360 LIVE: Laser Projector Build - Part 5 Heatsink & Gears

hello everyone and welcome to another episode of fusion 360 live my name is Brad tylose I'm from Autodesk I've got a Jason helping me out on the chat so today's topic we're gonna be creating this heatsink that you see on the screen this is part of that laser projector kind of thing you can kind of see this heatsink right here holding the sorry the camera is out of focus holding the laser diodes in there before we get started I actually wanted to point something out let me bring up a webpage so we've been getting comments you know we're doing a lot more live streams and people are like oh I'm not getting notified of when these live streams are happening and unfortunately YouTube is not the best for alerting you when the upcoming live streams are happening so what I personally recommend if you haven't already in YouTube do a search for fusion 360 live okay and that'll bring you to this channel right here make sure you subscribe if you haven't already but you'll see right here upcoming live streams and here's a list of the upcoming live streams and they're listed at the on the particular date and the particular time in your time zone so I'm in the Mountain Time Zone so this says 12 o'clock which is where we're at right now they're doing this cam hangout I think on Saturday it looks like Jason is doing his second part of his sketching livestream next week and notice the time and again make sure you look at what the time says when you go to this webpage because this time will be per your time zone so I recommend coming out here quite often honestly we're adding new live streams constantly I noticed in the chat before we started people were asking where's Lars well guess what on the 30th Jason and I thought it'd be kind of fun to hang out where we're gonna answer your questions you know we'll look at the chat the chat will answer some questions we'll kind of give you our background and stuff and we thought it'd be fun to bring in a guest speaker so of course we invited Lars so you'll find out what's he doing now and all that kind of stuff so definitely make sure you mark that one on your calendar now you can set these reminders but I've personally found that they aren't very helpful it sends you an email and unless you're on your email constantly you won't know so I personally recommend cleaning them in your calendar setting an alert etc you'll notice that we're having a lot of the the ecad types webinars in here also and we're constantly adding more and more topics so I recommend coming and looking at this at least once or twice a week if not more so okay let's dive in like I mentioned before we're gonna be creating this heat sink and then a couple of the gears there's some some small gears and it's gonna be kind of hard to see on the camera that rotate the the lenses in front of the laser so we're gonna we're gonna do basically two different topics today we're gonna learn a little bit about this heat sink and then we're gonna learn about some gears now this heat sink isn't overly complicated but I am gonna share some tips and tricks with you it's just kind of what I'm famous for you know different methodologies different ways of designing things that I ran across when I was reverse engineering this model so also in the description of the YouTube video livestream I've included the drawings for the heat sink and for the gears okay and then I've also included my outline which I usually put an outline out there so you can kind of follow along now it's they're pretty cryptic you know but I kind of highlight and bold kind of the key things but this is what I put together as designing the model so feel free to download both of those and use them to create these parts I I love seeing what people are doing I noticed I'll give a shout out to Steve Sneed he watches these live streams and post a video or a picture out on the fusion 360 Facebook group and it really warms my heart to see that the work that you know Jason and Angelo and all those guys and myself are putting into these live streams really are paying off so we love seeing what you guys are doing so make sure you post those out there if you want to you so so shout out to Steve okay um let's dive in so the first thing I'm gonna do is I like and you've heard me say this multiple times I like to start out by creating a new component that way everything is organized underneath these components so I'm gonna just call this one heat sink coming pretty self-explanatory I'll say okay and now you can see I have a component called a heat sink okay and again using this drawing so you'll notice that kind of dimensioned certain things out and all that kind of stuff how far things are separated etc so I'm going to use that too oops I go to this guy create my sketch so I'm gonna start and I'm gonna do the front plane in this case and I like to keep things as symmetric as possible so I'm gonna start with the rectangle and I really like this Center rectangle command and what that allows me to do is pick this zero zero and I'm gonna create a rectangle that's one point nine two wide now I'll hit the tab key to switch between my height or my length so I'll come in here and say one point nine two I'll hit the tab key in and I can do 0.25 tall let's kind of zoom up on this a little bit so again use the tab key to jump between those I'll do the exact same thing again I'll create there's another smaller rectangle and it is point 2 9 and again I personally like to type in the length first and then the height so point two nine by point two and notice everything is kind of centered okay the next thing I want to do so basically what I did here is I drew and I apologize for the flashing but it kind of highlight you can kind of see this rectangle here and then there's going to be a smaller rectangle in the center now you'll notice I didn't dimension where these circles are and that's because we're gonna let fusion define where they are and so you know as you're looking at some of my drawings you're like man he's missing a ton of dimensions I actually do that on purpose and it's for you to follow along the outline and follow along the video to see how powerful fusion really is so I purposely left dimensions off that way you have to use the special tools so okay so what I'm going to do now is create a couple circles and I'm going to purposely create them in the wrong location so these are point seven one okay so you can kind of see I can put that there and then I'm gonna draw another circle purposely in the wrong location and purposely the wrong size okay now I want these to be the same size so I'm gonna use the equal