Webinar Advanced Sketching

all right well I think it's about time we get started I've seen the attendees kind of level off so again thank you for joining in this webinar will be covering some advanced sketching topics in fusion 360 I am the only one I'm running the webinar and answering all the questions so if you have any questions you can leave them in the questions section in the GoToWebinar panel on the right hand side I'm going to do my best to get to them throughout the webinar but if it's something broader general if you could save it towards the end that would be great that we can get through all the content in time so let me switch over to our PowerPoint so I wanted to quickly review what we're going to be going over today so sketching is a pretty broad topic in fusion 360 nits really at the heart of everything that you do every extrusion revolve Loft everything really relies on sketches and it's important to really have both the fundamentals down as well as some advanced topics so today we're going to be covering sketching fundamentals best practices common workflows constraints and dimensions so what's the difference between a constraint or dimension how do they work what's the best process to use them sketch references so how do I reference geometry that might be outside of my current sketch and then we're going to be taking a look for the bulk of this webinar had some advanced tools so you've probably seen the basic tools like two-point rectangle and circle and all these constraints that are fairly straightforward but I wanted to cover some more advanced workflows that might be a little bit tricky to figure out how to how to go through them and then lastly I have some pro tips I guess productivity tips some quick tips that help you speed up your workflows and those are going to be at the very end so we can start things off just quickly making some definitions because I'm going to be referring to these terms throughout the webinar so it's good to have make sure that we're all on the same page so what's inside of a sketch so in fusion 360 there's mainly three things going on in a sketch you have your geometry and those are the shapes that you're drawing inside of your sketch these are made up of sketch curves sketch points and when you connect these curves they create profiles so those are the three terms to keep in mind as we go through this in addition to geometry we have constraints and you can think about constraints as simply rules that are applied that really relate the G a tree to each other inside of a sketch so constraints examples might be parallel coincident concentric fringe rules that define how certain sketch geometry can move and how it cannot move and then lastly we have dimensions which really just set the sizing of sketch elements this might be how large is your circle how far apart are two circles how long is your line what is the angle those sorts of things and I actually put them in this order because this is typically the order that we're going to be problem-solving in the sketch workspace inside a Fusion you're typically going to be drawing your sketch geometry then using constraints to eliminate degrees of freedom and really make sure that the sketch geometry will adapt in the way that you expect and then finally use dimensions to lock in those values that you have move for sizes or distances or something like that and it's important that you properly constrain everything ahead of time so that when you add a dimension it behaves the way that you expect so that being said I want to cover a simple example of this part that I have here on the right hand side it looks like a simple part it is what it's going to cover is creating geometry constraints dimensions the whole concept of degrees of freedom and then some other tools in the sketch palette such as mirror trim project some fairly straightforward things I know this isn't the most advanced example what I wanted to make sure that we could cover this at the beginning then we have a nice fundamental before we get into the more complex geometry so let me switch over to fusion 360 so I have a blank design here and everything that we're going to be doing today is essentially here in the sketch drop down menu so you see we have our sketch geometry that we can draw at the top here simple things lines different types of rectangles circles arcs the things that you would expect are up here we also have these other tools down on the bottom that interact with sketch geometry so instead of creating them these are tools I can interact them and edit them so for example we can add fill its trim break offset really interacting with existing sketch geometry and then down here we have the project slash include section of the sketch menu which really some of the advanced capabilities so taking a look at intersection where do we use that when is that common what does this include 3d geometry button how does that work projecting to a surface it's a nice way to create some 3d curves and we're going to show that at the end of this webinar so that being said let's go ahead and sketch out our sample part that we have so like every sketch I'm going to start by creating a sketch and fusions going to ask me to select a plane or a plane or face because I need a flat surface to draw on it doesn't really matter for this example which plane I pick I'm going to go ahead and pick this one right here and we'll see that we're reoriented automatically to look straight down and plan view at this work plane one thing the also notice is I do have the sketch grid on and this is something that's a personal preference I might leave it on for this one typically I have it off I just like a little bit of a cleaner workspace but it can be nice because you can snap to these grid markers in the origin and so forth so let's get started by