360 LIVE: Laser Projector Build - Part 4 The Front Mount

hello everyone and welcome to another fusion 360 tech Thursday I'm Brad talus from Autodesk and I know a lot of you are probably going hey you said you were going to be gone for like six weeks or so um I'm back I ended up cancelling my sabbatical early because of all the craziness that's going on right now I hope all of you you know you're our family we we love seeing you guys on the chat and all these live streams that we we had Autodesk really hope you are all doing okay we're making a mission to put out as much information as we can about our products like these live streams so please keep an eye out we're gonna be putting a ton of information out there in fact Jason and I are currently working on filling in our calendar I did see a comment yesterday on Tyler's live stream that some of you are confused and when these live streams are happening so what I personally recommend is in youtube do a search for Autodesk fusion 360s Channel and make sure you subscribe to our channel you'll see all of our upcoming live streams right here and you'll notice like for example Jason is going to be doing one on the fundamentals of sketching in some advanced sketching and you can see when they're scheduled at what time etc we're even going to try some different timeslots we're gonna be bringing alone some Morecambe the live stream is coming up here pretty soon so definitely keep an eye out and maybe add these to your personal calendar I know it says set reminder but I even experienced yesterday I signed up for Tyler's live stream and it didn't alert me unfortunately so I personally recommend adding them into your calendar mam and come back and check this page every every day or so because we're gonna be adding a lot more information in there I do have my friend Jason on chat today to help us out so if you have any questions or comments definitely put them in there and also if you have any ideas for topics that you would like our team to focus on on upcoming live streams throw them in the chat also and we'll see what we can do to accommodate those so I'm gonna continue my live stream on this little laser projector thing the part we're going to be working on today is this front component so not too complicated but I gotta talk a lot more about like draft this time now again I'm not showing you exactly how to design this thing from scratch I've seen a lot of comments like well can you 3d print it and what about draft angles and parting lines and all kind of stuff my main focus is to teach you more about you know tips and methodologies using fusion 360 so today I am gonna focus a little bit more on draft and we're gonna add draft to this part where as on maybe some of the other parts I've done I didn't worry too much about draft you absolutely could draft in there but I was focusing more on like maybe sketching or replace face or something so let's dive in I'm gonna switch my screen to fusion another thing is I'm also creating these parts individually and I typically don't do that I usually design in context where I use existing models to help me with my design but in this example I'm actually going to be using you know drawings to you know to create these parts okay you notice that's giving me a warning because I deleted deleted the part that the drawing is referencing but that's okay and again just like I mentioned before about I'm not showing you exactly how to do everything these drawings are not you know perfect drawings they're they have enough dimensions on here to allow us to get through how to create this part so I've included this drawing I've also included the outline that I usually put together in the description of the video so make sure you grab those okay let's dive right in so we're gonna be creating this this component right here and you'll notice I use the term component that's one of the first steps I'm going to do but you can cat again break it down into some simple forms and this first one is what I'm gonna call the cup it's basically this this ring right here we're gonna create this profile on the inside that you see and then we're gonna do these posts and it might be kind of hard to see but they have some drafted ribs on them that we're gonna also create so that's what we're gonna be doing in today's projects so let me jump back to fusion so the very first thing I like to do is to create a new component now there's different ways you can do this to get the same result so you'll notice under the assemble menu new component under the create menu new component exact same thing or I can even right-click at my top level over here in my browser and say new component and it'll go ahead and create a component and I kind of like this method because it doesn't ask me for a name or anything like that I could just leave it component one or I could double click on it and give it a name so let's go ahead and let's just call this front mount or something like that now the reason I like to use components is everything is going to be captured underneath it like my sketches bodies etc so I'm going to start with a sketch and in this example I'm gonna use the right plane so I'm gonna go ahead and click on this right plane hopefully you've noticed we pushed a release out I think it was last weekend or so some really cool new functionality with 3d sketching I have seen in the forums a lot of people are asking why they see like for example when you turn on 3d sketch why they see like a triad let me let's do this we look like and try it again there but why they see this new little triad thing if you're sketching and you see this thing the reason is because of this 3d sketch so go ahead and turn that off however if you don't know what 3d sketch is I highly recommend you watch Tyler's livestream like he did yesterday all on 3d sketching he made this really cool bumper frame on an ATV that is on ER fusion 360 live channel make sure you watch that it was really cool and really well done so okay so if I wanted to point out how because I've seen that a lot in the forum so turn 3d sketch off if you see that triad okay I'm gonna just start by creating the the main shape which is you know a circle that's according to the drawing three point six five in diameter okay now I've shown this trick before am I gonna highlight it again because I'm gonna show you some issues with it here just a little bit I could hit finish sketch or I can just click on my profile right mouse click