there so times 1.35 great so i could go down the list and drive all of these with one dimension so it's 70 and those others are going to update the little f x shows that it's a function that's being driven by the equation hey one of my all-time favorites when i select a face or a plane and hit sketch i hit the s key it wakes up my modular toolbar this is intelligent based on that i'm in a sketch that gives me sketch stuff and it's got an awesome search i love this thing i use it all the time if i'm looking for a fill it if i'm looking for a revolve if i'm looking for a pattern i start typing and it finds it i love that also we could if we wanted the one of the other rectangles like the center rectangle i can add that to the shortcut bar hit this little arrow it's going to add it right there now that is available for the next time hit s find that rectangular centered rectangle drag that in now okay a note about rectangles i'd say use those as often as possible why when you add those constraints the vertical and horizontals automatically as well as if i type in the number and hit tab it goes to the next one so it's letting me add dimensions as i go and relationships so that's a little bit more intelligent faster way than sketching it line by line okay what about the grid come down find your grid snap to grid settings and grid settings adaptive based relative to what you're working in or fixed lets you then set up your own grid that you want but it does have to be turned on in the sketch grid palette so i turn this on and now i have these snapping points that i can sketch to and so it's snapping to this large grid that we can use what about these other options in the palette construction line select an item it goes to reference the shortcut is x on the keyboard i love the look at option this one just looks directly or normal to your sketch so if your views are kind of out of sorts to where your front view is off it a little bit it's helpful just to go straight you can now look normal to it with the look at snapping is kind of obvious that it wants to snap too okay the next thing if you were to start a plane somewhere in the middle of this part so i'm gonna do an offset plane from this face somewhere in the middle of the part how about right there and you want to sketch in this geometry maybe we're going to work on a cut or a special slot or keyway whatever it is if i select the plane hit sketch if this geometry is in your way you can use the slice tool and it'll slice wherever you're at allowing you to sketch and work with this which also gives us next to some of our other things the profile and the projected geometries i now can snap to this projected geometry i'm using edges that aren't really there but they are the extension or the end of that virtual part pretty cool the other thing sometimes in a sketch it's helpful to turn off the dimensions temporarily it's also can be helpful turn off those constraints if they're getting in your way but keep in mind if there's so much on the screen that might mean that your sketch is getting a little too complicated just keep that in mind okay when you're sketching and you start a new part how do you change the units right here in document settings you can change it to any other units as well as this is where you can set your default or you can do it up in the preferences some of my favorite sketching preferences are under design go into design i definitely like to have the auto project project edges look right at the sketch by default i want it to go normal too when i drop a dimension i want it to automatically edit or open up i love that one and then this scale entire sketch at first dimension i love this one one of my absolute favorites and if you've seen my other video on that for scaling the entire sketch let's look at that real quick so if you go to the treble to get this fully nice dimension sketch you you know go to this treble to sketch it just right but and if you're off by an order of magnitude you can select the item if i make this a thousand instead of it going crazy and going just nuts it's going to look like the same sketch and that's because of that scale off of the first dimension i love this one when you're sketching lines you click you click and this is called chaining when you'd like to stop hit escape on the keyboard that'll stop it another way that you can snop when you're sketching is you can double-click really quickly and it it creates it but then stops or as you're sketching you can hit this little plus sign and it'll stop sketching i like the escape key it's probably my favorite let's talk about the box select if this is overlapping and we've got some lines that kind of correspond to the same spot when i drag to the right it's going to grab anything that touches the box or is in the box so it grabs everything that i was near right now if i select to the left a box to the left that is going to be more liberal if it's trending to the left more liberal it's going to let anything that even touches the box sorry i think so if i tr if i select to the right nothing is going to get selected in this case because that's not fully in the box go to the left it grabs that line sometimes you need to dimension from midpoint to midpoint a shortcut to do this hold shift on the keyboard get near the midpoint it'll wake it up get near the midpoint i'm holding shift and now i have a dimension to midpoints and i could do the true distance or maybe the horizontal distance or the vertical distance okay let's talk about the quick measure i love this one anytime you want to measure a line just simply select it down at the bottom it gives you that distance if you hold ctrl and select two lines at an angle it gives you an angle so it is intelligent kind of based on what you select if i select these two points i think it's just the distance between them all right if you have slots if i do a an s search for slot and i drop in my slot we'll make it horizontal okay if i want a dimension from arc to arc when i hit d for smart dimension place it guess what happens it goes center to center of those arcs not what i wanted so i'm going to right click do arc tangent before i place it now i'm going to right click it's arctangent still and click on it and now it goes arc to arc there we go okay here's the pro tip that i just figured out i'm so excited about it sometimes you need to be able to reuse geometry right so maybe you say like i need to get rid of this block right here what's very easy to do with the extrude command i can hit extrude and it's just going to reuse that profile and cut that out that's great that's not really a big new secret but when you want to sketch something again without having to there is the project tool now when you're sketching and you hit project it redraws that but but the thing is those really aren't sketch lines that i can reuse and maybe there is a way to do that i don't know how to do it so here's my workaround if if i want to resketch this face i'm going to start a sketch and i'm going to do offset and i'll select the edge the outer edge and i'm going to do an offset of 0. this was pretty exciting to me so it re-sketches that and now if i find that constraint for offset right there that little tiny icon and hit delete now these can be maneuvered and redefined i could add dimensions to this let's hide the body so you can see it so now i have this brand new sketch based off of something that was already drawn but i can add new constraints and design intent to it pretty cool the last few bonus tips of course the line to arc command hopefully you already know that one clicking as i'm clicking if i drag at the end point it's going to add a tangent arc okay when you're sketching um and this can be especially helpful like when you've got a bunch of parts or components like this one when i'm sketching on this top face it naturally wants to infer to everything underneath it's got all these snap points that it wants to go to so if you don't want to add a constraint you can hold control on the keyboard and it's not going to snap to anything this allows you to kind of sketch freely without any concerns that it's going to snap into place or add a constraint

Channel: Tyler Beck of Tech & Espresso

Views: 21,493

Keywords: fusion 360, fusion 360 tutorial, tyler beck, fusion 360 tutorial beginner, autodesk cad, autodesk fusion 360, fusion 360 tutorials, fusion 360 sketch, fusion 360 sketch tutorial, fusion 360 tips, fusion 360 line to arc, fusion 360 planes, fusion 360 beginner tutorial 2020, fusion 360 beginner course, fusion 360 sketch constraints, fusion 360 sketch scale, fusion 360 sketch planes, fusion 360 sketch dimension, fusion 360 sketch to solid, fusion 360 sketch tutorial 2020

Id: oVEaSKndyrU

Length: 23min 40sec (1420 seconds)

Published: Wed Aug 26 2020

Reddit Comments

[u/adamdavenport]

This changed my life, and you went at the exact right speed. Thank you.