drawing a few circles that represent the main shape of the part that we want to make if we look at it right here we can see that's made up of a few circles maybe some tangent lines let's start drawing those one thing that I would highly recommend that you have is under your preferences under preview if you check the box for this color sketch geometry based on constraint status I highly recommend it I have it on for this webinar and what it does is it's a very easy way to visualize if sketch geometry is fully constrained or if it still has degrees of freedom so I'd recommend you have that on what I have also here so I have my blank sketch let's start by drawing some circles so into the sketch drop down menu I can go to circle I'll choose Center diameter circle and one handy tip that I have is if you don't know what a command is wanting you to do just stop moving the mouse it'll tell you place a center point so the center point I'm going to position this on the origin it's just general best practice is if something can be centered on the origin why not so I'm going to click once to place it on the origin and as you can see I can move my mouse out to create a circle the dimension that I want if I have a dimension in mind I can type that in right now I don't so I'm just going to click you'll see that it creates the circle and it's drawn here in blue indicating that still has at least one degree of freedom and one way that you can test these degrees of freedom is by clicking and dragging on the geometry the center of the circle is fixed on the origin so that's not going to move but you'll if I click and drag on the outer perimeter of this circle I can move that around and that's why it's telling me that's not fully constrained because it's still able to change its diameter so next I'll draw another circle so from the sketch drop-down menu I'll choose center diameter circle and I'm going to place this somewhere over here at an arbitrary diameter what I'm actually going to do is turn off the sketch grid I just like having a clean workspace like this and we can jump into it so what we can do now is make sure that these points are horizontal from each other or we can start adding in some constraints because as you can see this circle can move anywhere that it likes and it can have any diameter I really want these to be horizontal so we can apply our first constraint between these so we have our constraints here on the right hand side so what I can do is select the constraint that I like to apply for example horizontal slash vertical and pick the two pieces of geometry that I'd like to constrain you'll see that the horizontal slash vertical constraint appears and now I can drag this around to any position but it's not going to let me move it up or down again I can drag on this to change its size and that looks good to me so next I'll draw some lines because I want to have tangent lines connecting these circles so I'll choose the line tool and often what I'll do is draw something rather arbitrary and then constrain it in the way that I want so I'll draw that line it adds my coincident constraints which means that the end point of this line lives on the perimeter of this circle you'll see I can drag it around and obeys that rule that I have set up let's make this tangent again to do that I can choose tangent select my line select my circle select my line select my circle and you'll see that I don't have to go back and choose the tangent command again it will go ahead and do that for me so I still have some degrees of freedom like wants to show a quick tip on how to draw another line this tangent without even having to go to the sketch palette again I can choose line and if I click and drag click and hold on the circle you'll see that it automatically adds this tangent constraint and if I hover over here I get another tangent constraint so there we go we have our two lines that are tangent to our circles now that I have you know relative a relatively constrained model here you'll see that it still has some degrees of freedom maybe we can start locking some of these down with dimensions so let's dimension how about the diameter of this circle and this one so to do that under the sketch drop down menu I'll choose sketch dimension I'll select this diameter let's type in 150 millimeters and for this one how about 80 you'll see that this circle turned black indicating that it's fully defined because we have its position in diameter locked in so it can't change unless we change this a diameter dimension over here now I can still move this around now what I can also do is now specify the how about the center distance between these again under sketch I'll choose sketched dimension select my two points and let's set this to be how about 200 that looks good so now I have a fully fully constrained sketch because you'll see that all the sketch lines are black and I have a few more circles that I need to draw so I have one circle here for a cutout so again I can choose center diameter circle or hit C for the hotkey for center diameter circle I'll Center it on this point right here and I'll draw it out we'll see that it's blue being that it still has at least one degree of freedom let's eliminate that degree of freedom by defining the distance between this outer circle in this inner one so again I can press D on the keyboard to start the sketch dimension tool I'll click on my two lines and I'll specify that this distance is 10 millimeters so our sketch is almost done I want to actually draw some lines over here so it'll start the line command I'll start it over here and as I move across I'll add a coincident constraint here to this inner circle and we'll see that we also have a horizontal constraint so this line is horizontal and its other end is coincident with the inner circle right here I'll