and you'll see some commands that make sense you'll see two different kinds of extrudes and offset plane you'll always want to do the first extrude and I get asked what's the difference well the first extrude is a solid extrude the second one is what we would call a surface like a thin-walled face so it basically would create almost like a ribbon in a circle well we obviously want this to be a solid so I'm going to use this first extrude I'll drag that up just to kind of get a little bit of a preview and again according to the drawing I want to extrude that one and a quarter in this case and again I'm not gonna go to the drawing too much but you can see right there there's the one and a quarter okay there's a really small Phillip point zero five on the bottom of the part so I'm going to go ahead and press select that edge right mouse click and it shows me the commands that make sense so let's just do a point zero five radius fill it okay so this is kind of a beginning of the cup now we want to hollow this out and my one of my favorite commands as I pre select a face and I'm gonna use shell okay what this allows me to do is to define a wall thickness and in this case I'm going to type in point zero eight is the thickness and there we go okay now I could have drawn a side profile right I mean I could have drawn an L shape and added to fill it as a profile and then revolved it around using the revolve command that would have totally created the same part but I kind of like doing it like this because I can always come back and easily change the shell thickness if I need to I could obviously do that with a sketch also but I like to keep my sketches simple you've heard me say this multiple times and let fusion do the hard work for me so I created a very simple sketch and we use the shell command okay the next thing I want to create and they're they're kind of hard to see but there's these little standoffs inside the model right here here's that kind of like a detailed view of what these are okay so and they are point let me see there's a view here here we go a section view there's these little standoffs because we're gonna create this counterbored hole that goes through here that the kind of screws go through to assemble the whole thing together and we can see that these are 0.15 off of the bottom of the part so a neat tool here is this offset plane so I'm gonna go ahead and click on offset plane I'm gonna select this inside face because that's where the dimension is coming from and so it basically creates a plane on that face but I can now offset it a certain distance from that face and then create a sketch on it so in this case we want it to be 0.15 and if I kind of look at it from the side here you can kind of see that sure enough that plane is above that inside face point one five and this is going to allow me to create a sketch on that plane and I'm just going to draw one of those circles now it's a point two five diameter circle and you'll notice again and I've mentioned this in previous live streams I purposely draw off-center and not where it's supposed to be then I force it using either constraints or dimensions where I want it to go so for example I want this to be vertical with my center point so I used the horizontal vertical constraint and I clicked on it and you can see how it forced it to go to be in line with my center point then I'm going to grab these two points here to specify a dimension and it's supposed to be one point six seven four up and you'll notice that the circle turned black which means it's been fully constrained it can't move left or right and it can't move up or down because the dimension constrains it up and down and the constraint constrains it from going left to right okay again keeping my profile very simple here now what I want to do is we're gonna actually use this sketch multiple times so I usually expand open my component and here again you can see how everything is organized its own origin its own body its own sketch any construction planes that were used I'll expand open my sketches we'll get back to that here in a minute and then I can click on my profile so I'm going to select it and say extrude now watch what happens when I start to drag down you can see that it's turning red that's because the circle interferes with the body well I want to turn this into a solid so I'm gonna say instead of cutting the material I want to join the material and I want it to go to this inside face I'm just gonna get click on that face you can kind of see how it's gonna snap down so as I'm I start to drag to kind of see what it looks like but then when I click you can see how it snaps down and I don't have to type in a distance again anytime I type something in I might accidentally type in one point five or point one four or whatever and make a mistake so I'm telling fusion to snap to that inside face and I'm gonna go ahead and say okay and we now have this little feature okay I'm going to turn my sketch to back on and I'm gonna select that profile again right click and say extrude but this time I'm gonna start to drag it up and in this case I do want to you know basically cut this little scallop or this little pocket into here and I want it to go all the way to the top so I just click on this top face okay you can kind of see what it's doing I'll say okay and we use the same profile to create the plastic part down here and we use the same profile to basically allow room for a screw head or something like that to come down into here or a screw driver or whatever it might be and that was just by turning that sketch back on I can turn it back off to kind of simplify my my screen here okay okay so the next thing we want to do is we created one of these but I need multiple ones and I want to I could pattern this around but I also showed in the drawing that there is this counterbored hole in fact if I scroll out here if you guys are using the drawing and you might see some terminology you're not familiar with so you'll see I have a point one diameter hole right here and then this means the counterbore so we're gonna do a point to one diameter counterbore that's point one three deep that's what that symbol means and there's six of them around okay so that's what that terminology means right there so I'm going to show you a really cool trick here I'm gonna use the hole command so I'm gonna come in here and say hole or I could use H as a shortcut and then I'm just gonna click somewhere random