360 LIVE: Creating In-Context Designs (part 2 of 3)

hello everyone and welcome to another fusion 360 tech Thursday livestream this is part two of our in context design last time we we met we did this we were started to work on this assembly here and today i'm gonna continue creating some of the parts i need to turn off my audio just a second sorry guys so i want to start out by answering a couple questions that have come up since this first one and one of them was what about tolerant sane and what do i mean by that well as we look at this assembly here when we created it the last time i basically used the inside of this part to define the width of this and you can see that there is zero clearance in here and again we're giving you methods and ideas on how you can design but when you go to manufacture this you have to have the experience and the knowledge on how is this going to be manufactured and so typically what people will do is they'll use for example tolerance blocks on their drawings when they've dimension their drawings they might have a tolerance block in the corner that says any dimension that's like one decimal place might be a tolerance of you know five thousands any decimal that's a - i'm sorry i need to mention that's a two decimal places might be like mm or something like that another way is you could actually physically model in the tolerance if you wanted to so for example i'm just gonna press this in a little bit let's just go - point zero - and you can physically see now there's some clearance in there so with that said i'm not telling you this is how you should do it hopefully you'll do the research or have the experience on you know figuring out how would you physically manufacture these parts there's many different ways you can do this and what i'm showing here is kind of that in context idea where you're using existing models to create new models and I'm going to continue with that today okay so let me jump in we left off here last week and I've uploaded the drawing with a bunch more sheets on it so it has for example the the shaft drawing the bushing drawing etc this is in the description of this livestream so you'll want to go ahead and download this latest drawing set so we're gonna start with this pin now you'll notice I have all of the dimensions on the drawing and I could model this pin using these dimensions but here's where the in context part kind of comes into play and I think this is really fun we're gonna use existing geometry to help us design and what do I mean by that well when I'm designing parts you know I might start with maybe like this base or something and then I start creating the other parts around it and I'm using existing geometry to help me with that so for example I know that I want a pin that's gonna go through here but you'll notice that we have two different size holes in here and I basically want the pin to rest against maybe this face right here for example so I'm actually gonna start out with a very simple design so the first thing I'm gonna do let me go ahead and delete this and remove it because I already had it in there the first thing I'm going to do is create a new component so I'm going to right mouse click at my top level and say new component and like I've mentioned in previous live streams you want to try using components as much as possible because it really does simplify your design you'll notice all my other parts are kind of ghosted out right now and my pin is the current active part or component I should say so what I'm going to do now is just create a sketch on this outside face and according to the drawing the diameter is 7/8 so I'm going to go ahead and draw a circle that's 7/8 in diameter so I can type in 7/8 which is kind of cool I don't have to do the math in my head automatically it it'll do it for me so you can actually see they're 0.875 and believe it or not I'm actually done with this I'm gonna finish my sketch I'll select the profile that I want and say extrude now I know that I want it to go a certain distance this way in fact I want it to go to this face I'm gonna go ahead and just click on that face but I also know according to the drawing that it needs to go to the right a little bit so one of the tips I'm gonna be sharing lots of tips in this live stream one of the tips I'm going to use is instead of just saying one side I can say two sides and that actually allows me to go to different directions so I can go to the left one distance and to the right another distance in this case I need to go 3/16 of an inch now notice there's a negative sign so I'm gonna have to type in minus 3/16 and I'll say ok now you're probably sitting there going well if we turn on our analysis we're obviously clashing with our other parts and sure enough we are ok oh it's not Laura genetic analysis so I'm gonna use these existing parts to change my design I'll come in here and say modify combine now this is a really powerful command and unfortunately some people like think all it does is combine parts together but it's actually 3 or 4 commands in one okay so I'll go ahead and say combine and it says what is the tar well this is the target and then what is the tool what are we going to use and I'm going to select my frame and notice the preview and that's because of this operation