draw another line down we'll have a perpendicular constraint and now I can draw it horizontal and coincident with that inner circle so it's still relatively undefined here so let's try to lock it in one thing that I might want to do is make sure that these two lines are symmetric about this center line of my part and I don't have that center line already so let's draw to do that I'll choose the line tool select on this center point and this one and we've drawn our line and we can use this as a center line but you'll see that it does interfere at the profiles because it is a normal sketch line to turn into a piece of construction geometry or a construction line I can select it I can choose normal slash construction here in the sketch palette or I can right click in two's normal slash construction we'll see that now it's dotted so I'm really just referencing it and it's not getting in the way of any sketch profiles so now if I want to make these symmetric I could choose my symmetric constraint and again if you stop moving the mouse that tells you select sketch objects or change constraint type so I'll choose my sketch objects so how about these two and now it's asking me to select a symmetry line and that's going to be this center line right here so you'll see that now if I drag this around everything stays symmetric that way that looks great and I'll go ahead and draw in one more line starting up here horizontal to this inner circle and instead of using symmetric there's another way I could do this I could mirror this line about that center line so to do that under the sketch drop-down menu I can choose mirror for the objects I'll choose this one and for my mirror line I'll choose this centerline essentially the same thing just a couple different ways you can go about it this is still relatively undefined I can actually dimension the distance between these two lines right here so I'll see that as I move them they adapt to stay mirrored about the center line what if I want the dimension between them to be something like 4 millimeters I can choose a sketch dimension tool and pick these two lines and set this to be 4 millimeters now we have this small gap and I can drag this corner in until it's somewhere that I like maybe this isn't a sketch dimension that I know or that I wanted to find I can leave it undefined right now and define it later or keep it like this where I can drag it around as I see fit so that looks really good to me the only thing that's left is to use a tool like trim to remove the excess profiles that we don't need this is not a necessary step but some people like having cleaner sketch profiles so to do this under the sketch drop them and you'll choose trim and we'll see that I can trim away this excess part of that circle as well as this and now I can come in here and remove these extra bits here so I'll remove this one and this one and that and then I can clean these up as well so we can choose trim and get rid of those so now we have a nice looking sketch here one thing that you might want to change is we do still have these diameter dimensions here which made a little bit more sense when these were circles so if we'd rather have those as radii you can select it and right click and choose toggle radius and now we have a radius dimension there so by default in Fusion when you create a circle it's going to use a diameter dimension and when you create an arc it's going to create a radius dimension and this is the way you can toggle between the two so that looks good so I'll hit stop sketch this is a sketching webinar so we're not going to do too much in the model workspace so I'm just going to simply extrude this profile up how about by 25 maybe a little bit more how about 40 there we go and we'll see that we have our part what if we wanted to have if we switch to the presentational so there is a hole running through the center here so if we wanted to add that how do we go about doing it simple ways I can create a new sketch on this work plane and I can choose the center diameter circle tool here and it looks like I could draw it I can eyeball it in the center but more often than not balling it's not good enough it should kind of give you an uneasy feeling and you should feel like yeah there's a better way to do this so how about before we draw the circle if we project in this face into our current sketch and to make a little bit clearer what project does is I'm going to turn on the sketch grid so you can see the grid that we're sketching on and to project this face in it's going to actually be a rectangle under the sketch drop down menu I can go to project slash include and choose project and I have two options I can project in an entire body which is just going to give me pretty much the cross-section or I can choose specified entities and for that I'll choose this face and now this face is projected in as you can see this curved face is projected into my current sketch really just has a rectangle so that looks good to me I'm going to draw a construction line from midpoint midpoint and I'll turn it into a construction line by selecting it and choosing normal slash construction and now I could draw a center diameter circle how about centered on that construction line and that triangle right there is the indicator telling me that it's a midpoint constraint on that line so I can draw my circle about 25 millimeters I'll stop my sketch and I can extrude this out I can cut through and I can cut through all of the material so there's our sample part that really shows what you can do with just simple constraints dimensions and the workflow for really drawing the geometry using constraints to set up the rules that you need and then using the sketch dimension tool to really define those distances and those dimensions of your sketch one thing that I like to show is