360 LIVE: Creating In-Context Designs (multi-part series)

hello everyone and welcome to another fusion 360 tech Thursday my name is Brad talus from Autodesk wanted to welcome you and I also have a guest helper this time actually my boss is helping me answer the Q&A today so make sure you only say really nice things anyways we are going to be talking about in context design so what is that well basically what it is is using existing models to help you design the other models in your design so for example I have this belt tightener assembly and we're actually gonna create this frame and this bracket in today's session and you'll notice that this bracket fits perfectly inside of this frame and we're actually gonna use information from the frame to help us design that bracket part now I actually grabbed this from an old drafting book I got from one of my teachers way back in college so here's the here's the drawing that I'm using I've also included the drawing in the description of this livestream so feel free to go ahead and grab that and try and create these parts after the live stream so like I mentioned we're gonna go through and learn how to create two of these parts so let's go ahead and do that this is the drawing that I was talking about looks like I've made some changes so you'll see for example here's the full assembly on the next sheet where I have an exploded view and this is a multi-part series so we're gonna learn how to create part number one in part number two today and then in future series we're gonna go ahead and learn how to create the rest of these parts and then I'll even show how to create this exploded drawing on sheet three is the frame sorry I was looking for the name and on c-4 we have the bracket and you'll actually notice there's not very many dimensions on the bracket and like I said we're gonna use a lot of the material from the frame to help us design our part so this is the drawing I'm referencing and like I mentioned it is available in the description of this livestream okay so I'm gonna start a new design and this drawing is in inches so I'm going to take a look at my document settings and confirm that I'm in inches which I am and then the very first thing I'm going to do is to create a new component and I've mentioned in other live streams I personally like to create everything in components because it just helps organize things so much easier so I can give it a name we'll call this one frame I'll say okay and we can see that we now have a new component called frame I'm going to start by creating a sketch and in this case I'm going to basically draw from the side view because this part is pretty symmetric and I want to keep that symmetry so I'm going to draw from the side view and and the reason I'm doing this side is because I'm going to start with the basic circles that kind of define the pivot points of this frame so I'm just gonna start by throwing a circle on here and I'm I clicked at the zero zero point and it's asking for a diameter in this case it's one and a quarter so I could type in one point two five or check this out I can actually type in 1 and 1/4 and it'll actually figure out the fraction for me and this is pretty important because on this drawing there's quite a few fractions like three thirty-seconds and three sixteenths and stuff so my first tip of this live stream is that you can actually type infractions so one and a quarter okay so that's the bottom circle I'm gonna go ahead and do the top circle now how I'm showing how I'm doing this there's probably multiple different ways of doing this I wanted to show some tips and tricks that I personally do and I'm not saying this is the right way or the only way to do it but this is what I do to help me make sure that I'm creating these parts as correct as possible so one of the first things I do is I want to have a circle that's perfectly in line or straight above this I purposely over exaggerated and put it off to the side and you'll see why here in just a moment so this is 1 and 7/8 so I'm gonna type in 1 and then a space and then 7/8 and I'll go ahead and hit enter now you'll notice that this circle is blue which means it's not fully constrained now the reason I put it off to the side is because I want to force it I want to make sure that it's perfectly in line with this other circle and if I had just drawn a circle that was pretty close like right here and drawn a circle that looks perfectly centered but if we were to zoom up on that we can obviously see that it's off a little bit ok so but that's kind of hard to see when you're zoomed out right there it looks pretty good so this is why I kind of over exaggerate the mistake and then I can come in and say I want that point and that point to be vertical with each other and I physically see it kind of snap into place so that's one of my my tips that I usually use and I teach in my classes I also want to define how far away these circles are from each other so I'm gonna use my dimension tool now I have it up in my tool bar but you could also use the D key D for dimension and these circles are five and a half away from each other so you can see when I typed in that to mention that this circle is now black which means that it's fully constrained okay and I'm actually gonna stop there I'm gonna go ahead and finish my sketch and I'm going to extrude this bottom circle now the reason I'm not going to do both at the same time is because according to the drawing there are actually different lengths or widths depending on which term you want to use so I'm going to do one at a time and again one of my tips that I always use is I pre select my profile I right mouse click and it shows me the commands that make sense in this case I could extrude that profile I could create an offset plane or I could even edit the sketch so in this case I obviously want to extrude and another tip that I like to use is when you're extruding don't be looking straight on at it it's kind of hard to see which direction it's going so I tend to rotate a little bit isometric so I'm kind of looking at it at an angle I'm going to go ahead and start to drag a distance okay like I mentioned this is a very symmetric part so I'm actually gonna change the direction from one side to symmetric and what that's gonna do is it's going to extrude equal distances in both directions you'll notice what I did that it gave me this measurement option and one of them is half length and the other one