on the screen and you can kind of see it it puts a preview what this is gonna look like okay but I can't see where this needs to go and if I start to drag I don't have anything to snap it to which you know you see me before I can snap it to the center really easily if there's that existing little dot I can snap it to it but you'll notice there isn't one over here well if I click on this reference and then I'm gonna rotate and click on this arced edge right here you'll see that it moved over okay and even though this edge is you know up above the bottom of the park it is now perfectly centered with that existing little plastic standoff okay so that's a cool little trick using that reference okay the next thing I want to do is I want to do a counterbored hole so I'm gonna go ahead and this is a simple hole where you can see it's basically like a drill straight through I'll go ahead and click on this one and you can see how the image updates and gives me a little bit more information I like to type in my well I got a weird air that are here to hopefully we're still sharing okay you can see the the diameter right here so I'm going to go ahead and highlight the diameter and this is supposed to be point one according to the drawing then the counter bore diameter I'm going to again according to the drawing is supposed to be point two one and the depth of which you can see I've already done this is point one three okay so you might have to change these numbers yours might be different okay and then for the height what I typically do and you'll see there's a an arrow right here I'm gonna just start to drag that down and then I can reference a face so I'm just gonna click on that face and you'll see it changed it from like two and a half inches or whatever it was it's now drilling through to that face right there let's kind of zoom up on this a little bit and you'll see sure enough we now have a counterbored hole it's the hole itself is point one in diameter and then we specified the diameter of the counterbore and the diameter or the depth of the counterbore so i'm gonna go ahead and say okay and that was you know it took a couple you know a minute or two for me to explain that but the whole command is extremely powerful because it creates it as a feature in the timeline and I can always come back and edit or change that I didn't have to create a sketch and do a revolve or anything like that okay cool so I pretty much finished what I want this standoff to look like so I'm going to pattern it around so we'll say create pattern circular pattern okay now by default this usually comes up as faces and I would have to come in and manually click all of these faces including all the counterbore and all that kind of stuff okay which would take some time and could potentially result in an error so instead change my pattern type from faces to features okay what this allows me to do is to actually select features in the timeline and so we can see here kind of going back in time so here's the whole here was the the extrude cut here was the extrude join so I'm actually gonna select all three of these features in the timeline and you'll notice that it's selected all of the faces for me automatically so much faster and much more precise okay so it found three features my axis I'll just click on a circular edge or a circular face and quantity I can either type in or hit this little up or down arrow so I'm gonna say six I'll say okay and I now have those standoffs inside and on the outside you can kind of see the counterbore is going all the way around it's a really quick way of saving time by using the pattern and again I could have done this in my original sketch you know I could have patterned a circle all the way around but I would have had it done multiple extrudes etc etc so again I love I love the keeping my sketches simple and letting fusion do the work for me okay the the next thing I want to do is we're gonna create this little cutout you see inside the part and again actually it might turn it right-side up pretty simple I can see a circle and a couple rectangles with fileted edges so I'm gonna keep my sketch simple now what I'm gonna do is you know I could create another sketch on this face but I have my original sketch that we first started out with way back here in times and I can actually edit that but watch what happens when I edit it we're way back at the very beginning so you don't see any 3d model or anything like that but in this case that's okay okay so I'm gonna start out by creating another circle again according to the drawing it's 1.97 I'm gonna create a rectangle and I like to use this Center rectangle so I'm going to click on that little icon there click my Center and you'll notice that the rectangle is being created from the center okay so this is supposed to be point eight seven five by two point five again according to the drawing here okay so I created that rectangle now I want to create another rectangle that's perfectly centered up here so I'm gonna say rectangle Center now I'm gonna show you a neat little trick here if I hover near this edge you'll notice that it's kind of snapping to that edge so wants to create this Center rectangle coincident with that edge now if I get right here you'll notice it doesn't seem to be snapping vertically right so what I'm gonna do is I'm just gonna click somewhere if I think I'm over-exaggerating that's like way over here and create my rectangle okay so in this case it's point three tall point three by point 4 2 wide ok now if I were to grab this point you'll notice that it wants to stay on that circle because it created that coincident constraint for me automatically you can see them right there but of course I want this to be perfectly centered and vertical from here so I'm going to say horizontal vertical and what that point and that point and notice what it does it keeps it on the existing circle but it made that center point be perfectly lined up vertically constrained with the center of the circle so again just a little tip that I use I draw it off-center and I watch it get moved into place and again we can see that it's perfectly constrained because it's it's turned black instead of the blue okay so here's the thing I was going to show you I earlier I showed you I could pre select my profile so I'm going to go ahead and select these profiles okay to extrude I didn't say finish sketch but when I right mouse click and say extrude we don't see anything and