that if we wanted to change this maybe we wanted to change this profile over here we don't actually have to jump back into the sketch in the timeline and choose edit one nice little trick is that if I turn on the visibility of sketch 1 and I have some sketch curves that still have at least one degree of freedom for example these corners I can drag them around to do some more dynamic changes so if this is something that maybe you don't know the dimension maybe it's in context of something else you can drag these around and change the geometry outside of the sketch without having to right-click and choose edit sketch you can do that outside of it and it's really nice for making quick changes so that was a simple example I know we have 40 minutes left and I have a lot that I want to get through so we can jump to some more advanced topics hopefully this is nothing new this is just kind of the fundamentals of sketching and fusion and we can now look at something a little bit more complex so we're making a little bit of a jump here what if we wanted to use a tool like intersect when is a tool like intersect useful and how does it work so this is a shape this is just an example where I made a complex curvy shape and wanted to see how do I grab the intersection of a plane in that curved shape and then use that intersection for a path for a sweep or something like that so I can switch to fusion and I have this intersect example here so you'll see that we have the complex shape it's tapered it is curved on the top and the bottom and all sides nothing that is really convenient so if I wanted to maybe find the intersection of a plane here and the curved body it's going to be a lot easier to do that than to sketch around a spline that matches the outer profile of this so what I have is a construction plane that I've created here and as you can see it intersects our part and what the intersect tool in the sketch drop down menu does is going to leave me with the intersection of this work plane and this body so let's see how it works to do that I'll first create a sketch on my work plane and we'll see here that our sketch grid shows where it with this intersection is going to happen and what I can do now is under the sketch drop down menu under project slash include I can choose intersect and again I have similar options I can choose specific entities that I'd like to find the intersection of or I can choose bodies to find the intersection of an entire solid body and really just find its cross section at the work plane that I'm working on so I'll choose that and I'll select this body and as you'll see this intersection is projected into my current sketch so they rehab it so what's an example of something you might want to do what if we want to run a circular cut along this path and perform a sweep all the way around using this intersection profile as the path and a circle as a profile so walk through the quick steps to do that we're actually done with this sketch all that we'd have to do is create a sketch somewhere on a plane perpendicular to this path and then sweep it across and I'm going to show how to create that and make sure that was perpendicular because it is a little bit tricky so to do that under the construct menu I'll choose plane along path I'll choose my path to be this intersection curve and as you can see I can drag this around and choose any position on this curve and it's going to create a work plane that is normal to that curve so it doesn't really matter at all where I place this I'm just going to choose somewhere that looks nice I'll hit OK and now I can create a sketch on this work plane and we can see that we're working now on this plane one thing that would be nice is to project in maybe the intersection of this curve with our current work plane so to do that under the sketch drop down menu I can choose project and maybe intersect and for the entities I can choose this path right here and it may not look like it did much but really I'm finding the intersection of this curve with my current work planes similar to what we did in the first step so if I hide this and hide our initial sketch basically that leaves me at this point it's actually really close to the origin that for the accidental subdue that I can choose a circle and I'll draw it here about eight millimeters and you'll see that I have this circle that is centered on this curve and now I can run this through for a sweep so I can stop my sketch show body 1 and under the create menu I can do sweep choose my profile and my path is going to be this curve right here and I've performed that sort of center cut out all the way around the intersection so you can see how we use the intersect tool twice there once to create a path that is an intersection of a work plane and a body using the bodies filter if you will on the intersection tool and then we're able to use the intersect tool again to find the intersection of that path as well as the work plane that I was working on to create that point so there's an example of using the intersect tool something that's a little bit trickier we can go back to the slides take a look what we have next and this is one that I find really useful it's for creating 3d curves without really having to sketch them in 3d what you're using is here is the project to surface command in fusion 360 to project a curve onto an existing face and it creates some really nice 3d curves that you can use for something like a pipe command or a loft or a sweep and I'll show you in a few steps how we can create a pattern like this on something like a maybe a handle grip or something like that so to do that let me switch to the part so we have here this bike handle grip that we want to add this pattern to one thing that I did ahead of time is I created a work plane up here I sketched on that and I just