constraint I'll say I want that circle and that circle to be equal I also want them to be horizontal with each other so I'm going to say horizontal vertical and I'll click the center points of those and you can see how this one dropped down and now they're at the same level so if I were to move one the other one has to move also okay then finally what I'm going to do is put a dimension on here so I'm going to say from here to here I want that to be exactly one inch in this case and you can see how they move together now I want to put them in the correct location so I'm going to go ahead and say tangent and what this is going to allow me to do is I want this edge to be tangent with this edge of the smaller rectangle so I'm gonna you can see I mean my tangent constraint so I'll click there and then I'll click there and you can see that they moved over if I were to move down you can see that sure enough their tangent okay however they're still in the wrong location let me just drop it right there for example the last thing I want to do is line them up with the center so one more time I'll do this horizontal vertical and I can click that point and that point there and you'll see that they dropped down into location and they turned from blue to black which means that the sketch is fully constrained okay so I used a couple different constraints there to help me with this design I could have left off this one inch and made both of these tangent that's totally fine but I was kind of showing you how we started out here in space and then we kind of force the circles to go where we wanted them to go using constraints okay I have mentioned before I like to keep my sketches simple so I'm gonna leave it at this and then I want to extrude now I don't want to extrude what I'm in my outline I call these the little wings I don't want to extrude those so I'm going to draw a box like so and notice I was able to select all of the probe using a selection window otherwise I would have had to click here control click here control click here probably have to zoom up a little bit grab all of these regions and you can see how lengthy that's taking well just draw a selection box around making sure you don't go too far because then it would select that wing but I'm just gonna do something like that and it allows me to select all of those profiles with one click ok now I can right click and say extrude will start to drag and we can kind of see what the profile looks like and according to the drawing and again I'm not gonna jump back and forth too much but it's 1.8 in depth and I'll say ok now like one of the other reasons I mentioned I like components is I can expand these open and for example I can expand open my sketches I can expand upon my bodies and I can turn my sketch on or off at any time I really like that flexibility ok the next thing I want to do is I want to you know hollow this thing out ok and now you can kind of see why we didn't do these little wings at first because we're gonna shell this part out and I don't want the shell to go into this little extra area right here so we're kind of breaking it down into smaller chunks smaller components I'm going to click on this front face right mouse click and it shows me the commands that make sense now Jason showed some really cool functionality in his live stream one of the things I'm really bad at is the S key if you hit the S key on your keyboard you can search for particular commands so for example I could start typing in shell so I type in SH and there's the shell command so if you're used to like typing in commands or if you're really used to going into menus and having to look for it or whatever that S key is a really cool shortcut and it allows you to even run the command right from that shortcut key that s key so we're gonna do a shell I'm gonna click that front face and I want to select the back face and I've shown this but I'm gonna reiterate if I click and hold it allows me to probe through and grab so it's almost like a laser pointer so the laser would first hit this front face and then it would hit that back face so I can actually select both of those faces without having to rotate and I know personally that especially if you don't have like a 3d connection mouse or a 3d mouse having to rotate can get pretty cumbersome if you're doing it over and over again so I really like to probe through and select those faces without having to rotate ok the thickness is gonna be point zero seven five according to the drawing and I'll go ahead and say ok and again right here is that point zero seven five kind of showing the thickness of that shell I use the shell command all the time I could have drawn and you know on my sketch I could have drawn a couple more circles couple more lines and just extruded that particular profile but that would have taken a lot of time and then if I wanted to change the thickness I'd have to change multiple dimensions I'd have to change that circle I'd have to change that circle I'd have to change this dimension between those lines so I think the shell command is extremely useful ok now I'm going to turn my sketch back on and I can select these two regions I'll right-click and say extrude or you can hit the e key as the shortcut key and I'm going to start to drag now again I could type in the demand or if I just click you can no this is I'm gonna hover over here it's gonna snap to that okay or I could come in and say all and you'll notice that's more for like cutting stuff away and so it's same tool body creation failed so I've gotten this question before we're all it's like well can't you just say through all and it'll go here well it doesn't no it's trying to go to infinity basically and it can't find anything to intersect with so in this case I like to click with distance or I can say to object and here I would have to select and rotate and grab that back face right or I could have probed through so it's really up to you I I usually keep it to distance and I just hover and click okay obviously we want to join that together and now we have those little wings what's not what's I'm calling it in the outline and then finally I've got this smaller rectangle I want to remove that so I'm going to click here and say extrude again just click on that back face and you can see that it's gonna do a cut through there because it's overlapping geometry I'll go ahead and say okay turn off my sketch and you can kind of see what we did there using just basic sketch you know a couple circles and a couple rectangles and then we use parts of that sketch to do a couple different extrudes okay I want to chamfer these you can kind of see right here we've got