it's extruding this instead of cutting it now why is this and I'm pointing this out because I've seen in the forums sometimes people say I'm getting a weird result or whatever so check this out the reason why is because we edited the very first thing we ever did which was create a sketch the extrude for the cup hasn't happened yet or the shell etc so my little shortcut I just showed you doesn't really help me in this particular situation however if I say finish sketch now we're at the end of our timeline because you know we went back here and edit it in time but then it went and finished everything including the pattern in the shell and everything like that but I now need to turn on sketch one and there it is you can kind of see it's underneath my model okay so sometimes that pre-select and not having to say finish sketch is really handy but in some situations it won't work like in this case okay so I'm going to select my profile I'll say extrude I'll start to drag okay how far well I could say in this case I could say through all but I'm just going to go ahead and select that face right there and it's going to snap to that face and you can see it took that profile and cut through the body I'll go ahead and turn off my sketch again I I don't need to see him all the time and then let's just take a look at the drawing really quick you'll notice I have radius of point one two five ten places you can kind of see it all the way around you'll notice that there's like a rectangle in here also I turn on my sketch so I could kind of show like how to dimension and a lot kind of stuff there so you can kind of see that and then we've got two of them that are point zero two okay so what I'm going to do is select one of these edges and say fill it point one two five we can kind of see what that looks like and then I'm just going to ctrl select working my way around and you'll notice even if the edge is hidden I can still click on it and pan over just a little bit sometimes that gets in the way now for example this edge I can't really get because it's kind of around the corner so I'm just gonna continue working my way around grabbing all the edges that I can see and then I might rotate to a slightly different orientation something like this and then I can continue my selection so you can see I can grab that edge let me zoom up a little bit grab this ASPs that edge and that edge there and so you'll see that I was able to grab all those edges with basically just one move in between now all of these these ten edges are 0.125 I could say okay and then create another Filat for these little guys up here but I like this functionality since this is like all one basic profile I'm going to come in here and hit this add new selection and what that's going to allow me to do is come in and say I want that edge there to be point zero two and you can see how these are large but that one's small in fact I can come in and grab that edge there you'll see there's two edges that are point zero two and when I say okay I'm only gonna have one Phillip feature in my timeline okay you can see it right there but if I were to come back and need to change that I could edit this and I can see all of the sizes that kind of have to do with this one you know cut through feature so kind of a neat little tip right there is you can add multiple selections if need be okay looks like we're doing okay so the next thing I want to do is add some draft okay again I'm kind of breaking this part into like these sub components so we're working with this Cup and then I'm going to come in and do these little standoffs but because you guys were asking about well how would you manufacture this part you'd have to have draft for it to be able to come out you know of an injection mold or something like that I'm going to talk about the draft command now when you do an extrude I'm gonna go all the way back here when you do an extrude you'll notice that there's this taper angle so I'm gonna say like two degrees when I got let me go five degrees so you can kind of see it better you'll notice that when it's extruding it's actually adding five degrees of draft or taper to this I personally don't like using this because if I needed to change my draft from one millimeter to two millimeters or something like that or I'm sorry one degree to two degrees you know I I don't want to be able to have to hunt where that was okay so I like to use the draft command okay what this allows you to do is to specify a draft plane specify which faces you want drafted and then specify the the degrees of draft now the first thing it's asking for is a plane so I'm going to go ahead and I'm gonna click on this top face you'll notice that it says plane is selected now it's asking which face I'm gonna use just go I'm gonna select one face for now a lot of people get confused what's a draft plane and the best way I can explain it is basically it's the the surface that you would attach a hinge to to rotate the face so for example if I grab this little guy here and start to rotate you're gonna see that it's going to hinge on this line right here okay so this is my draft plane and you'll notice I added like in this case let's just say five degrees of draft so it's it's drafting down like so okay if I were to say my draft plane was down here and this might work might not work yeah there we go you can kind of see it it's gonna hinge around this edge down here okay because this is my draft plane so the best way to think of it is your draft plane is where you want to hinge the faces around okay and in this case we're gonna do a pretty small draft I think in fact let me see my angle I think is just 0.5 for the for the draft angle it's a little bit hard to see but if I hold down my control key you kind of see it toggle from flat so kind of watch in this area right here and then you can kind of see it extend a little bit okay so anything coming here and add in more faces so let me clear that I'm gonna say this face this face this face and you'll see how it's gonna draft those faces okay so I'm just gonna walk around real quick grab these vertical faces in here and it's gonna add half a degree of draft to that okay which might be enough for for a part this size I'm not the injection molder or anything like that okay now what about these vertical faces right here let me kind of move back where our cursor is okay I want to draft this face here also now watch what happens when I select that face you'll see that