I mentioned it's not just a combine like join things together you can actually join things together combine them together or you can cut them apart or you could say intersect only keep what's intersecting between the parts well in this case we're going to say cut and I'm also going to select that other shape this other part and notice what we're getting it's basically taking this solid cylinder that was going all the way through these parts insane I'm going to remove what's clashing basically I'm gonna cut that away I'll go ahead and say okay let's turn on our our analysis again and you can see what our pin looks like so we instead of having to create a whole bunch of dimensions or whatever and again this is basically like right like I mentioned earlier zero tolerance but this pin will fit inside of these parts when they're manufactured using tolerancing okay now with that said one of the things I typically do is like okay that looks pretty cool and I notice my overall length of this pin is one and a half and I want to verify that okay especially when I'm doing this kind of design even though I've got a fully dimension drawing I want to make sure that that's one and a half so I'm gonna click on this measure I'll click on that face there and this face over here making sure I grab the face and notice it says the distance is 1.4 3/8 so even though I use this really cool trick the cylinder wasn't quite long enough okay because I basically captured to this back face right here when in reality the pin actually sticks out a little bit so how do we fix this well here's and here's the first really cool trick I want to show I'm gonna go ahead and click on this face and I wanna make sure you'll notice when I click on it it actually selects the wrong face I'm gonna click and hold to make sure I get this end face right here all right mouse click and do a press pull so I'm basically gonna add some geometry to this well how much geometry do I need to add I don't know and I don't want to have to know I don't want have to do a whole bunch of calculations or whatever but what it's saying is I've added point 5 7 8 inches of material from where it was well check this out I hit this little down arrow and I can say reinker and what this is going to allow me to do is instead of measuring from this edge I can measure from way over here so I'm going to say reinker I'll click on that face and now you can see that dimension in there says two point zero one six right so it's saying that this face is - well you know 2 plus inches from this face and I can come in and say well I know that that has to be one and a half so I'll say one point five and sure enough the total length of this pin now is one and a half inches so I used that reinker command instead of measuring it from this face here I wanted to measure it from this face way back here I see a couple thumbs up sign up in the chat I forgot to mention Aaron is back and he is helping me out also my buddy Angelo looks like he's on so if you have any tolerance type questions since he's a way better machinist than I could ever imagine being he might be able to answer those for you so Aaron and Angelo thanks again for helping out so yes I think this is a really cool trick with that that reinker command so believe it or not I'm almost done with my design you can kind of see how the 3d model or models helped shape this design right here this this taper down you can kind of see so I need to throw in a chamfer it looks like and I need to throw in a radius and then this slot so let's just go ahead and do that really quick so I might put my chamfer on here so let me click on this edge right there say chamfer and again it was 1/16 according to the drawing and there we go now I get this question a lot I need to put that slot through the side here but there's also a Phillip that goes all the way around and doesn't matter which order I do the same and the answer is it really kind of depends so for example if I put the slot through first it's going to require me to select two edges to put that fill it on but if I put the Phillip on first and then machined in the slot I'd only have to select one edge now you might be saying one edge versus two edges well if you're doing a lot of CAD design every little step' matters as it adds up so I personally like to make things as simple as possible so I'm going to put the fill it on first because I don't only have to select this one edge so I'll select it say fill it and according to the drawing it's 1/16 and you can see how it went all the way around and then the last thing I need to do is put my slot through there so I'm going to click on the face say create the sketch and here's another neat little trick I'm gonna say rectangle and I've shown this before I could go into create rectangle and come down and pick whichever rectangle I want or I'm in no command I could hit our four rectangle and it shows me my three rectangle types over here in my sketch palette and I'm actually gonna do a center rectangle I'll grab the center here start to drag and I know the thickness or the heighth I should say is 1/8 so I'm going to type in 1/8 and honestly the length doesn't matter so I'm just gonna hit enter so I know for a fact that this is an eighth of an inch tall and I'll just say finish my sketch then