these little edges right there and iíd tail them out point zero five chamfer on those edges so I'm going to do that now a couple different ways I could do this so I'm going to go ahead and click on this edge here and say chamfer now I could type it in because that's what the drawing says okay or let's pretend maybe it wasn't on the drawing and I just wanted to change this face to be sloped so check this out I'm gonna right click and say chamfer and then I'm going to click on this little down arrow and say measure and what that's going to allow me to do is to pick on an edge and it's going to measure that edge and put that into the distance and that's how I actually came up with a point zero five instead of having to guess or type multiple different numbers like point zero three point zero four point zero five you know you can just measure that existing edge and I'm gonna go ahead and select all four of those okay I'll say okay and there we go quickly chamfer those and I could always come back and edit that in the timeline if I wanted to the next thing I want to do is I want to create these holes and I think I realize I didn't dimension them so I'm gonna have to update the drawing I apologize they are in the outline their point one diameter but I should have put those in the yang this actually means a lot of work I apologize I need to locate where they're at so follow the outline and not the drawing I will update that and re-upload it into the description so maybe wait a couple hours after this livestream and I will update that drawing I apologize guys okay I want to create a hole I personally like to use the whole command which you can see here is in the my shortcut right here at like about four o'clock okay or it's in the create menu hole or the H shortcut key okay now you'll notice it just puts it on the the face randomly and it's really large this is supposed to be 0.1 in diameter okay now I want to put it in a certain location and you'll notice as I kind of zoom up here and move around you can see this black line appearing and this is what we call our reference and you can see it even says add reference and you can see we have two references in the menu okay so all I have to do for example is I'm going to click on this edge and it's supposed to be point zero nine and so you see the circle kind of moved over a little bit okay then I'm going to click for example on this top edge and that is supposed to be point one two five and you'll see now it's referencing this edge of point zero nine and referencing this edge 0.125 and that's how I'm able to kind of position where I want that circle to be without having to use like a sketch or a projected geometry or anything okay now I want it to go all the way through as a simple hole it's just a it's not even tapped or anything like that so I'll keep it simple and I wants to go all the way through now by default it looks like it is okay but let's pretend that it was and I'm going to drag this back let's say maybe it came in looking something like this here I could come in and say go through all and it's gonna go all the way through the model correctly okay so I'll go ahead and say okay and then I'm going to do the same thing on the other side now I could mirror that's totally fine this is really up to you I could mirror this whole feature or I could create another one again it's it's up to you what you think is better there's no right or wrong in honesty I'd probably mirror it just because that way if I change one both of them change but I'm going to go ahead and do that whole feature again just to kind of reiterate how it works so in this case I'm gonna say hole and you'll notice it's randomly on that face I can grab that blue dot move it around if I want to but you'll notice it's not gonna snap automatically to anything if I get near an edge you see it doesn't snap to that or whatever so this is where that reference really comes into play so again I'll do that and that's supposed to be the point zero nine and that edge there is the point one two five one two five and distance I'm going to say go through all and it's gonna cut all the way through the model okay and like I said I would probably mirror that feature but I just wanted to kind of show the power of the whole command okay looking at the drawing you can see that there's like a little notch that goes into this little hole region and it's a point zero six five wide so I'm gonna edit the sketch and you know use a basic rectangle to do that to cut that geometry away now I could create a new sketch but because this one sketch should already have has a lot of the information already I'm actually gonna go all the way back in time edit that sketch now we're at the very beginning so that's why you don't see any 3d model or anything like that but I'm gonna go ahead and use this sketch and add some more complexity to it so I you've heard me say before keep your sketches simple and and in this case we did couple circles couple rectangles but now we're coming back and then just a little bit more to it and we're gonna use that downstream it'll be pretty cool actually so instead of having multiple sketches we're gonna kind of keep it to one sketch in this case so I'm gonna say rectangle I love the centered rectangle so all I have to do is get near this edge and you can see it's snapping to that edge and if I get near the mid you'll see that it automatically snaps to the midpoint for me right there and then I can type in the distance so in this case I'm gonna say point one two five and the overall height was point zero six five okay and you'll see how it's fully defined it's constrained to the midpoint so the line is black I'll do the exact same thing on this other side now I get asked well couldn't you just mirror that and the answer is yes I could but I have to have a mirror line and so I'd have to spend the time drawing a line changing it to construction geometry etc where maybe I just want to draw a rectangle and I don't care what size it is like so and then I can come in and say equal I want that edge and that edge to be equal I want that edge and that edge to be equal and you can see no matter what this dimension is over here or these dimensions are this one has to be equal to it so if I made this let me escape out of here if I made that point one you'll see that it will update and so will this one over here does they have to stay equal so again it's totally up to you whether you want a mirror or if you want to add constraints or whatever I I personally don't like to use mirror all that much because it adds a lot of extra constraint icons onto my sketch I like doing mirror in 3d versus 2d so but again