is whole length so what this is basically saying is this is gonna go about three point three in one direction and three point three in the other direction for a total of like six point six well I want to do the whole length and the whole length that this needs to go is four and a quarter so four point two five or I could type in four and a quarter so now from this back edge to this front edge is four and a quarter inches long because I used that whole length option okay when I hit the okay button you're gonna see the my circles went away and I wanted to extrude that top circle well all it did is under my sketches folder you'll notice that the light bulb next to my sketch is turned off I'll just go ahead and click on it to turn it back on and now we can see that sketch and again another reason I like to use components is you can see how well organized this is so underneath that component is its own origin it's the body and the sketches that have to do with this particular frame component okay so I'm going to do the exact same thing again I'm gonna say extrude I'm going to start to drag will say symmetric will do the whole length and this length is a little bit larger instead of 4 and a quarter it's 4 and 3/4 so I could type in 4.75 or I could type in 4 and 3/4 and say ok now watch what happens I'm gonna expand open my bodies folder and you'll notice right now I have 1 body which happens to be this one as soon as I say ok you'll see that we now have two separate bodies and that's because they're not intersecting with each other so body 2 is the second one I created and body 1 is the first one that we created now as we go through this drawing so basically we started with this cylinder up here and this cylinder down here we're gonna start joining these parts together ok so the next thing I want to do is basically create this open air space between these cylinders and so we can see that there are 2 and 3/4 wide and that's both at the top and at the bottom ok so I'm going to do that next I'm gonna turn off that first sketch I'll say let's create a new sketch and because I I'm keeping everything symmetric you'll notice that it's equal distance to the left equal distance to the right and it's basically on this front plane so I'm going to draw on this front plane and let's just draw a basic rectangle I don't care about what size it is just something like that now according to the drawing it's one inch or this area here is about one inch wide so I'm gonna throw a dimension from here to this edge and you'll notice it's snapping to that edge I can place my dimension and I'm gonna type in 1 and watch what happens to the rectangle you can see how it moves over a little bit to make sure that that's one inch I need to do the same thing on the other side so I'm going to throw a dimension here to here and we can see that this one's point seven zero one nine well I also want it to be one inch so I could type in one but here's another tip I want it to be the same as this dimension over here so while this is highlighted blue I can just click on this existing dimension and you'll see d8 and basically what that's doing is it's referencing that dimension and as soon as I hit Enter we'll see this little formula FX is 1 and if I were to come in and change this to you know 1 and 1/2 that has to change to one and a half so it's a great way to basically type in your dimension once and then have other dimensions reference that okay so I'll finish my sketch we'll go ahead and extrude this and again I'm going to pull in one direction but I want it to go both so I'll just say symmetric and you can see as I'm pulling this profile it's cutting through both of those parts and all I have to do is just go far enough like so I'm just wanting to remove that general area so I'll go ahead and say ok but notice what happened to my body's folder now I have 4 separate bodies which kind of makes sense they're not intersecting with each other or interfering with each other so there are 4 separate bodies okay so let's take a look at the drawing we've basically created you know these four circular areas the next thing I want to do is to create this this beam or whatever you want to call it that goes from the top to the bottom and you'll notice that it's actually tapered and that's because of the different sized circles so I'm gonna show you a cool command called loft that's how we're gonna go ahead and create this so I want to basically create a sketch on the center of this cylinder well if I turn on my origin we can see that the origin is way down here I could do an offset plane a certain distance but let me show you a cool tip under the constructive menu you'll see that we have a bunch of different types of construction planes construction axes and construction points well I want to put a plane that's horizontal through the center of the cylinder but if I do this little pull down you'll see that there isn't really I'm there's a tangent plane but that would be on the edge I want it to go through the center so what I'm gonna do is actually create an axis through a cylinder it's asking for the face I'll just go ahead and click on this circular face and you'll see this little blue line up here that's going through the center of that cylinder and I'll just say okay and we now have an axis that's going through the center of that particular component now check this out I can actually say plane at an angle I want to specify where that plane is and notice even the little tooltip says creates a construction plane through an edge or through an axis or through a line so I'm going to say plane at an angle and it's asking what's the line I'm gonna go ahead and click on this axis and you'll see that it's putting this construction plane and I can put that plane at any angle I want you can kind of see it rotating around that backsies okay well in this case I obviously want it to be horizontal I'm gonna leave it at zero and say okay and I now have a plane that slices right through the center of that cylinder perfect okay so I'm gonna go ahead and turn off these two parts so I don't need to see right now I just want to kind of focus on these in fact I might even turn off this little one at the bottom for now so I'm just gonna worry about this guy and I'm gonna say create a sketch okay I'm gonna show a couple tips here if I do my line command and I get near the edge you'll notice that it's not snapping to the edge of the cylinder and that's because there's