it looks like it gets a little bit bigger okay now why is that well it's hinging around this plane way up here okay so be aware of that so in this case I might want to make my draft plane actually be on this face I'm hovering over right now instead of this face up here and then it would hinge right here and draft half a degree so just be aware of the different result okay in fact I'm going to do that actually in the outline I didn't do that I just selected it's not gonna keep I'm gonna keep doing what I did with the outline so I'm gonna select them like so it's gonna add half a degree a draft it's gonna keep everything the same which is good and one last one right there I'll say okay okay now like I said I'm not showing you exactly how to do this I'm showing you different methods could I have added my draft before I did my pattern could I have added my draft to the little boss and that cut out and then pattern absolutely in fact that's probably a better method than how I did it now that I'm thinking about it it's like I had to select a whole bunch of faces I should have drafted the cup and then drafted the boss etc and then patterned it so again multiple different ways of doing this so fact Jason's probably answering comments like why did he do it that way so okay moving on so I want to basically I've created the cup I've created the cutout I've added some draft the next thing I want to work on is creating these little ribbed standoffs so I'm gonna go ahead and work on that next okay so this time I am gonna create a new sketch because I want the standoffs to be on this like inside face here so I might just select it create a sketch and again this kind of helps me simplify my design instead of always editing one sketch and making it really complicated I now basically have a sketch that just has to deal with these little standoff so I'm gonna go ahead and draw a circle again purposely not drawing it where it's supposed to be I am drawing it the right size though but I'm just gonna go ahead and draw 2.3 circles here I could have drawn one and then maybe other one equal to that it's whatever method you want to do there I do know that they need to be vertical with each other so I'm gonna select one and then select the other one and you'll see how this one moved over now I'm gonna undo hopefully you've all watched my live streams where I've given some tips and tricks on constraints and I get asked a lot it doesn't matter which order you click and the answer is yes kind of and it depends and I know that's a funny answer but I've come up with a phrase that helps me remember so I'm gonna do my constraint and my phrase is click to keep so I'm going to click this one because I want to keep this location so click to keep and then I'll click this guy and you'll notice that it moved over to match that one okay so let me undo again I'll do the exact same thing but this time I'm gonna click to keep that one I'll click that one and you'll see how it moved over so that's one of those little methodologies I've come up with click to keep so if it if matters to which one stays put maybe remember that phrase so click to keep that one's gonna line up vertically with it you know in this case it doesn't matter because we're going to dimension it so I'm going to throw a dimension from here to here I want that to be a vertical dimension and it is supposed to be point seven up and let's do a horizontal dimension and I'll kind of pan a little bit so you can kind of see the dimension easier and it supposed to be 1.05 over and you'll notice that is now fully constrained this one is still vertical with it but you'll notice that it's not constrained fully yet and the reason for that is because it can move up or down okay so let's add a dimension here and that is supposed to be one point zero five according to the drawing and now we can see that it is constrained also now I want this on the other side so I need to mirror this but to be able to mirror I have to have a line to mirror or something to mirror with so I'm going to draw a line from the center straight up okay now I don't want this to be an object line so I select it I tell it to be construction and you'll notice that it changed to this dashed line so it's no longer an object line it's not gonna cut through my profiles anything like that but now I have something that when I say mirror what are the objects that circle in that circle what's my mirror line I now have something I can select unfortunately you can't select like dimension extension lines or anything like that and that's why I had to physically create a line so I'm going to go ahead and select it you can see how it mirrors to the other side I'll say okay and just like before I could come in here without even having say finish sketch I can come in here and select these profiles I'll go ahead and grab those guys and say extrude and when I do that you'll notice it finishes my sketch for me automatically I can start to drag those up and the height is supposed to be two point five seven in this case okay and again I could add taper to it but I don't like to that's just a personal preference I'll say okay and we now have this extrusion okay so we're gonna add some draft to these posts and again I kind of like to keep them sort of organized so I I know that this is my extrusion of my post then I'm gonna do my draft so I'll come in here and say draft now I'm gonna show again two different results if my draft plane was up here and this was my face you'll notice that the bottom got bigger okay in fact let me let me say like two degrees or something like that so this face is hinging on this top face right here and so obviously it's getting bigger at the bottom if oh my god I'm gonna set this back to 0.5 if I changed my draft plane to be this face you'll notice that the top gets smaller and again it's because it's hinging the angle on this bottom inside face and in fact that's what we want to do we want to select this inside face as our plane and then I can come in here and say I want these four faces and you'll see the tops get kind of smaller with that half a degree of draft and that's what we want in this case it'll allow to be pulled out of the mold easier okay I'll say okay and there we go okay I'm just looking at my outline here making sure we're on track and doing everything so the next thing I want to do I don't know if we can see it on the camera there's there's some holes inside here and they actually go all the way all