it's totally up to you so I'm gonna say finish sketch now here's the cool thing so we just went way back in time and edited that sketch and when I said finish sketch it came forward in time and did all of the extrudes and the shells and the holes etc and you might be saying well how come it didn't you know punch those holes through well because we didn't tell it to for example in this extrude we told it to use these profiles we didn't tell it to use these rectangles or anything like that so it's kind of cool that you can go back in time and edit that sketch now I can turn it on I'll go ahead and add in these profiles now I like to over exaggerate so I'm going to grab even the stuff that's out in the air now you might be asking well do you have two and the answer is no but what if this face ended up being drafted one degree or something like that down the road well then this would create a sliver face you know so I like to do something like this that way even if this face changes if it gets drafted a degree or whatever we're obviously still going to be cutting through it it's almost like this is a big cutting tool okay again you could totally do it this way it's it's up to you but I like to make sure okay so I'm gonna say extrude I could say this in this case I could say extrude all and now because there was geometry that it was interfering with it knows how far to go whereas before when I tried to do it it didn't know how far to go and that's why through me that error I'll turn my sketch off and you can see we just kind of created those grooves through those holes okay I'm just following along my outline here so the next thing I want to do is we've basically created the main shape this little dog bone whatever you want to call it then there's this added little area which on the model I'm not exactly 100% sure what it's for you can kind of see it here so there's the two laser diodes and then there's this and I'm not sure if that's like a thermostat so it's checking to see if the laser is getting too hot and if it does maybe it automatically shuts off is my guess but we're gonna go ahead and create that geometry there so let me put that down okay so I'm gonna draw this circle here and we can see that's point three up and point three over with point four diameter okay now I could go back and edit this original sketch but now I'm kind of like okay I'm done with this area now I want to do this other area so I'm going to create a new sketch so I'm kind of breaking this down into like these sub components and I just want this circle over here to kind of be by itself and not be part of the original this is just a personal preference not saying this is how you have to do it so I'm gonna come in here and say point four for the diameter I'll throw some dimensions on here so I'll go from here you can see it'll automatically catch to the center of that circle I've shown this tip before I'm just gonna reiterate it when I go to move my cursor you'll notice my dimensions aligned or at the wrong angle or whatever if you move around you'll get it finally to go horizontal or you'll get it to finally go vertical but you kind of have to know where to go to make that happen well if you have a hard time with that just right mouse click and say I want this to be a horizontal dimension and now you'll notice no matter where I move it has to be a horizontal dimension so I'll say 0.3 I'll do the same thing again click those two points and you can kind of see how moving around is gonna give me different results or whatever but my right mouse-click I can say I want this to be a vertical dimension and now no matter what its going to be a vertical dimension so just that might help you down the road so I'm going to say point three and point three and we can see that it moved that circle into place okay okay I'm gonna leave it like that say finish sketch click on my profile here now I'm not gonna select you know all of these profiles I don't need to okay I'm just gonna grab this outside one right here I'll say extrude and just click on that back face you'll notice I haven't even had to rotate or even look at the back of this thing at all yet okay and I'm gonna join that together so it's going to take that profile join it to that model now I want to create the 0.25 hole that goes through there like I mentioned before I really like the whole command so I'm going to say hole and notice it randomly put it on that face well here's a cool trick if I grab this blue dot and start to move around notice all the little dots on the screen now obviously there's one right here that's in the center of this circle right here there's also one down here there's also a couple over here and a lot kind of stuff so if you already have the geometry existing it's really easy to automatically catch to the center of that feature basically again not having to use a sketch to do that it's 0.25 in diameter I want it to go through all so we can kind of see you sure enough I'll say okay and the other reason I like using the whole command is I can always come back and in fact I could even click the face in the on the part itself and it highlights which whole feature that was in my timeline just by clicking on the face you can kind of see that so I can always come back and edit this and say okay maybe 0.25 is too big we want it to be 0.2 for example and it's a very quick and easy way of changing that I'm not going to do but you can kind of see why I like using the whole feature okay let's take a look at our drawing we pretty much modeled all of this stuff here we've got that extra little hole the next thing is the ribs or the you know I guess the ribs on the heat sink oh and this is where I'm gonna share a couple neat little tips okay let me jump back here and I'm gonna do this a couple different ways to kind of show you what you might experience so just like I said before I kind of like to break this down into smaller sub components so I want to create another sketch so I'm actually gonna click on that face and say create sketch could I have gone back to this sketch or even this sketch absolutely I could have it's again it's up to you but I like to kind of keep my sketches defining which things I'm working on so obviously this sketch is gonna have to do with the ribs so I'm gonna start out by just drawing a rectangle out here somewhere okay obviously I drew it too big and I drew it in the wrong spot but like I've shown before I like to dimension this I'm gonna come in here and say for the total width it supposed to be point zero three okay and for the total height that's supposed to be point three I know a lot of these numbers are pretty similar okay now if I