physically no geometry if I turn off the part you'll notice there's no geometry there for it to snap to well I want to basically grab the information from this part so while I'm in sketch I can use the project command or the shortcut is P for project now in the project command there's actually two options and I'm going to show the difference between the two so you can see specified entities or the whole body so what specified entities does is it allows you to basically click for example this edge or this edge for example I want to specify the specific edge that I want to select okay or the specific face I want to select so I'm gonna click on that face and say okay and if I were to turn off the body notice what it did it projected the two edges of that cylinder but you don't see a line going across the top or the bottom and that's because there really isn't an edge on a circular face okay so I'm going to undo that let's go ahead and undo that and I'm going to do the exact same thing again I'll say project but this time I'm going to change it to bodies and I just have to get near the body you'll notice it's not letting me select edges for example it's gonna project the whole body and when I say ok and turn that off you'll notice in this case it kind of did like a silhouette projection where it did create lines all the way around and that's what I want in this case so I want to be able to grab on this edge here now notice like when I get with the line command it's gonna snap to that corner it's gonna snap to this edge and it'll even snap to this edge and even find for example the center of that edge so there might be situations where when you want to grab information from an existing model you'll have to project that information onto your sketch and then you can use that information to create your sketch and that's what we did here okay so I projected that I now like to use the ellipse command because I want to create a half inch wide ellipse once again I'm going to purposely over exaggerate and kind of go off away from where it needs to be so I'm going to click the center point and then the end point and then I'm going to start to define the width and so you can kind of see now it's it's asking for the width of this ellipse so according to the drawing it's point five and I'll say okay now obviously I'm way off but I did that on purpose okay now I can come in and say I want that point to be coincident with this line so I'm going to click on that point I'll click on that line and you'll see how that point is now coincident with that line I'll do the same thing here that point that line and you can see it still kept my point five wide dimension but now I know for a fact that this ellipse is exactly touching those two edges now it's still blue because it's not fully constrained so the last thing I'm going to do is throw a dimension let's just go from there to this edge and that according to the drawing is point one two five we'll see that that ellipse is kind of slid over the points are still coincident on those edges and it is now fully constrained which is good I'm done with that so I'm gonna say finish sketch and you can kind of see what we did we we drew an ellipse that's the exact width of the cylinder and it's a certain distance from the edge so now all I have to do is kind of do the same thing down here on this bottom part so let's go ahead and turn those guys off now in this case I actually don't have to create an axes because we we actually created that circle right in the center so it already has an axes and it already has a plane so I'm gonna go ahead and just sketch on that plane and I'm gonna do the exact same thing P for project I'll make sure that my body's option is selected and I'm just going to go ahead and project that body we can see sure enough it's a full rectangle and then I'll come in and create the ellipse once again kind of off here in space a little bit making sure that's 0.5 wide I'll do the coincident constraints like so and then finally I'll throw my dimension on here to this edge and let's just make that the point one two five like we did before finish my sketch okay let's turn those bodies back on and let's turn those two sketches back on so now I have a longer ellipse at the top and a little shorter lips at the bottom and I want to connect the two so we're going to use the loft command and you can kind of see by the thumbnail it basically goes from one shape to another where sweep kind of takes a profile and goes along a path Loft is like how you would do like an airplane wing where it's you know wide at the fuselage but kind of narrow at the tip of the wing that's you would use the loft command for that so I'm going to say loft what's the profile well that's one profile and this is the other profile now notice what happens when I do that it kind of turns red and it looks like it's kind of cutting some stuff away and in fact it is you can see the operation is set to cut well instead of cutting the material I want to say join and now you can see that it's taking that shape and going down to that shape and it's kind of join together I'll go ahead and say okay and we now have this really cool looking kind of tapered face that goes from the top and it's tangent right down to the bottom okay I'm going to turn these other bodies back on now that was a lot of work I mean it wasn't really but a lot of talking I want to put this over here instead of recreating it let's just come in and say mirror what do we want a mirror well by default I think it's usually set to faces I would come in here and change it to features and say I want to mirror that loft that we just did what's the mirror plane well I click on select it brings up my origin right there and I can click on that plane because you can kind of imagine like placing a mirror in that direction you would see the reflection on the other side and so that's what it's showing there and as soon as I say okay we've now mirrored that other arm to the other side okay we've actually got kind of the complicated part done the the next thing to do on this part is to go ahead and update this is to create this kind of this i-beam looking shape I just hit updates that's updating the drawing on this i-beam shape right here and it's one inch up from the center of this hole and then all of the other dimensions that I'm using are taken from the section Bibi right here okay so I'm going to create a new sketch and I want to kind of draw