I can select these profiles let me grab the profile here say extrude or press pull they're pretty much the exact same command doesn't really matter and I like to start to drag to visually see what it's gonna look like and I can see that it's going in the negative direction okay so I'm gonna type in minus 1/16 of an inch okay now I'm typing in a dimension right there and I know for a fact that it's going - 1/16 well check this out I can also I'll grab these profiles again say press poll or extrude I can actually click on like an edge for example and you can see that it's gonna snap to that edge so instead of having to type in a distance I could click on a face or an edge and it's gonna snap to that particular edge so there we go we've actually very quickly finished our pin and again what I'm showing here is I'm not saying this is how you should design or how you have to design it's more if you're coming up with an idea and you want to just kind of like start building things on top of each other and say I can I know this is going to be supported by a bracket there's gonna be some pins that go in here that might have the Machine you can use the existing geometry to help you speed up your design now to speed things up even more I know that I need to have a pin on the other side so I'm going to use the mirror command so I'll say mirror what's the pattern type by default you'll see that it comes up as faces but we also have bodies features and components now which one should I use well features is like a Filat or a chamfer or a hole or something like that these down here and my timeline on my features like here's the chamfer the Phillip the extrude etc bodies their effect if would be what I would use if I have just like a single body but I'm actually working with components and you can tell that by these little cube icons that we see in the browser and we also see that cube icon right here so it makes sense for me to mirror the pin component so I'll say components which is my object the pin what's my mirror plane as soon as I click on select you'll see that it brings up my origin and I can actually select him kind of rotate around so you can kind of see what's going on here there is my origin if fact if I turn that on you can see that I'll click on it and it's gonna mirror that pin across the center of this whole assembly I'll say ok and then we'll see that we have pin and pin mirror ok so we now have this put together down here the the next part we want to work on is I'll just go to the next little icon here is the shaft part and again I mentioned a majority of it but again we're gonna use 3d geometry to help us out now I'm going to create this slightly different just to show you other methods ok something jump over here again what I'll do is right-click at the top level and say new component and I want to name this I'll call it shaft we can see the pins have kind of ghost it out and our current component now is the shaft okay so I'll start a new sketch and I'll do this front plane now in the last example I used a 3d part and I you know had it intersecting this frame and we kind of you know combined cut it away this method I'm going to show how you can use projected geometry to help you create a sketch so instead of 3d we're going to do it a little bit more 2d this time so I'm going to use the create project command or the P key for the shortcut and when I do that you'll notice I have two options in this selection filter one is entities and one is bodies okay now watch what happens right now it's selected two entities and as I get near geometry you can kind of see how it's gonna project for example the spline it'll project just this edge if I click on bodies notice kind of like the preview you see it's almost doing like a silhouette trace so it's not projecting like these little splines right here it's basically projecting the whole outside of it so this allows you to basically get different results using these selection filters okay well I want to project this cylinder right here and so I'm going to rotate a little bit more isometric so you can kind of see what's going on but notice what happens when I kind of hover over that circular cylinder you can kind of see this line right here so if I click it basically project let me turn off the frame it projected those two lines of that cylinder so hopefully you can kind of see what it did there you'll notice it didn't project the horizontal lines or anything like that and that's because I basically hooked it on the cylinder and it's basically projecting the edges of it which are the ends okay so I'll do the same thing over on this side which it's a smaller cylinder in fact notice if I hover over this face it's wanting to project all the way from the top to the bottom if I hover over this cylinder it's only projecting the edge of that cylinder right there and I'll say okay also so we basically grabbed information from the 3d geometry to help us with our sketch okay so now I'm gonna come in and basically draw the profile of this to create my design so I can see you know five eighths three quarters seven eighths etc so I'm going to use those dimensions again so let's go ahead and maybe draw a center line so I just have to get near this edge right here you can kind of see how it does catch us to the center