grab this you'll see that it's gonna stay the same shape now here's an interesting thing you'll notice I mean kind of I'm gonna undo here real quick I'm gonna zoom up so you can kind of see what's going on I'm gonna drag this corner point and if I get near this edge it's really hard to see but now there's a little X underneath it and you can see as I'm moving it's actually following the curve so it's actually gonna create a coincident constraint for me automatically okay and if I hover over it sure enough we can see that coincident constraint that it created or I could come in here and say coincident that point with that edge and I get the same result and you'll notice now and dragging that rectangle and it's following along so my tip here is fusions gonna try and create the correct constraint for you automatically or you can force it you can tell it I want this to be a coincident constraint so just kind of a heads up there right okay so I make that coincident with the circle and then Jason showed this in his beginner sketching I use this all the time I'm six I want to Center this and if I were to come in here and let's try it the wrong way I'm gonna say midpoint I want the middle of this line to be in the middle of this line here you'll notice it can't it won't let me fail to solve okay so how do I get this to be perfectly lined up well a quick shortcut is just draw a line from the center to the center of the circle you kind of see how that's snapping to the center of the circle okay then I usually turn this to a construction line because I don't want it to cut through my model and then finally I click horizontal vertical and notice what it did okay it still had to keep this point coincident on this edge but then it brought it along until this line was perfectly vertical so now I know that my rib is perfectly centered where it needs to be okay I recommend re watching that on the video if you haven't tried this out but it's kind of a really cool trick like I mentioned you know Jason showed it in his sketching that last week I use this all the time I think he uses it all the time I think he's the one that taught me how to do it if I remember correctly so okay so I finally got my profile where I want I'm going to extrude this okay how far I'm just gonna click and notice it says join now I'm gonna do it the right way first and then I'm gonna come back and edit my timeline and do it the wrong way and show you why I'm doing it this way I'm gonna actually say new body okay not new component not in this case I'm gonna just say new body because I want this body to be part of my heatsink component and just say okay and now you'll notice I have this part and I have this part and it's a separate body and you'll see why here in just a moment okay I also want to add some draft to this now I talked a lot about the draft command in last week's livestream so hopefully you're comfortable with it now so I'm going to say draft and I want these faces to kind of splay out so my draft plane is going to be here because I want this edge to become a hinge right so that's what the draft plane means you can kind of imagine there's a long piano hinge right there so now if I select that face and that face and we add some draft to it I didn't select the other face sorry you'll see that it's hinging on that draft plane okay so that's what that draft plane means now we're only gonna add about half a degree of draft we don't need a whole bunch here but it is gonna splay it out just a little bit if I look at it kind of from the front you can kind of see that how it's angled up okay so I now have created my rib and here's kind of where the magic happens we're obviously gonna create a pattern a circular pattern to make these ribs but we're gonna want to be able to not have all of them appear so check this out I'm gonna come under create pattern circular pattern now by default it's usually set to faces I love to use features but notice one of the options is bodies now I could use features and select my extrude and my draft features and that would work but because we created this as a separate body I can just say pattern that body right there okay what's the axis well the axis I'm just gonna click either on a cylindrical face or an edge it doesn't matter and you'll see I get a preview and as I increase the quantity you know the preview updates accordingly now according to the drawing there's 22 ribs so I'm going to type in 22 and you'll see it creates quite a few ribs that's let's take a look at it from the front okay so here's the cool thing I wanted to show you notice right here it says suppress and it has a checkbox and you'll notice that every single rib has a checkbox on it and so I can click on any of those to unselect them so I want to keep this one but I don't want that one that one I don't want these two that I've already unselected and I don't want that guy and that guy so I still have 22 ribs going all the way around but then I removed a couple of them okay think about how complex my sketch would have to be you know to you know create this as a sketch and not have them here I'm gonna go ahead and do the pattern and then suppress some of them so they don't appear when I say okay here's the result and notice I got a ton of bodies over here okay then all I have to do is combine so I'm gonna come in here and say combine what's the target that's the target what's the tool well I could select them individually or I'm just gonna draw a big box around all of them I want to join them together and you can even see the preview kind of shows the lines have gone away when I say okay we are now back to one body and it kept the ribs that I wanted and I was able to remove the ribs that I didn't want okay now I'm gonna step back quite a bit and we're gonna redo all those ribs because some of you might be saying well couldn't you have just joined it and then pattern the feature and the answer is yes but watch what happens when I do that okay so I'm gonna undo actually I don't you have to undo let me well yeah well let me undo back sorry let me go to my extrude and instead of saying new body I'm gonna say join actually let me let me do it the right way I'm going to step back okay instead of new body I'm gonna say join and you'll notice when I say okay it's joined that rib to the part okay then I'll come in and I'll add my draft there's my draft I don't know if you can see that it's kind of cool it was before there it is after a little bit of draft okay now I'm not gonna bring ups bring up this pattern I'm gonna recreate a new pattern so let's go here and say pattern circular pattern now obviously I don't want to do the body so I'm gonna