the eye shape of it so I'm gonna select this plane that goes kind of through the middle of it like so okay here's another couple tips I'm going to share with you we want to draw that Eyebeam shape but you'll notice that these lines are tapered so it's not a perfect i-beam shape it's kind of a tapered i-beam so I want to use information from these legs so I'm going to come in here and project those legs so I'm gonna say project I'll do the body will click on that guy say okay and if I were to turn off all the bodies you can see how it projected that geometry okay so let's start building the i-beam I'm just gonna draw a line somewhere across okay now here's one of the tips that I'm gonna share with you if I go ahead and place that line you'll notice that you know it's out here in space and I would have to come in and trim these and to trim back to this edge right here so instead of going out in space like that I'm gonna say line and all I have to do is get near this edge and I'm gonna go ahead and click you can kind of see how there's a little X right there so I'm gonna go ahead and click I'll make sure I'm horizontal you can kind of see let me zoom up here it kind of snap into place so it's snapping to the geometry to this sketch geometry so you can see those two black dots are on that edge now here's what's really cool about this I'm going to throw a dimension on here so let's go from that edge to the center of the circle and that's supposed to be one inch now watch what happens to those black dots they actually follow the taper of this arm and that's because they know that they're supposed to stay coincident to that edge so it doesn't matter if I came in and said make this four inches you'll see how that line is wide way up there compared to one inch down here so I personally like to click on the edges and have them catch like that so I'll do another one up here somewhere I'll go something like this making sure and then I'm going to do a line down through the center and so you can kind of see I started to create the basic shape of this now somebody might ask well couldn't you have just offset this original line to go up here well let me show you what would happen if we had so I'm gonna say offset I'll click on that edge and I'm gonna start to drag up and again I'm over-exaggerating but notice what's happening here it doesn't know that it's supposed to stay coincident with that edge you're basically taking a certain length edge and offsetting it a certain distance so that's why I didn't use the offset to create that particular line okay now I am gonna use offset to create the rest of this to show you how would you work around that issue so for example I'll say offset I'll click on this line and tell it I want to go in this direction which in this case is in the negative direction well I want it to go 3/16 of an inch so I could say minus 3/16 and you can see that it's actually going to figure that for me I'll go ahead and hit enter but if i zoom up we can see that particular issue well there's a really cool command under modify called trim or extend trim is if the lines too long you want to trim it back extend all I have to do is get near the line it's kind of hard to see but you'll see a little red line up here and now it's extended over okay and I could do that there also and it's extended to that edge so you just have to kind of be aware of that now what would happen if I didn't do that is it wouldn't think it's a closed profile so let's just go ahead and do the 3/16 there and in this case you'll notice that the line is too long so I could come in and say trim all I have to do is get near that little segment it'll trim back get near that little segment and a little clips should zoom it up a little bit more let me zoom up hit trim and I'll click on that little segment right there okay now the last thing I want to do is to create my offset from the middle so I'm going to go ahead and click on that guy and it's gonna be a total of three sixteenths wide and let's say I'm really bad at fractions I want to go 1/2 of 3/16 so I could type in left parenthesis and do 3/16 right parenthesis and you can see it gives me a quick preview what that's going to look like and it's basically solving for 3/16 but now if I say divided by 2 you'll see that it came back a little bit now why did I put it in parenthesis well because it's kind of mathematical operations we need to solve that first and then divide it in half otherwise it would be like 3/16 divided by 2 and what's the answer to that right so in some cases you might have to throw the operator in some parentheses like so okay and I'll do the exact same thing I'll grab this guy and move it in this direction but we can see that's in the minus direction so I'm gonna say left parenthesis minus three sixteenths divided by two and you can see how it kind of snaps back in place so now we can kind of see our eye beams shape and the last tip I want to show here is if I were let me just turn off the bodies you'll notice that this is broken down into a whole bunch of little areas okay when I go to extrude I'm actually gonna have to select all of these areas to extrude okay well this middle line right here I don't need it to be an object line so I'm gonna select it and click on construction and you'll see how it's now a dashed line and now instead of being split into two rectangles it's not an object line anymore so it actually allows me to select way less areas to extrude so I'll select those and say extrude I'll turn my bodies back on so you can see what's going on here I'll start to drag and again I want it to go symmetric so I'll come in here and say symmetric now how far do I need to go well I really don't know the answer to that I don't know what the distance is so I'm gonna change that from distance to all now when I do that you can see that it's gonna extrude all the way through and it thinks oh you're wanting to cut geometry away no I want to join it together so I'm going to just change from cut to join and we can see how it's going to take that I beam and extrude it to these tapered shaped arms what I'm hoping you're seeing here is we're keeping our sketches pretty simple I'm not doing lots of fill it's and all that kind of stuff it's circles and ellipses and rectangles so far and we're extruding two phases we're extruding two objects etc now we're gonna start finishing the design of this guy okay all of these parts are touching but you'll notice I