simply skip this spline nothing fancy you'll see that it is just a 2d sketch from the side it looks like a flat line so what I want to do now is project this spline down onto this existing surface so to do that under the sketch menu under project slash include I can choose project to surface it's going to need me to choose a plane or planar face and this is going to be the default direction that it's going to project from printer normal to the work plane that you choose so I'll choose this plane it's going to ask me to first select faces and for the face I'm just going to select this face right here for the curves I'll select this curve that we have sort of above the surface and you'll see that with the project types at the closest point it'll project a curve onto the face that you select really looking at this curve and projecting them the closest point that it possibly can that looks good but what might be better is if we sort of want to drape this along and to do that I can choose a long vector it shows the right direction already but I can also choose a project direction so I'll choose this vertical work axis and now we can see that if we look at it from the top it matches that profile exactly and it sort of drapes it down top to bottom along that surface so I'll hit OK and I'll hide how about sketch 14 at the top and I'll stop my sketch so we now have this nice 3d curve that we can work with on our existing surface you can imagine how hard it would be to draw this if we couldn't project it to a surface I can imagine trying to draw a curve that follow this unique profile and always maintain continuity on this existing surface so now I'll walk through the steps again this is more about sketching than anything else but I want to show the steps to create this cutout because it is a little bit unique and a little bit tricky so to do that I could use something the pipe tool one thing that you'll see is that if I choose pipe and i zoom in I don't really have the end conditions that I need because this curve is not flush with the surface the plane that's normal to this curve at the end does not match up with this plane so we have some kind of nasty end conditions here so pipe isn't this what we want so what I do want is actually the end conditions here if we were to imagine sweeping a circle along this path is I want that circle to be flush with this face at both ends and to follow this path so to do that I'll first create a sketch on this face I'll look at it from a 3d view and I'm going to go ahead and project in this endpoint of my 3d curve and now I can snap to that with something like a center diameter circle so I can draw my circle how about at one millimeter in diameter and I have that if I want this curve to be a construction line I can do that so it doesn't get in the way of any profiles I'll stop my sketch and then we're going to do the same thing at the other end so again I'll create a new sketch on this existing face using the project tool I can project in the endpoint of this 3d curve draw another circle at one millimeter and lastly I'll turn this into a construction line so we have three sketches here we have this curve which is really going to be the center line for this as well as two profiles that represent the end condition that I want so now I sweep isn't exactly what I want what I really want is loft so from the create drop-down menu I'll choose loft and I'll choose first this profile and for my second profile it's going to be this one over here and you'll see that fusion so sure I can loft between those is just going to be a straight line make sense but we can add in here some sort of rail or center line so I'll choose center line and the center line that I want this Loft to follow is this 3d curve that we just created I want the operation to be a cut and now we can see that it has sorry the end conditions that we need it's nice and flush on both sides and it follows this 3d curve so lastly to finish this up what I could do is maybe add a nice little fill it on these two edges just round it off a little bit and now if I want to pattern those two features around this cylindrical face under Rheda I can choose pattern and circular pattern for the objects I'll have my sort of filter set to features and choose the loft and the fill it features and for the axis I can choose any work access or I can choose any cylindrical face and it will find its central axis for me and for the quantity really up to you how about 18 I'll hit OK fusion is going to take a minute to calculate this it's a little kind of a lot that we're asking we're asking it to do a two-point loft with a centerline 18 times around the cylindrical face oh and add Phillips to every heads that you see there so that's how we can use the project to surface tool to create a nice 3d curve that we need that would be really hard to draw and then create some interesting features here around this cylindrical face I wanted to change the number of instances in this pattern I could simply right-click on this feature and choose edit feature so it looks good to me I'm going to take a second here to see if we have any questions I don't think we do so I'm going to keep moving on thank you for saving your questions for the end or I guess no one has any questions so that was the bike grip and the last example here that I want to show is a little bit more about 3d splines sketching in 3d is always tricky I think it's always going to be tricky as long as we're sketching three-dimensional things on a two-dimensional laptop screen if you will or two-dimensional surfaces so I can show you how 3d sketching works inside a fusion 360 so let me switch over to fusion I'll make a new design and a quick example let me see if there's a question here I guess everything's going well I'll go ahead and create a new sketch on this