and then same thing here it kind of catches to the center right there now this is an object line and what I'm basically doing is I want to create some light pencil lines and kind of trace over everything so I'm gonna select that line and change it to a construction line and when I do that you'll notice it turns dashed it is no longer an object line it's kind of like a light pencil line okay okay next thing I might do is using some of the dimensions that I have I know that it's going to go through this edge here and it's going to go through this edge here but I don't know where this middle part is so I'm going to use the offset command this is a pretty powerful command I'll click on that line and you can see that we can offset this a certain distance well I know that the diameter that I need it to be is the diameter is 3/4 so if I go like that you'll see it's gonna do 3/4 but I need half of that and I show this in the last example I can't just type in / - well I guess I could catch me surprised I didn't think I could do that so that's interesting let me show you how you should do it I'm going to put this 3/4 in parenthesis so we're basically you know doing mathematical orders right here so we're putting 3/4 in the parenthesis and we're dividing that by 2 okay so that's how you typically would have to do it and I'll say ok and you can see that it took that line and it offset it half of 3/4 okay so now I actually have enough geometry that I could start drawing so I could start here come over to there I'll connect those two dots there I'll connect those two dots there and I'll come over to here for example and then the last thing I need to do is we're gonna revolve this around so I need to come down to this center point and let's go all the way across you'll notice as soon as I do that it kind of shades in and shows me my profile and that's this option right here so profile if you don't like it you can turn that off I personally like it because it shows me but that's a valid closed profile okay I'm gonna go ahead and finish my sketch and I have enough information here to start creating this part so I'm going to grab my profile and for those of you that haven't seen this in previous live streams that I've done you'll notice that if I can't I can select this profile but this profile is buried by this other part I could turn off the frame but a neat trick is to click and hold for about a second and it allows you to probe through until I get to that profile so I'll select that and then the same thing here click and hold grab the profile I love that tip I use it all the time okay we're gonna create a revolution or revolve there is my profiles three of them are selected what's my axis we're gonna go around the center axis and there's my 3d model and again it fits perfectly because we're using information from the 3d model but this time we projected it onto our sketch instead of doing you know like machining type stuff like cuts and stuff like that okay now for the really observant of those of you attending I purposely made a mistake and we're gonna run into that mistake here in a little bit and I'll show you how we can get around fixing it so well I don't haven't checked the chat but there you'll see an issue come up here just a second okay so I'm gonna start working on the the holes back here and you can actually see I'm kind of zoom up on this area there's a drill that goes all the way through and you can see it has a drill point at the end and then there's a drill that goes to the top I'm gonna show you some really neat tips and tricks using the hole command and then finally we can see that there's this BSP pipe thread in there also we're gonna deal with okay so I personally like using the hole command instead of creating another sketch typing in dimensions do extrude having to taper the ends I'm gonna use the whole command now it's asking for a face I purposely click I kind of over exaggerate I click away and out of where it needs to be obviously it's off-center okay and you'll see why here in just a second you can see the different hole types simple counterbore countersink so I'm going to do simple what's the hole tap type simple clearance tapped or tapered well I'm going to say simple in this example because we're just doing a drill we're not tapping it and then you can see drill point is it flat or is it angle so I'm going to do angle and if I kind of rotate you can sort of kind of hard to see you'll see how it's doing that angled drill point at the bottom ok so here's my tip that I want to share with you see this blue little dot I'm gonna grab it and move it around and you can see I can reposition this hole and you'll see that other little blue dot which I can't really point to but it's right above where I'm at right now all I have to do is get near that and you'll see it snap right to the center of the shaft I didn't have to do any offsets or measuring or anything it's it's gonna automatically snap to the in to the center of that part okay so now what I want to do is start filling in this information so we know that this drill is a 5/16 according to the dimension drawing oops that's the diameter so I guess I think I said length but yes the diameter is 5/16 so I just type that in and I don't know if you saw the circle get a little bit