come in here and save features because this is all one body I don't want to pattern that obviously right so I'm gonna come in and say features and I'm gonna say I want to pattern the extrude feature and the draft feature but notice what it's selected okay and when I start adding in I'm getting kind of a weird preview right well that's because this rib was joined to this body if I were to say okay let me just do five if I were to say okay you'll notice it does it correctly but the preview is pretty darn confusing in fact watch what happens when we get to 22 okay and it's difficult to see which ribs do we want to turn on or off and stuff like that so this is the exact reason even though it's really pretty this is the exact reason why instead of joining the rib I ended up doing it as a separate body and then patterning it and then combining it together okay so hopefully that makes sense there so I'm gonna go ahead and delete that guy let's edit this guy again and make it a new body and I should be able to step to the end and there we go okay so quick review when I did the extrude we kept it as a separate body I was able to add draft I was able to pattern the body okay I was able to suppress and I get a really nice preview what that looks like and then I did the combine to join them all into one body okay hopefully that makes sense and and the only reason I'm showing this is because you know I ran into this when I was reverse engineering this this model so you might run into something similar and hopefully these little tips and tricks will help you down the road okay finishing up here I'm going to click fill it on that guy and do a point zero two and I must talk too much because I noticed we're almost near the top of the hour so I'm just gonna go ahead and fill it those guys I want to make sure I show the gears so we are gonna go a little bit long which I do appreciate everybody says we don't care if you go along so again you can always rewatch on the YouTube channel later on okay the last thing I want to do is there's a hole and man this drawing is awful I apologize I must have man I must have missed a lot of dimensions or missed a version or something so again I will update the drawing follow the outline so I'm going to create a sketch on here now in this case I'm not gonna use the whole command and the main reason for that is the whole command doesn't like to be out in the open like this it likes to be on a face and I don't really have anything to reference so I'm gonna use just a regular circle command so I'll say circle and I'm gonna purposely draw it in the wrong spot and point one in diameter I'll throw some dimensions on here so I'm going to grab that guy and it's supposed to be 0.5 from the edge and then I want it to be in line with this origin so again that horizontal vertical is extremely useful because it forces those to stay horizontal I can see that it's fully constrained I can now click on this profile here and extrude fruit okay so I could do to that face or I could say all and it looks screwed all the way through the model and there we go okay the last thing I tell you to do in the outline is to add an appearance so I hit the a key on my keyboard I'm gonna go into metal under aluminum there's one called bead blasted and this aluminum is kind of looks like it's bead blasted so I'm gonna go ahead just drag that on there it doesn't look like it did much but if i zoom up you'll actually see that there is a bead blasted texture on there and it just adds that little bit of realism and we can kind of see that that's made out of be bast blasted aluminum okay not a complex part but I wanted to show some tips with the patterns that kind of stuff so now we're gonna do the gears and the gears are not that complicated and I did see a comment before we started somebody said Oh gears are very difficult and Jason actually answer or somebody else I think it was actually another viewer answer there's some plugins and that's exactly what I'm gonna be showing here there's some really cool plugins out there that will speed up the process for you so I'm gonna show that live let me switch back I'm gonna create a new design and there's two different gears and they are slightly different from each other but they're pretty similar so I'm gonna start with this drive gear and the reason for this is you'll notice there's this little square boss that actually connects into a shaft that rotates the are actually connected to the stepper motor now you'll notice I have an image here with lots of information and it says FM gears this is the actual app that we're going to be using and I'll show you how I went about doing this but it actually creates the complex tooth profile for you automatic all you need to know is like what's the pitch diameter I'm sorry the hole diameter and you can see you can fill these in how many teeth thickness of the gear etc so we're gonna use that to kind of get the basic shape and then we'll just add some extra stuff on to it okay so where do you get this fm gear I'm in a new session I'm gonna create a new component and I'll just call this gear wants to call it drive gear I'll say okay there we go okay if I go into this tools tab right here there's a section called add-ins and you'll see says scripts and add-ins and then fusion 360 app store I'm gonna click on that app store and of course it's gonna bring it up okay good it brought up the right window this is our fusion 360 app store and you'll notice that there's some featured apps like slicer a bomber etc helical gear generator well I'm not just coming here and search for gear and hit enter and you'll see there's a bunch of different ones bevel gear design spur gear helical gear rack gears etc then there's this FM gear so I'm just gonna go ahead and click on that guy and it gives you a description it talks about what it can do you know what people think about it reviews etc and then I can come in here and specify which OS sometimes it'll say Mac sometimes they'll say PC and I just hit download and they'll probably ask me to log in I'll go ahead and say next and sign in using your Autodesk ID and you'll see that it's gonna download that and I just ran it and it installed it I doesn't have to do anything special or spectacular okay then I go back into fusion under my tools scripts and add-ins now you'll notice we already have like spur gear in there but I'm gonna go to this add-ins and there it is FM gears okay here's another one I use all the time parameter IO okay the Veroni sketch generator etc so this is where they usually show up so if you click on FM gears mine's already running but let's just say stop you might have to hit this run