bottom face and if I choose a spline I'll go ahead and draw how about a four-point spline like that you'll see that this is perfectly flat on this plane to enable 3d sketching under your preferences and in design make sure that you have the allow 3d sketching of lines and splines checked so one way that we can create a 3d spline is by sketching it and then using the Move command to move one of these control points up or down so let me switch this to sketch choose my control point and I can move this up or down and you can see that I can create this 3d spline that way this is one way to create them in fusion I'm another way that we can do it is by using the include 3d geometry tool so let me exit out of this design make a new one and let's go ahead and start by sketching out a few two-point rectangles so do that I can hit the our hotkey so let's draw one here and how about another one right over here and you'll see that the size of these doesn't really matter it's more for an exercise so I'll stop my sketch and I have these two rectangles here I can extrude this one how about 75 millimeters up and I'll sketch the extrude sorry the other one something less about 40 so you'll see here that we have these two rectangles I can drag these points around and do some live editing to kind of inch them around if I like but what if we wanted to draw some 3d splines that maybe connected each of these individual corners and we're tangent to these edges at each of those corners so it's something that would be traditionally just hard to draw hard to imagine how you would draw it and this is really where include 3d geometry comes into play so to do this under the sketch menu we'll create a new sketch and really the sketch plane that you create this on is rather arbitrary because you are creating a 3d curve at the end of the day so I'll choose this plane again it doesn't really matter and what I can do now is before I draw any splines under the project slash include menu I'll choose include 3d geometry and you'll see that I can select these two edges and now these two edges are included in my sketch so if I hide the bodies you'll see that in 3d space I have these two edges and this is the biggest difference between include and project if I were to project these edges into my current sketch what that's going to do is project them and everything is going to be planar on this face I can even show you we can take a look at what that might look like if I were to choose project instead of include and I choose these two edges you'll see that it projects in to the sketch plane that I have right here and it's now kind of taking it down to two dimensions instead of three and that's not what I want so I'll undo that and make sure that I again to include 3d geometry which is correct and now what I can do is with the spline tool you'll see that it is on this work plane but if I hover over this 3d point it'll snap to it and I can move it again onto this plane or I can now snap to this point and hit the green check and now I have this two point spline that is a 3d curve the last thing I can do is make these tangent so I can choose tangent choose my curve choose my 3d geometry and again choose my curve and my 3d geometry so now I have this 3d spline that is tangent to these lines that I've included in my sketch and you can do this for all four things and create a really powerful kind of system here so let me switch over to this one so what you can see here that I have is let me go back a few steps so I did this for all four I have these curves here that are tangent to all of these and what's really nice is that these undefined or under defined rectangles that represent these extrusions I can still move them around so I can drag these curves around so let me hide how about these bodies and what I can do is move these edges around and you'll see that these 3d splines are adapting to everything that I do which is really handy what I can also do is I could perform maybe a loft so let's see what that looks like I already did this in the timeline but I can walk through the steps here so I can choose create and loft and let's loft between this profile and this one and it's trying to figure it out and I can give it actually how about four rails so I can pick this one this one this one and this one and it doesn't like something here so let me actually go back to where we have it done so there we have a loft between these two profiles using those four rails and as you can see I can adjust this around and that Loft is going to update really in real time as those sketches update what's really nice is I can even tack on an additional feature so you'll see here I add it on a Filat so I can hide these sketches so now I'm lost in between these with four rails for the loft and I've rounded all four corners and I can still in real time drag these around and create some really complex 3d curves that are really being used to drive the loft here I mean this is something that I think is really powerful it really shows off what you can do with 3d splines and the key here is really using those two-point splines because with the two points and the tangent constraint you're really guaranteed you're gonna have one smooth curve from one point to the other so let me see if there's there are some questions here I'll answer some quick ones yes this recording is going to be available we're recording it live right now this is going to be on YouTube and doesn't matter where that plane exists that was three minutes ago so I believe that was when we were creating these 3d splines no it does not matter where that plane is really the reason why it's asking you to choose a plane is any command that is going to create sketch geometry Fusion is going to want it to have a work plane that it lives on even if the curves are in 3d so that's why it's