smaller let me do this like so I'll come in here and say 5/16 and you'll see that it gets smaller then I want to specify the depth and in this case it's 1 in 3/4 so I could type in 1 and 3/4 I could type in 1.75 five doesn't really matter and I get a nice live preview what that's gonna look like and I'll say okay we've just created a drill that goes all the way into the park at a very specific distance so if I turn on my section analysis we can see what that looks like okay so the next thing I want to do is I want to put this whole this 21 64th down through the top of it also okay now here's another neat tip I'm gonna use the whole command again and I'm gonna click near the top so I'm just going to click somewhere like that and fusion will automatically put it right at the top tangency of that and let me show you what I mean by that okay if I say hole and I click kind of over here you'll see how it put it going that direction if I click near the top it's gonna put it at the top so again didn't have to do any measuring or anything like that now this time I do want this hole to be a very specific distance from the end of the part so I can just click on this face right here and you'll see that it added in a reference right there and I could type in that is supposed to be 1.5 and you'll see the hole move over so we're referencing the edge of this shaft according to the drawing now I think it remembers the last dimension you typed in but just to make sure I'm going to come in here and say 5/16 and I say okay I think my actually my drawing yep I lied I need my drawing I'm using this old I changed it the 2160 fourths so that's what it should be I'm gonna leave it 5/16 but you guys are going to do sixty fourths so okay now what's neat about this is if i zoom up we can actually physically see that those holes are perfectly intersected with each other and if we do our section analysis I can see that in our section analysis it looks just like our drawing it's perfect okay we turn off the analysis so again according to the drawing we have this BSP pipe thread and it's only a quarter inch deep and that's what this little symbol right here means 0.25 deep so if you're following the drawing and you don't know what that means that's that's what it means okay so another little tip here um I I can't really modify this existing hole through here because the BSP pipe is going to be a different size than this drill hole through so I need to create another hole again I over exaggerate and put it off to the side I'll go ahead and drop it into place and you'll see I probably get an error message or a warning or something potentially okay I did yeah there we go no target body found to cut or intersect why it's because it's the exact same size so what I'm going to do now is make this a little bit larger like so and I'm going to start going through I want to do a simple yes but I want this to be a tapped hole so I'm gonna say tapped let me move this up a little bit and according to the drawing and it's a BSP pipe thread so I'm going to come down here and go to BSP pipe and you can see that that kind of changed a little bit and then it says size is 1/16 but according to the drawing it's 1/8 and you can see how that got a little bit larger and it's also a flat so I'm going to change it to flat bottom and I know that the depth according to the drawing is only supposed to be a quarter inch deep so after I do all that you can see it gives me a nice preview of what that's gonna look like it automatically threads those holes for me or that hole I should say it's a little bit bigger than the drill through that we did earlier I'll say okay and we now have the end of the shaft drilled through or I'm sorry tapped the correct distance so again to do that I kind of made the hole a little bit bigger that way it wasn't modifying the existing one and then I came in and specified all the settings okay so the next thing I'm going to do with the shaft is we're gonna put in this wood roof key slot now I do know that there's Woodruff key tables out there and all that kind of stuff I simplified things by actually putting dimensions on there instead of saying it's like a 206 Woodruff key I just went ahead and put dimensions on here for you and so we can kind of see it's 7/16 from an edge looks like it's an eighth of an inch up above this edge so let's go ahead and do that I'll create a sketch and I'm gonna show you a cool little trick here okay you notice that all of my parts are visible and sometimes that's nice but sometimes it gets in the way well right now I'm only working on the shaft so I'm gonna right-click on the shaft and say isolate and what this is basically gonna do is isolate it it's gonna turn off all of my other parts and only so the shaft and I do this quite often also because you know I've already got the information from the 3d model that I want so I don't really need to see those other 3d models so it kind of simplifies my view okay so now I'll say create a sketch we'll do it on this front face I'll create my circle and again I'm just gonna throw it out here in space I've mentioned this in previous live streams I typically over exaggerate things like to be farther away than they're supposed to be and then when I put in my constraints or my dimensions I can see it move into