the way through so I'm gonna show you some cool tips with using the hole command now again many different ways I could create this part I could have created one of these put the hole through it and then mirrored it multiple times but you'll see here that it's not symmetrical as much as you think that's why I ended up creating four of these and also it's not symmetrical in how the ribs are created if i zoom up on this one you'll see there's like three little ribs here but then there's a larger rib on this guy here so that's why I ended up drawing all four of them and we're basically gonna work on one at a time and then pattern some of the stuff that we've done so I want to create holes that go through these posts excuse me now if I use the hole command it only lets me do one at a time so I click on this face and it's gonna let me do the hole on this face however there's a really cool option in here from sketch for multiple holes okay but it does require a sketch to do this so that's what I'm gonna do let's create a sketch maybe on this top face I'll say create sketch now I want to grab information so I'm going to project so create project I always use the P key for the shortcut and I'm just going to click on these top faces here and you can even see in the preview you can see the draft that's been added to all of this here because you kind of see those double lines and stuff okay so I projected those four faces and then I'm going to use a command that you haven't seen me use very often called point what this is going to allow me to do is I just have to get near the center because we projected that geometry it kind of snaps to the centre and when I click it's gonna create a point at the center of each of these projected circles okay that are sitting on top of these little posts now when I use my whole command I'll come in here and say hole what's my placement I'm gonna say from the sketch and I can click on you can see how it's going to grab that point instead of a face for example so I'm going to click there and here we can see the preview of that hole now we don't want it to be counterbored so I'm gonna come over here and say I want it to be a simple hole and I'm gonna type in the diameter which in this case is 0.125 and I want it to go all the way through now I could drag I could drag this arrow down or whatever but instead of distance I could just say all and you'll see that it kind of does that automatically for me so I don't even have to type in a distance or drag but what's cool about this is now I can click these other points really quickly and I have holes going through all of those now by using a sketch so if you haven't seen that before it's kind of a really quick way of adding a bunch of similar sized holes okay so the next thing it looks like we're doing pretty good on track the next thing I want to do is I'm going to create these these little ribs you see here again using the drawing I can see that there you know where their location is what size they are all that kind of stuff I'm just using my outline here but I want to be able to create these ribs and I'm gonna use the whoops rib command I clicked on the wrong tab here I want to use this rib command you've seen me use the web command quite a bit but I haven't really talked about the rib command this is really cool it allows you to start with a simple profile and it's gonna create a rib for you so for example on this post here if I were to just kind of draw the outline of a rib it will extrude it to the tapered angle to the curbed face everything really easily for me however I need to create a sketch and I want to create that sketch on the surface of this stand off so the easiest way of doing that is to create a plane at an angle and you'll notice the description says creates a construction plane through an edge an axis that's the keyword there or a line now I don't have an edge to select I also don't have a line to select and I also don't have an axis to select so I'm gonna create an axis so check this out I'm gonna go to construct axis through cylinder cone or torus so I'm gonna say through cylinder and I can just click on this cylinder right here and you'll see this blue line up here and this is an axis that's going right down the center of that cylinder okay then I can come in here and say plane at an angle what's the line and now I have something I can select when I click on that you'll see that it's actually going to create a plane that goes through that axis and I can actually set this plane to whatever angle I want so I could say 90 degrees or whatever I'm gonna leave it obviously at zero in this case but I now have a plane that's slicing perfectly through the center of that standoff okay so I'm gonna make this a little bit smaller just by grabbing in the corners what I can do now is create a sketch so I select my my plane there I'll say create a sketch it rotated it for me which I actually kind of like looking at it in 3d anyways so you can see that my my sketch is going right through the center of there you know I want to capture some information so I'm gonna use my p4 project and I've shown this before but I gonna highlight it again and I think it's really important we have two options specified entities or bodies if I were to click on this face here and project it and I turn off my body you'll notice it only projected the edges because there's not really an edge on a cylindrical surface you don't see it project that okay so I'm gonna undo and I'm gonna say project again but this time I'm gonna say bodies I'll say okay I'll turn off the body and you'll notice this time it did it's almost like it cuts through and almost as like a section analysis or a silhouette is probably a better description and you can see that's the result that I got okay so in some cases it's actually better to project the body than it is to project an entity now it does like I said it does a silhouette so it projected the bottom but it did not project this inside face so I'm gonna come back specify an entity and I'm gonna project that inside face let's turn off the body now and now you can see I have something here and I can catch to this inside and so that's the key trick there okay so I'm going to draw a clique profile here so I'm just going to get near this edge you can kind of see how it snaps to that edge I'm going to draw straight out and again using the drawing point one in this case and then I'm gonna do the exact same thing down here I'll zoom up