telling you to pick a plane if it didn't have a work plane to work on fusions not going to like it too much it needs a work plane for reference but unlike the project a surface command that doesn't have any effect over that 3d spline at all so let me I think that's all the questions that I see right now that are at least super relevant to what I just showed I'm going to save some time for the end so that is creating 3d splines in Fusion and we have 20 minutes and I have a few more things I want to show some quick pro tips either professional or productivity whatever you wish and I wanted to show you some quick things here so first what I want to show is how to break a projected link so let me go back to Fusion and I can actually go to this example and what you'll see is that currently in sketch 2 I've projected in this geometry so if this X were to change and I were to move this up that projection changes and because this circle is defined to be on the midpoint of this curve it stays in the middle this is I can think 90% of the time what you want you'd like it to update with these but what if you no longer want this to be linked so what you can do is in your sketch where you have that projection going on what you can do is you can select the curve so I'm going to choose all this projected geometry and you can right click and choose break link and now it's just some undefined or sorry under defined geometry so now if I were to go back and change this extrusion you'll see that that projection does not update probably not what you want but some people do ask you know maybe I've projected something in and I don't want it to update anymore I just wanted to grab a center point that that is how you can break the link of that projection so let's run through these so we did that how do we add a spline point this is one that I get a lot so if I go to a new document and I create a sketch what I can do is I'll draw a spline so let's say we have a three-point spline here and what if I really wanted to add an additional point in here all you have to do is select the line right-click and choose insert spline fit point and now you'll have this crosshair show up and you can place as many spline points as you want so I'll scape out of there now I've added two more control points and I can drag those around to any position that I like if you want you can delete them easily and that's how you can drag them around and adjust them so again you choose the spline right click and choose insert spline fit point you see if we do have some questions in here I'm going to try to get to these to the end I think a few more things to run through so you can easily the other thing is clicking and holding to draw an arc so to do that what I can do is let's stop this sketch if you find yourself drawing a lot of lines and you'd like to add in some arcs easily you can do that with the line tool so if I draw and I click I drew one line but if I actually click and hold and drag now I can create an arc so I could draw that I can click again and now I can hold and create another arc over here this is a nice little segue into the next tip that I have which is to use these constraints you don't always have to go over here to the sketch palette on the right hand side what you can do is choose the sketch geometry that you'd like to constrain and then right click and you'll be given a list of options here in the marking menu that you can use to constrain it so these two points that I've selected there's only three options I can make them coincident not really what I want here I can fix them or unfix or I can make them horizontal or vertical to one another so that's the one that I want so I can choose those and make those horizontal vertical I can choose these and again choose horizontal / vertical and this is a nice and quick way to do it because any lines that you choose you're only going to be given the constraints that make sense and you'll see that these match up with the ones that are not grayed out here on the right hand side in the sketch palette that's a quick little time-saving tip right there so that was everything that I had as far as these quick productivity tips and then what I have lastly are some resources for everyone before I get into all the QA so some with resources for learning fusion more we have our YouTube channel so if you go to youtube.com slash Autodesk fusion 360 you can watch all sorts of videos from longer tutorials that we do to quick tips to webinars like these that are recorded and uploaded to YouTube we have our fusion 360 website so autodesk.com slash fusion 360 where we have our Learning Center you'll see that over here the left image here where we have again tutorials content on how each of the tools work workflows basic training that sort of thing and we also have our forums on the Autodesk fusion 360 website so the forums great place to go if you have any questions and you want a quick answer I can almost guarantee that you'll get an answer in less than 24 hours we're really on top of the forums it's a great place to go with any questions if you want to do anything on social media maybe you want to tweet at us you can tweet the fusion 360 team at twitter.com/usembassymanila underscore Stein but that being said I want to thank everyone for joining and I appreciate your time have a great day

Channel: Autodesk Fusion 360

Views: 193,439

Keywords: fusion 360, autodesk, design, engineering, mechanical design, mechanical engineering, industrial design, product design, software, CAD, CAD software, Computer Aided Design, Modeling, Rendering, 3D software, Autodesk fusion 360, cloud based CAD, CAD in the cloud, cloud, Free CAD, Free CAD Software, Autodesk CAD, cloud manufacturing, free CAD program, 3D CAD solution

Id: Dfxm8irfEhc

Length: 40min 35sec (2435 seconds)

Published: Tue Dec 01 2015