and you'll also notice you can have it run on startup so you don't have to remember to do this every single time so I'm gonna go ahead and say run and it says the FM gears command has been added to the create panel of the model workspace okay so here's I'm in my design workspace create and right here FM gears so if anybody writes a plug-in or an add-in or something you can add them into Fusion very easily and there's more than just gears there's like dog-bone creators for your sketch if you're having parts fit together I mean there's a ton of stuff out there I recommend taking a look at that okay so here's the FM gears and I could make this a little bit bigger the the image kind of talks about what it's expecting and you can see like this blue line or purple line is your pitch diameter etc I've already provided the information I just basically reverse-engineered the gears that came in this laser projector so the whole diameter is point zero five it's a very small hole pressure angle is 20 the diametral pitch is gonna be you can kind of see that right here that's gonna be twenty six and the number of teeth is gonna be 24 I left the route Filat radius that's kind of like what this is right here it's kind of hard to see and then gear thickness is point one seven now watch what happens when I say okay it's gonna think for a little bit you see it create a sketch and then it extruded that in fact it created its own component so I'm going to go ahead and get rid of mine you know we don't need that one in there I'm gonna make this one active so they created its own component I forgot that I was going to do that okay and if we take a look at this we can see sure enough it's 26 teeth here's the that size that we were we're talking about the radius etc I did not have to draw a sketch here's the point zero five hole diameter through the part okay and again this is all listed right here this is what I use to type in those numbers okay using the rest of the drawing I'm going to create these little standoffs this little indentation and these holes okay so the next thing I'm going to do is basically now that I got the gear the way I want it I'll just create a new sketch again I'm making sure that my component is active I can see all the sketches that were used to create it and now my new sketch and then I can add in some extra geometry so I'm going to throw in a circle it's point four to two in diameter okay I'm gonna offset that in so what's the sketch curve I'll go ahead and Susan's thinking hopefully it's not Auto saving Wow give me just a second guys there we go okay the joys of pushing a lot of data over hill on stream okay it's asking for an offset and I'm gonna type in - point zero five okay I'm getting a lot of lag I'm gonna save just in case I don't know if hopefully my son is not streaming videos or like that so I'm gonna do an offset in fact I'm going to save real quick give me a second here guys wait say I'm just gonna call this drive gear okay um oops accepted my offset so I'm gonna type in - point zero five now I could have typed in you know diameter of 0.42 - and then figured out the math and made another circle but I like to use the offset command because it allows you to specify a distance and I'm just gonna say it's a law thing as a point zero five then I'll do a rectangle Center rectangle here and this is supposed to be point one two five point one two it's just a square rectangle I can select those two profiles and to say extrude let's just do a point one five for the extrude you can kind of see how easy this is and we're gonna join that to the existing gear the hole still goes all the way through it's pretty much done with the front of the gear now I want to work on the back of the gear so I'm going to select the face right click and say create sketch and now we're sketching on the back of the gear okay as you can kind of see how the sketch is on the back again just using information from the drawing and all this information I know the gear drawings are good okay so this is supposed to be point seven in diameter and then I'm gonna draw another circle over here somewhere and let's just make this point zero six okay and like I've shown before I always over exaggerate I draw it not where it's supposed to be and that way when I come in and I start constraining it I can verify and visually see that things are happening correctly so 0.3 over and then I want that to be horizontal with that and I can see it kind of jump down into and it's perfectly lined up and it's fully constrained okay this next tip I actually just learned I answered a question on the forum and somebody was asking like how would they mirror something from upper right corner to the lower left corner of like a rectangle and I was like man I wish I could use like pattern to do that but I ended up doing mirrors and stuff and somebody says oh you can use pattern just do a quantity of two so I could mirror this circle but instead I'm just gonna come in here and do a circular pattern what's the object that guy Centrepointe is already there I didn't have to draw any extra geometry and instead of a quantity of three I'm going to say a quantity of two and you can kind of see it's almost like it mirrored it to the other side so I thought this was a really cool tip and this is a simple example you know there's was going from one corner of a rectangle to the other but I just thought this was a neat tip okay so I'm going to extrude this profile into the part now you'll notice I didn't select these circles I could have but you'll notice it's not necessary in this case so I'm gonna go ahead and specify the distance according to the drawing it is supposed to be 0.1 so I'm gonna say minus 0.1 I'll say okay and I'm left with something looks like this I'll turn that sketch back on and this time I'll select these profiles say extrude and as I start to extrude you'll notice it's basically machining them away in fact it's gonna go all the way through I'm gonna just pick on that bottom face say okay and I'm now left with something that looks like this so we use the plug-in to create the gear and then we just modify that to add some extra geometry to it I'll go ahead and turn off that last sketch I'm gonna add an appearance and in this case these are made out of nylon so I'm gonna switch to my plastic and here's that nylon 6-6 I'm just gonna drag that onto there and now it's made from that material now this is just an appearance let me show this I'm gonna go to the create menu let's see if I want to sorry modify menu we have appearance and we have physical material if I wanted to simulate like how much this thing is gonna weigh what's the mass properties