have three separate bodies I have that guy and then I have the small cylinder down here and then I have this large cylinder up here well you know remember they were separate bodies well they still are and I want them to be all one body under the modify command I can come in here and say combine I want to combine these bodies together so I'm gonna say combine what's the target basically it's asking what are we combining two so I'm going to say that's my target and then what tools are we combining with so we're gonna say that one and that one now watch what happens when I say okay we are now back to one singular body under this component so the key thing here is you can have multiple bodies and simplify your design using multiple bodies and then combine them together once you've got more of your design kind of like how we now have all of these arms together okay again if you have any questions or comments throw them out in the chat Jaime's out there helping me out so thumbs up if you're learning anything you know it other tips and tricks you want to see just let me know in the comments and I'll try and show those okay let's take a look at the drawing now and I haven't had a chance to look through the chat I'm guessing some of you were like well how come you didn't extrude the holes through at the same time that you made these cylinders and I very well could have looks wrong button but what I wanted to do here is show you a really cool trick now you'll notice my axis is still showing up that's under my construction menu right here and I can just hit that little light bulb to turn it off or turn it on so these planes and axes I can just turn those off using that little light bulb okay so I didn't draw a hole here originally because I wanted to show the whole command and there's a really neat tip with this that I use all the time so I'm gonna say hole and it's gonna ask for a placement which face again I purposely click away from where it needs to be so I'm going to click up here and you can kind of see that it put that circle right there I'm going to zoom up here and you'll notice this little blue crosshair dot thing in the center of that circle well I'm gonna start to drag it and move it out of the way and you'll notice a little dot right in the middle of this circular face so all I have to do is get near that circle and you can kind of see it snap right to the center of the cylindrical face according to the drawing this hole is 7/8 ream so affectin 7/8 and you can see right here it's showing that's the diameter of the shaft now if I look at it from the side we can see that it's not going all the way through so I could drag this arrow until we went far enough or I could just click on this face and you'll see it snap the correct distance so I don't have to type in any dimensions I'm saying drill through to that face now there's lots of options in here I'm doing a simple hole we could do a counter board hold countersink holes but then you also known as flat and angle so it's only go to the side if this was you know a blind hole where I didn't go all the way through you would have a point at the end right in fact if I drag this back a little bit you can see how it doesn't go all the way through so I'd have to make sure that I'm going all the way through in that case or I'm just gonna change it to flat okay and I'll say okay and it will create that hole for me okay now one thing I'm really bad at when I'm doing these live streams is I just keep talking and demoing and stuff like that I should be saving every so often so I'm gonna do that now hopefully you do that also so I'm gonna come in here and hit save it's in the correct location I'm just gonna call this bracket part actually I'm sorry frame frame part and save it okay so now we're gonna see that go from version zero to version one once it's saved and there we go so you should save often now I want to put a hole here now you're saying well why didn't you do it at the same time well because they're actually two different sizes and you can actually see that kind of in this 3d view a larger hole here and a smaller hole with a keyway that goes through it so the smaller hole is a 5h dream so I'm gonna do the exact same thing I'll click on that face I'll use the whole command out of my marking menu or I could get it from my create menu but I'm just gonna do that and you'll notice that's kind of off to the side all I have to do is grab it you can see that little blue dot I'm just gonna get near that blue dot and it's gonna snap right in place what's the diameter well in this case it's five-eighths and so you'll see sure enough the preview is smaller than that one and how far do I need it to machine well I'm just gonna click on that face and say okay there we go and then finally the hole through the bottom so I'm gonna repeat my last command I'll just click cut off to the side on that face notice it remembers my last dimension which is great the five eighths so I'm just gonna drag this down to that point and in this case they are both the same size so I can drag this and click on that face and have it drill all the way through in this example I'll say okay okay looking at the drawing there's a whole bunch of blends or fill it's on this i-beam part and like I mentioned before I kept my sketch very simple I didn't do all of these phillotson my sketch I just did you know sharp corners extruded it and now I'm going to use 3d fill it's to round over these edges okay so let's do that we can see that the the edges are 3/32 and then the rest of them are 1/8 so I'm going to do the three thirty-seconds first so let's just go ahead and click on an edge right mouse click and it shows me the commands that make sense fill it or chamfer I'll go ahead and say fill it and again I'm really bad at math so I'm going to type in free / 32 and it figures that out for me and then I'll just go ahead and click the rest of these edges and you'll see it gives me a nice preview of what that's gonna look like I'll come around over here I'll say that edge that edge that edge and that edge say okay and we've fileted all of those edges okay now there's a bunch of other edges in here that need to be fileted okay so I'm going to select one of them I'll say fill it and these are supposed to be 1/8 so I'll type in 1/8 but notice how long it's gonna take me to select all of these edges I'm kind of walking around grabbing all of these edges and that's gonna take quite some time so here's