you can see how it's gonna catch to that point and I'm gonna come out 0.15 in this case again according to the drying okay and in the outline I show a cool image of this and then I'm going to connect the dots so I'm just gonna basically come here and connect those two dots right there and then the last thing is I want to specify how far from the top this rib is so I'm going to say dimension from there to there it's supposed to be point two and you'll notice it continued stayin coincident with that edge and it lifted it up and it's black which is good so I'm gonna say finish sketch okay let's do the rib command so I gotta come over here and say rib and it's asking for a curve now watch what happens when I click on this curve I get this little arrow I'm gonna start to drag so you can kind of see what's going on here and we get a really weird result okay well don't freak out right here it says flip directions so I'm going to say flip direction and you can see it's basically are we doing the inside of the curve or the outside of the curve and so obviously by default I did the outside if I flip direction it does the inside the overall thickness is supposed to be point zero four according to the drawing if i zoom up you can see that's matching the curve and the taper so it's a really cool command it's really really powerful so I'm going to go ahead and say okay and if I don't want my axis to show up anymore I can turn off my construction right there or I can turn it off you know individually like so okay I was able to create a rib pretty fast I want it to go all the way around so we'll use the pattern command again so I'll do a circular pattern again I'm gonna say features and I'm gonna select the rib feature what's the axis I'll select maybe this cylinder here and just like before you can type in how many you want you know in this case I only want three I'll say okay and I now have three of those ribs on that stand off very quickly and very easily okay now I want to basically mirror what we just did so I don't have to recreate so I'm going to mirror it to this other side now in this case if I turn my origin on because I started at the very center I can do this mirror very easily so I'm going to say create mirror again notice I said by default it's usually faces we're gonna come in here and say features and I want to mirror the rib and the pattern at the same time what's my mirror plane my mirror plane is gonna be this vertical plane you can kind of think of it as an actual mirror you would see the reflection in it and I get a little preview over here and I'll say okay and now my ribs are mirrored over to the other side now here's the dilemma I want to mirror this down to these posts but these posts are not perfectly symmetric with this plane or pretty much anything on here and so if I were to try and mirror they would end up floating out here somewhere and that would fail so I need to create a mirror plane now you've already seen the beginning of this I'm gonna turn my access back on I'm going to want to create a mid plane between the center of this circle and the center of this circle if we were to find the mid plane then I would be able to mirror across it but to do that I need to have a plane to select so I'm going to build those planes so check this out I'm gonna say axis through cylinder I'm going to go ahead and select all four of these posts okay we already have this plane I'll go ahead and turn it back on I'm gonna do the exact same thing I'm gonna say plane at an angle we'll select this guy okay I'll shrink them down just a little bit so now I have a plane that cuts through here I have a plane that cuts through here and if I were to come in and say mid plane I can click that plane I can click that plane and it's going to slice right between the two and say okay I now have a mirror plane in fact you can see how far off it was from Center but if I were to come in and say create mirror features I'm gonna select the rib I'm gonna select the pattern and I'm gonna select the mirror okay and then what's the mirror plane I'll come in and grab this middle face there kind of gives me a preview I'll say okay and those rib features are now on those posts they are also okay now again there's probably multiple different ways you could create this I could have created one added the done a circular pattern after I figured out where that axis needed to be for example that totally would have worked so maybe try different methods as you're going through this project okay I'm gonna turn off my construction we don't need to in my origin don't need to see those right now the the last thing and it's kind of hard to see is on the drawing I have the this rib actually extends out to the body and so we're gonna do that and then there's also these little support ribs right here that you can see dimension or point zero eight from an edge Oh point zero four up from the center okay so let's finish up with that we're pretty much almost on time okay so I'm going to create a sketch and this new rib is actually going to go to the very top of this cup so I'm going to select that face and say create sketch okay now I want to basically extend this existing rib so I want to grab some information from it so I'm going to do p4 project I'm going to project just that face okay and I'll say okay then I'm going to draw a line and if I get close enough it's kind of hard to see but it kind of snaps it's gonna it's a kind of hard with the gray but as I get near the center it's gonna automatically snap to the midpoint there and I'm gonna purposely draw off an angle and not all the way okay then I can come in here and say I want this line to be parallel with that line so now I know for a fact that this line is exactly in parallel with the shape of it okay then I'm gonna come in and draw those two lines over here so I might just kind of mock this up real quick now I'm gonna purposely overlap I'm gonna come into something like this and you'll see why here in a moment okay and I'll go ahead and draw another line down here I got a purposely overlap okay I want these two points so click to keep and want those to be vertical with each other so I wanted to keep that one there and then I'll throw some dimensions on here so again according to the drawing that these are Oh point 0 4 I think it is I'm trying to point 4 so I'll do a dimension from here to here and that's supposed to be point 4 from here to here is also supposed to be point four now hopefully