place that it just it's a confirmation to me that everything worked correctly so when you hear me say over exaggerate that's kind of what I mean okay so in this case it's three quarters of an inch in diameter and I could probably move that you know kind of closer to where it needs to be something like that then I might come in and throw my dimension on here well I know that it needs to be a quarter of an inch up so I'm gonna go like that oops click and that is supposed to be point one two five okay and then I know it's supposed to be a certain distance over and that's supposed to be 7/16 okay however I'm starting to potentially see an issue here and this is the mistake I was telling you about if I look at my drawing we can see that the Woodruff key is kind of close to the shoulder and there's a lot of extra material over here but when I look at my 3d model it doesn't look like that extra material is existing so that is why I mentioned before usually after you know I've used 3d geometry I might come in and verify my dimensions so we can see that the total length is five and a quarter so we're gonna check that here in just a bit let's go ahead and finish this Woodruff key so I'll go ahead and select it say extrude so I've created the right thing and I've created it in the correct position now what I'm going to do is I'm going to start creating the the actual key way itself I want it to be centered or symmetrical so I'll come in here and change my direction to be symmetric and now you can see we can specify the width of this key way and when I do symmetric you'll notice I get this measurement half length and whole length I'm gonna click on whole length and what that's basically doing is it's saying the distance from one side of the key to the other side of the key needs to be in this case it's a eighth of an inch so point one two five and kind of see how that updated so we're going to point one two five from one side to the other the whole distance and I'll say okay and there we go I got my Woodruff key however let me go ahead let me show you another tip here comes another free tip for all of you I want to turn all of my parts back on okay now I could come in and click on these individual little light bulbs but that would take quite some time especially with a complex assembly well if I right-click on shaft you'll notice it says show all components but when I do that nothing happens and here's the trick with this basically what you're saying is at this level show all the components well there's nothing underneath it there's no other sub assemblies or whatever however if I come up to the top level and say show all components you'll notice it turns them all on okay so this show all components is actually at the level that you're at so it's a great way of turning on or off sub assemblies or sub sub assemblies etc so make sure if you want to turn everything on you go to your top level and say show all components neat little tip there okay so now I can see what this looks like according to the drawing this is supposed to be five and a quarter so I could come in here and do a quick measure from that face to that face and it says it's 4 and 3/4 so again we're off but simple fix I'll just come in here press poll or extrude doesn't matter I like to start to drag to kind of get a visual over-exaggeration will say reinker to this back face here and it's supposed to be five point two five five point two five we can see that that updates and now the keyway kind of makes more sense it's it's in here where it's supposed to be if we look at our belt tightener the finished assembly you'll see that there's a nut on the end and that's sure enough that's why the shaft has to extend out past this end part there so we were able to easily fix that or let's undo I could go all the way back to my sketch and add in I could do a rectangle I could do a line it doesn't really matter I could do something like that throw a dimension on here from that edge to that edge it's supposed to be five point two five you can see how that rectangle updated accordingly but watch what happens when I say finished sketch it didn't do anything well that's because in the revolve we only had three of these profiles selected but I could come in here and add as a 4th and say okay so two different ways that we solve that problem in reality I would probably recommend updating the sketch that's kind of your driving master you know of this part offset phases are really cool but you kind of have to know oh i offset that face a certain distance and it's different than my sketch so i would recommend and editing the sketch and that's why i show both of those methods okay so the next thing is to add a thread to this here's another free tip for all of you I will go ahead and say thread what's the face I'll go ahead and click on this face and you'll notice that it's threading the whole thing well right here you'll notice by default it's set to full length so I'm gonna turn that guy off and now I can specify the length of the thread well I know according to the drawing it's half inch by clicking on that face Fusion was smart enough to say oh it's probably you want it to be a 5/8 by 11 so you can kind of see I could do five eighths by twelve I mean fine threads etc but sure enough according to the drawing