a neat trick I'm gonna cancel out I'll come into my Philip command and I'm just gonna draw a selection box around the whole eye beam like so what's the size Oh point one to five and it instantly fill its all of those edges at once I didn't have to manually click on them and hope I don't make a mistake or miss click or slip off the holding down the shift-key or whatever so hopefully you found that tip kind of cool I use that one quite a bit okay and then the rest honestly is there's a fill it on this edge that's point one two five and on that edge and on this curve and on that curve now you'll notice I'm selecting all four of those at the same time and that's because they're all the same size so instead of doing and having a whole bunch of Filat features in my timeline I'm kind of grouping them together so these are all my 0.125 s and then down here I'll do a new Filat and these are 1/16 so I'll say that edge that edge that edge and I'll just come across like so and these are all going to be 1/16 in radius and there we are we are done with the design of the frame now you know when I first looked at this I'm like wow this is kind of a complex part how am I gonna do these tapered faces and your curve blends and stuff like that so I tried to break it down into its simplest form and like I said there's probably other ways you could make this part so when you give this a try if you make it a different way let me know leave a comment you know on the YouTube video at a later date and say how you went about doing it because I'd love to learn other ways okay so I'm gonna save obviously cuz we're finished and I'm gonna say finished frame and the next thing I want to do is to create the bracket that's gonna go in between this frame and this is where the in context starts to come into play so right now my frame is my active component well I want to activate this i shouldn'ta called a frame part it's actually we're doing the whole design so I'll rename that later but I'm gonna activate my top-level assembly I'll come in here and say new component and the new component is gonna be the bracket so I'll go ahead and say ok and you'll notice that the frame kind of ghosts out a little bit I go ahead and minimize all this stuff and you'll notice that we have the frame component and now we have this bracket component with nothing underneath it okay so let me jump to the drawing we'll jump over to the bracket drawing oh yeah so we can kind of see pretty simple shape kind of triangulated the the holes are three inches apart we kind of know that these arms are half-inch wide and we know about the size of the holes so what I'm gonna do is start by creating an offset plane now why am I doing this well the bottom of the bracket sits about an inch and a quarter below these holes and I know that the this plane right here is slicing right through the middle of those holes so I'm going to offset that plane down I can see in the negative directions I'm gonna type in minus 1 and 1/4 or 1.25 and I now have a piece of paper that's sitting an inch and a quarter below the center of these holes and I'll sketch on that plane so I'm just gonna select it and say create sketch you can kind of see my screen reorient it but let me rotate a little bit when we can see that we now have a piece of paper below that frame and that's what we're gonna use now I want to grab information from this frame so again I'm gonna use the project command but notice what happens when I hover over the body it's kind of like I mentioned before it's kind of doing a silhouette projection if the body option is selected so you can kind of see looks like a little barbell or dog bone or something like that I'm gonna change to specify entities and now you can see I can actually specify what do I want to project okay now I've kind of dug myself a little bit of a hole right here because I want to go to this edge but that edge is shorter than this edge because of the filler and this will make more sense here in just a moment but I'm gonna project both of those edges by selecting that fill it I'll also project that fill it and you can see that it's taking the information and bringing it down onto that plane well I'll say okay okay the next thing I want to kind of do is kind of create the that tapered look so I'm gonna draw a line out here in space I know it needs to be three inches long so I just did that out there in space and it's three inches long now I'm doing something a little bit different that you guys probably aren't used to me doing I'm usually looking at everything orthographic right I'm kind of looking straight down on the piece of paper but doing this in context design we can actually look at our piece of paper from any direction in any angle and some kind of sketching in this isometric mode okay now I want to put this centered so I'm going to say midpoint that line to that point and you'll see that it took the line that's three inches long and it put it right in the center and because it's constrained I can tell because it's no longer blue now I don't want this to be an object line so I'm going to click on it and hit the construction icon over here and you can see that it turned it to a dashed line now I you know this might be confusing to some people but I am actually old enough that I learned drafting on a drafting board where you drew light pencil lines that kind of got your shape the way you wanted and then you would come back and use a harder pencil or or ink even and trace over those well those light pencil lines were what we called construction lines and then we went over and trace them and those were the object lines and that's the exact same thing in fusion we've got construction lines and we've got object lines okay so now I can throw my circles on here and here's another tip according to the drawing it's asking for a half-inch radius circle and you'll notice it's asking for a diameter right now well I could do the math so I could say you know 0.5 times 2 or something like that or I could just draw a circle I don't care what size it is in fact I'll draw another circle I'll make it even larger like so doesn't matter then I'll do my dimension oops D for dimension and I'll click on that and again notice it's asking for a diameter well if I right mouse click it gives me the option to specify a radius so you can see diameter is checked I'm going to click on radius and now it says R zero point three nine three zero line well I can come in and say