you know this trick I could type it in or I could click on an existing dimension hit enter and it references that dimension okay then I know this distance from here to here is supposed to be point zero eight okay now by me adding these dimensions you'll notice for example this dot came out I'm gonna drag it back so just inside this body a little bit and again I'll explain this here in just a second but I now have this line and these two other lines where they're supposed to be so I'll say finish sketch and let's start with this guy here so I'm gonna come in here and use that rib command one more time so I'm gonna say rib what's the curve okay and that didn't go the way I expected it to go why is that some direction that's odd I'm sorry I know why I apologize I got confused I actually need to use the web of command so the rib command is good for things like these ribs right here the web command is kind of like what it's showing in the image where it's going to extend to faces kind of fill in a void so even though I this is a rib we're gonna use the web command what's the curve this guy and then I'm gonna start to drag and watch what we get so you can kind of see what it's doing here it's actually kind of extending to this body here it's extending down to there how far I'm just gonna click on an existing face which is the point 0 4 if I didn't turn on extend curves notice what it does it just grabs that line and extends it but this extend curves is extremely useful and because this face was tapered or I should say drafted it extended to that and it extended to this wall over here I could have made my sketch go all the way into this wall and that would totally have worked that's totally fine but I I left it short just to show you that extend curve now here's the dilemma if I were to add in this edge here notice the results that I get because it's trying to extend the curves and it gets really confused so we're gonna have to break this down into two separate web commands so I'm going to do this first one here I'll say ok and let's turn our sketch back on then I'll repeat that command again I'll come in here and say web what's the curve this guy now I'm gonna turn off extend curves it remembers my last dimension the point zero four and you can see because I drew my point all the way in it's extending basically into the body and it's gonna match okay if I had extend curves on you'll see it extends all the way to this outside edge right here and all the way to this outside edge over here so obviously we can't use extend curves in this case but I can do both of these lines the same time okay and then finally I'm going to mirror so I'll come in here and say mirror the features I want to mirror both of these web features what's my mirror plane I'll select that vertical plane there say ok and we now have let me turn off my sketch we have that weird-looking rib right there that extends all the way to the body and we've got these extra little supports that were supposed to have okay last thing is this is a very black shiny plastic you can kind of see how the lights reflecting off of that I want to simulate that in fusion so I'm gonna hit a for appearance so I click the a command and my appearance comes up and obviously it's plastic so I'm going to select plastic and if I scroll down you can see we've got a couple different kinds like nylon ABS etc I'm gonna do a translucent plastic but you'll notice there's blue grey green white red etc but I don't see a black in here so I'm gonna grab this blue glossy I'm just going to drag and drop it onto my design and I'm gonna start to rotate around and I can see a little bit of light highlights but not as much as I want so I'm gonna right click and say edit and I have a couple options in here so for example reflectance if I drag it down you'll see it gets really flat doesn't look all that great if I drag this up it's gonna reflect a lot more of the surroundings but I also have this roughness and you'll notice if I crank it down and it looks really plastically you know almost too much right you can kind of see the highlight there and stuff like that so I might crank this up a little bit and you can start to see how that highlight is affected by adding this roughness so obviously the higher I go it's you know less polished if you want to say so let's put it maybe right about there okay and then finally the color I'm just going to drag all the way down to zero zero zero which is full black and now we can kind of see what this plastic is going to look like I'll say done and my little icon will turn from blue to black and there we go that is it I only went six minutes over hopefully you learned some new stuff with this I picked a topic which was the draft command to kind of show how you can add draft I would also I just noticed I should have graphed to the outside face I did to the inside face but obviously you'd want to add draft to the outside face also the drawing and the outline are linked in the description of this video please feel free to go through and try this out if you have any questions or comments post them in the video I always go through and read those also post your success out on the fusion 360 Facebook group I love seeing everybody out there you know showing what projects they're working on and stuff like that I want to thank Jason for for actively answering the questions in the chat and again like I mentioned before please definitely make sure you check out the Autodesk fusion 360 live Facebook group and see what the upcoming live streams are like here's one that we just did that what's new and the March release definitely watch that we talked about you know the the 3d splines for example here's Tyler's live stream he did yesterday um you know creating that welded tubular front atv frame you'll see upcoming live streams etc so with that I want to thank everybody I missed you all when I was gone glad I'm back I know that sounds bad yeah saying I'm glad I'm back from vacation but with what's going on out there right now we're doing everything we can to make your lives more successful and more enjoyable so thank you and have a wonderful rest of your day happy fusion team you

Channel: Autodesk Fusion 360

Views: 9,599

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, computer aided design, free software, 3d modeling tutorial, control arm, manufacturing, pumpkin, freeform, surfacing

Id: RE93prVAIho

Length: 70min 9sec (4209 seconds)

Published: Thu Mar 26 2020