it's a 5/8 by eleven thread I'll say okay and there we go now you'll notice that these threads are just like a decal almost like a sticker I could come in here edit that feature and say modeled and it'll physically model those threads for me but I would recommend not doing this unless absolutely necessary for example maybe your 3d printing it or something like that I would just leave it as a representation that way it kind of speeds up everything with all those extra edges and faces it can start to slow down your machine it's trying to calculate shadows and occlusion and all kind of stuff so I usually leave them as decals like you see there okay last thing here is I'll go ahead and chamfer that edge and in this case it's a sixteenth of an inch so I'll say 1/16 say okay and we are good to go that's our next part designed exactly where it needs to be okay this next part I'm gonna do is the bushing and then we're gonna stop there we've got about 15 minutes left and in in part three we're gonna do this pulley and then just the rest of the really simple parts like a washer and a nut etc and I'll show you how I went about creating the exploded view we can do rendering etc now this pulley is a little bit more difficult so I'm gonna show some neat tips and tricks with that in our next session but let's go ahead and do this bushing now looks pretty simple and I'm gonna show you a cool another neat little tip with this so we can see that sure enough it's 2 and 1/2 in length so let's jump in here I'm going to create a new component and we'll call it bushing let me get my drawing up here for me yep called bushing okay so I'm gonna create this one a little bit different again to show you a couple different ways I'm just gonna say create a sketch but instead of doing a revolve in the front plane I'm gonna sketch on this side plane okay well I know that I probably want to know the diameter of the shaft so let's go ahead and project the shaft and you'll notice as I get near geometry how it's trying to project all of that onto this plane it's slicing right through the middle so I'm gonna go ahead and click on that and say ok and now I have a circle there I'll create another circle using the center of that circle again I think it's so cool that everything is projected off of this geometry and this is gonna be one in 1/16 in diameter and I'm done actually that's all I need to do actually you know what let's let's speed things up here I could come in here and draw there's a groove it's kind of hard to see right here that goes all the way through the length of this bushing and I think it's because it allows oil or whatever to go the full length of that bushing so let's go ahead and draw that while we're in here so I'll say rectangle Center rectangle I use this one a lot I really like it I'll click on that projection point right there now I know that the width of this is supposed to be point 1 to 5 oops 1 to 5 and the height of it is 1/64 of an inch and it's gonna be hard to show but it's basically from that point up is 1/64 of an inch but you'll notice the height here is showing the full height so again I could type in one 64th divided by 2 and you can kind of see what that's doing ok or I could let me just do like just do one 30 seconds of an inch I think that's what actually it's supposed to be my drawing is wrong I apologize I was like that looks a little small so this is supposed to be 1/32 am i bad so you can see I wrote it down wrong on my drawing one 30 seconds overall height would be one sixty-fourth total height so let's go ahead and do that the joys of live streams okay so I now have that shape I'll say finish sketch click on this profile and I'm actually gonna back up really quick cuz I'm going to show you another tip that I hopefully you all know about I'm in my sketch I've I've just completed adding my dimensions etc and you'll notice I'm still in my sketch environment but I can click this profile right mouse click and say extrude or say presspull watch what happens when I do this I'm gonna say extrude it automatically kicks me out of my sketch puts me into my screwed command so instead of having a hit finish sketch and then go into extrude I can I can actually activate the command while I'm in my sketch okay pretty self that self-explanatory um similar to what we've done before I'm gonna come in here and say symmetric the whole length and the whole length of this is supposed to be 2.5 you can see how it's taking that profile and extruding it the whole length of 2.5 and I'll say okay now once again there's a lot of geometry in the way so I'm gonna right click on my bushing and say isolate we've turned off all of that other geometry and now I can see what this bushing looks like now there's a groove in here and there's many different ways you could create this some of you might draw a rectangle on the front face dimension it may be revolved cut that away maybe you could have drawn this complex profile originally and revolved it around absolutely that would work I'm going to show you an interesting tip here again not saying this is exactly how you should do it it's just a method of how you could do it I'm actually gonna draw that groove on this face I'm gonna say create a sketch and I'm gonna keep it simple I'm gonna draw a circle now we know that