I want that to be 0.5 and it's gonna make that circle a half-inch radius I'll do the same thing here it's it currently diameter I'll right-click and say radius I want it to be the same as that guy so I'll just go ahead and click on it and it's gonna be the same it's gonna reference that for me so that's how you can do radius size holes okay the the next thing I want to do is create a line that comes over here and this will make more sense why I had to do these two lines now well I want a line to be tangent to the circle and another tip is if you hold down your Shift key when you're clicking on that circle so I'm holding down shift and I'm holding down my left mouse button you'll notice that this line that I'm creating is constantly staying tangent to that circle as soon as I let go I can let go shift right now but if I were to place a line you'll see that it created that tangent icon for me okay so a neat little trick instead of having to come back and do tangent I'm just gonna hold down shift click and hold now I want to go to this distance here but I want to be up at the height of this other line right here so all I have to do is get kind of near it in fact let me let me zoom up a little bit more before I do this because I want you to kind of see what's going on here let's do let's do that I'll say line hold down my shift key come across so I need to be here but I need to be up a little bit but you'll notice it doesn't know how far up it needs to go well all I have to do is hover for about half a second and now you can see it's in line with that other dot and then I'm just gonna come back here and it's kind of hard to see cuz my cursors covering it but there's now two dashed lines and it's basically saying you're lined up with this dot and you're lined up with that dot okay so all you have to do is hover for about half a second and I'll just go ahead and click that I'll do the same thing here I'll just kind of hover and hover then hold down my shift key as I'm moving along and we'll see it actually kind of snap into place boom and you can see that little tangent icon right there okay so I'll do the same thing over here and I'm hoping this kind of makes sense and once we extrude you'll see why I had to do that but I'll go ahead and hold down my shift key again I'll come to here come to here move over a little bit and we can see that we're now lined up same thing with that and hold down my shift key get near that edge and you can kind of see it snap into place and I now have the shape of my part I'll finish my sketch notice because these are object lines I could have trimmed these back but instead I'm just gonna select those as part of my profile also right mouse click it shows me the command that makes sense in this case I'll say extrude how far point five according to the drawing so I'm going to type in point five and say okay so let me see if I can show it from this direction it'll be kind of hard to see but this edge is now perfectly in line with that edge of the circle and with that edge of the circle if I hadn't done that they would have been lined up with this edge and this edge which is incorrect okay so now what well now I want to create these little wings whatever tabs if you want to call it that but we're gonna use the 3d model to help us with our design I did throw a dimension on here but we're actually not even going to use that dimension so check this out this is actually pretty cool okay I'm going to create a new sketch because it's symmetric I'm gonna click on this kind of this horizontal or this right-side plane right there so we're slicing through the center of our parts right there and I'm gonna use our favorite command the project command so I'll say project now I could do the whole body but I don't want to in this case I want to be very specific so I'm gonna say specified entities and notice as I move around how it's trying to project these faces and edges and stuff on to that piece of paper that's slicing right through the middle well I want to grab this outside edge so I'm going to click on that edge and you can see how it projected it well I also want to know how far down I need to go so I'm actually gonna project the face of this part and this is what I think so cool we're actually grabbing information from one component and grabbing information from a second component to help us with our design I need to create some vertical walls here you could do this many different ways I find using the rectangle command pretty fast and again I'm gonna over exaggerate my rectangle so it'll look something like that okay but I was careful to make sure it cuz snap to that bottom line which it did well I want this line to be tangent to the circle so I'll say tangent that line to that circle and you'll see how that moves over I'll say that line to that circle and we can see how that moves over but I got a bunch of extra garbage up here I want this line to be at the same level as this center line so I'm going to use coincident coincident means they need to occupy the same space so I'm going to say that line and that point and you'll see how that line now occupies that point and we have really nice straight lines everything is no longer blue so we know that it's fully constrained and I'm gonna say finish my sketch again I could have trimmed I could have done construction lines if I wanted to it's really up to you but I'm just gonna select those three regions right mouse click and say extrude I start to drag so I get kind of a visual picture of what its gonna look like well how far do I need to go well instead of typing in a dimension I can actually hover over this face right here and you'll notice it says snap - I'm just gonna click on that face and you'll notice that it extrudes to that face I can also come here and say symmetric and it's gonna go symmetrically both ways so again instead of having to type in distances and whole lengths and all that kind of stuff all I did was click on existing geometry to help define the width of that part okay now I want to make those little stand offs or whatever but this is one big solid chunk here's another neat little tip I want to work on just the bracket and the frame is kind of in the way now I've used it as much as I need to in this case so I don't want to see it anymore so I could right mouse click on bracket and say isolate and it would turn off all of my other components and it isolates and just displays this one so you can see sure enough it turned off my frame okay so again keeping things simple I'm gonna say create a sketch on this plane right here if I try and create a line or a rectangle you'll notice it's not snapping to this edge right here so I need to project that so I'm gonna come in here and say project I'll rotate it isometrically so you can kind of see what's going on here I'm gonna project that face or I could do an edge it really doesn't matter I'm gonna do the whole face say okay now notice when I do my rectangle command it is snapping to that projected edge okay so I'm just going to go ahead and draw a rectangle here something like this doesn't matter what size I'll throw a dimension on here I'll say from here to here needs to be 0.5 according to the drawing and the same thing here to here and I'll click on this existing dimension instead having to type it in I'll just click on that one say okay and it's referencing it so now it's basically centered if you want to look at it that way we'll grab that profile extrude you can see as I start to extrude it kind of cuts that away well I want to go instead of a distance let's just extrude through all of it symmetrically so it's extruding as far as it needs to go through the model so I change that to symmetric to make it go both directions and I changed the extent from a distance to all and we'll say okay there we go again I'm gonna use my favorite whole command so I'll say whole click off to the side a little bit drag that down where it needs to go and kind of automatically snaps right to the center of that radius and to me this is so much faster than typing in dimensions and projecting faces and creating more sketches or whatever these are supposed to be a half inch so I'm going to type in 0.5 how far does it need to go well I could do just one side if I wanted to or I can drag and have it go all the way through do both holes at the same time in one feature and then the last thing with this and we're just at the top of the hour so there's lots of blends that kind of knock all the sharp edges on this so I'm gonna go ahead and do those according to the drawing so I'll select one edge right mouse click and again it shows me the the two commands that makes sense in this case fill it and you'll notice that when I type it in it actually goes all the way around even though I only clicked one edge it went all the way around and that's because of this tangent chain command what that means is if I have an edge selected is there another edge tangent to it yes there is okay go ahead and select it is there another edge tangent to that yes there is go ahead and select that edge now this one is not tangent to it it comes at a sharp angle so that's why it's only selecting those three edges okay now I could come in here and select all of these other edges but that would take quite a few clicks so check this out I'm gonna just say okay on those two edge loops that we selected I'll hit f4 fill it again but instead of selecting edges I'm gonna select this face I'll type in 0.125 and watch what happens it selected all of the edges of that face for me so saving quite a bit of time I'll say okay let's go ahead and save and I could come in here and say finished bracket we'll turn the frame back on and again here is one of the reasons I really like using components is that you'll notice my bracket component is active right now these are all of the steps that were necessary to create that bracket not very many if I were to activate the frame here's all of the steps that were necessary to create that frame and you'll kind of notice I sort of grouped things together I kind of waited and did all my Philip's to the end I kind of did all my holes together and I've seen this question a couple times so let me go ahead and cover this I'm gonna select all four of those fill its features right mouse click and you can see we can create a group and you'll notice that it's now a single icon and if I hover over it it shows all of the features that are inside of that group and I could expand that open to see them or I could minimize them but my favorite thing is you can rename it so I'm going to right click and say rename and I could call this small Phillips or something like that okay I could group these together and I could rename that and say main holes or whatever and I can I can even give dimensions or something like that but now when I hover over this group I can see oh those are all my small Phillips these are all my main holes you can actually rename anything you see in here so for example right here I could rename this guy and call it you know hole sketch and as I'm going through like this one just says sketch - but now when I hover over this I know that that's the sketch that kind of defines the holes or the cylinders I should say so kind of a cool tip there that you can actually rename anything in your timeline and you can group them together okay so I'm going to go ahead and act my top-level assembly and now we can see all of the features that were used to create these two components which in reality I think this is actually a pretty clean it did not take a whole bunch of steps to create these let's for fun come in here and do a section analysis I'm gonna use my origin here let's cut right through there and we can visually see you know solid objects and that these are touching perfectly right there and you'll see we're gonna create the screw that's going to go in here and thread into this section so we can visually see the different size holes and everything okay so like I mentioned this is part one of a multi-part series I'm going to continue creating the rest of these parts in context we're going to use the 3d geometry to help us with our design so hopefully you learn something new today make sure you subscribe keep an eye out for those other live streams we're actually doing a ton of live streams Jason's doing a bunch sweet Aaron's doing some Angelo or machinist has been doing a bunch so it'll probably be about another two weeks or so before I can actually have a free timeslot to do this next one but make sure you subscribe and we'd love to see your comments and hope you have a wonderful rest of your day thank you

Channel: Autodesk Fusion 360

Views: 13,484

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, photogrammetry, computer aided design, free software, 3d modeling tutorial, in-context design

Id: x9l-bJvnVR8

Length: 69min 35sec (4175 seconds)

Published: Thu Jun 27 2019