the diameter of this is supposed to be thirteen sixteenths and when I draw that circle you can see sure enough there it is but it's on this end face now here's here's the magic check this out I'm going to select those two profiles I'll say extrude and if I start extruding it's gonna extrude from the end of this part but right here under start you'll see it says start at the profile plane and that's exactly what it's doing well I could come in here and say let's offset that plane how far do we want to offset it 7/16 now you'll notice it went the wrong direction so I'm going to type in minus 7/16 and what it's actually doing now it's kind of hard to see but it took my profile it's offsetting at 7/16 and then doing the extrude cut and in this case 5/16 would kind of seal update of that and there we go let me let's do the analysis really quick so you can see what happened so basically I drew my profile on this end face then I did the extrude command and said Starck seven sixteenths of an inch in and then do the cut so again it kind of simplifies instead of creating like a complex sketch and doing leave all those and all kind of stuff I kept it simple using just a circle and then using this offset plane option so hopefully you found that kind of useful maybe down the road you'll be able to use that okay I want to show everything so I'm going to right click at the top and say show all components everything is kind of ghosted out well if I activate like top level component we can now see everything and we've actually done quite a bit today we've gotten the two pins done we've got the shaft done we got the the bushing done I like to turn on my analysis really quick just to kind of verify everything I'll look at the front and we can see that these pins look really good they sit right up against that the frame if we kind of move up here we can see that the shaft fits perfectly in these holes the Woodruff key is in there or that I should say the Woodruff key slot is in there and we can see the bushing and you can actually see how this is all gonna work where if they screwed in some kind of a grease gun in here and was able to inject some grease it would actually go into this groove right here which actually then goes into this groove that goes all the way across now I showed how to do the analysis last time but if you don't remember how I did that let me go ahead and delete it and show you the quick and easy way of creating a section analysis so under the inspect menu section analysis okay and allows you to pick on a face or even a plane now I know that this plane slices exactly centered through my whole assembly so I'm going to click on that plane and there you go you can kind of see how it's sectioning through I could change the distance if I wanted to and kind of almost like an MRI or a cat scan or whatever so you can kind of slice through it you can change the angle of it so we could rotate this to be like 90 degrees and we can look at it up and down kind of slice through it this direction see what that looks like and you can even have multiple sections so for example I'll come in here and say section analysis I'll do that face again say okay and you'll notice I now have two of them and I could toggle between multiple ones so and then if I don't want to see it anymore I just hit the little light bulb next to analysis and it's a toggle on or off okay with that hopefully you absorb some of these tips and tricks that I've shared on today's live stream the part three of this we're gonna finish this guy up we're gonna put in the the nut and the washers and the Woodruff key then I'll show you how I created that drawing how I created that exploded view before we end I want to add a plug it's about a month away a little bit less than a month for our Fusion Academy in Portland I'm hoping erin has posted some stuff out in the chat about that if you can attend I highly highly recommend it marketing just shared a really cool video about what is fusion Academy hopefully Aaron linked that video you can go watch it the little little cameo of me in there that I think is pretty pretty fun so if you could make it I highly highly recommend it basically pretty much all of us from Autodesk on the fusion team will be there answering questions meeting people doing classes etc if you have ideas for future live streams please make sure you put them in the comments so we can kind of see what those are and add those to our list we are because of the summer time everybody is on vacation and travel and stuff we are going to start doing these about once a week instead of twice a week so definitely make sure that you subscribe hit the little bell icon and that will I think subscribe you to our channel and alert you when these upcoming live streams are happening and if you haven't already make sure you've signed up for the fusion 360 Facebook group there's a lot of really cool people out there that are sharing what they're designing in Fusion we post stuff out there about upcoming live streams etc so with that I hope you have a wonderful rest of your day and we'll see you on a future livestream thank you you

Channel: Autodesk Fusion 360

Views: 6,580

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: 0--Gm7QS_c4

Length: 61min 7sec (3667 seconds)

Published: Thu Jul 11 2019