and stuff like that I would definitely want to make sure to use physical material and it looks almost exactly the same I could come in here and say plastic but you'll notice I've got a bunch of different plastics in here okay and then I can drag and drop that on there and it's gonna apply not only the appearance but it's also going to apply all of the mass properties of that particular body so if I were to come in here and go to properties we can see the appearance and the physical material how much it's gonna weigh what's the total area etc where's the center of mass etc etc so make sure if you're curious about all the you know the mass properties make sure you're using the physical material okay moving on to the next gear it's I'm gonna go a little bit faster but there's an interesting thing I wanted to show in this one which are these little slots that kind of go through like how do we create those so I'm gonna again use this information that you see here to create the gear it is slightly smaller than the last gear but then I'm gonna focus on the pretty in those slots cuz there's some kind of cool tips and tricks with that and it shouldn't take very long okay so new design and I'm going to go to my create fm gears now this time I'm gonna change this is going to be point three two so it's gonna be much larger hole going through that pressure angle is 20 now you'll notice this pitch diameter watch what happens to this pitch diameter as I go through and edit some of these numbers you'll see that it actually updates automatically so this is gonna be twenty six point five and sure enough you can see that pitch diameter changed number of teeth is going to be 23 in this case I'm gonna see that and the thickness is point one seven I'll say okay and notice for example in this case the hole is much larger coming through okay and it's a smaller diameter now I want to make sure I'm gonna activate that component otherwise everything is gonna be at my top level so I'm gonna go ahead and say activate that component I'll expand it open just I like doing that okay and then let's just quickly create a sketch a circle here notice that's lots of comments and questions in the QA so Jason thanks for helping answer all of those hopefully everything's making sense for everybody I'm gonna do a point four to two circle here and extrude that profile 0.15 just like we did on the last one okay and then the next section is working on the back of the design and this is where we're gonna create those slots so I'm going to click that face create sketch and again using this drawing here so you can see I gave some dimensions there point one up and point one down and in the need to give the width again it's in the outline I must be really bad at creating drawings I apologize so I'm gonna create a circle and it's gonna be point six eight five and I will update those drawings okay then I'm gonna create another circle 0.6 but this is what we're going to kind of use as a reference I'm going to click on it and change it to a construction circle okay I don't want it to be an object okay and we're gonna use this construction circle to create a slot now we don't have a squared off slot but we do have these arc slots which are really cool and I'm gonna use the center point arc slot okay so the first thing is asking for a select center point of arc so I'm going to click here and then it's I'm gonna go ahead and click somewhere on this circle there and then somewhere over here and then finally when I move you can kind of see what's happening okay well I'm actually going to click on that line or that circle I should say and I just created this curved slot now I didn't do any dimensions it didn't really ask for any dimensions it was all just kind of clicking around now I want to make sure everything is good you'll notice I can come in and say I want this point to be coincident with that circle make sure I did that sure enough I did and you'll notice how this arc is now black this arc gets kind of hard to see is also black so I've constrained this slot to the edge of that circle now I need to add some dimensions in here so I know from here to here is 0.1 and we can see that that turned black and I'll say from here to here I want that to be the same so I'm just gonna click on that existing dimension and hit enter and I got a different result which is not what I expected so let me undo I wonder why that like one yeah that's not sure why it's doing that so I'm going to type in point one Wow it might be because of the tangent thing so let me let me delete this again live everything's live I'm gonna bring that up like so let's see if that makes a difference oh look go in here go in there and say point one yeah okay so it happens to the to all of us right so what I ended up doing is I was getting some weird result I don't know why I'd almost looks like it was measuring off the right side of the circle so I just stepped back a little bit and forced a change and then through that dimension back in there and that seemed to fix it so okay now I got that the way I want the last thing I'm going to do is I want to square these off so I'm just gonna get near this arc right here and then you'll see it kind of snap automatically and then snap automatically it's kind of hard to see cuz of the gray background but it's catching to the end of this arc and catching to the end of that arc so all I have to do is get close get close and now you can see I'm left with this squared off curved region so yeah it took me a little bit of time to create the slot but think about how fast this would be doing it this way so I'll go ahead and say finish sketch let's extrude that through so I'm going to just kind of start to extrude click on that back face like so okay then I might come in and create a circular pattern feature I'll use that extrude feature what's my axis I can either click on that or maybe the center axis through here and then again I'll do a quantity of two and I get that particular shape there and then finally I'll turn my sketch back on and I want to make sure I'm extruding all of this down I think it's minus point one in this case so mine is point one and I'll say okay let's turn off our sketch now you might run into this now you'll notice that there's these edges right here now I could leave those that's totally fine I could also click on that face and hit the Delete key and notice that it basically healed that region now the only thing I can think of is that you know the curve of the circle and the curve of the slot we're just ever so slightly different maybe and so mathematically they didn't match up so it left that face but by clicking on that face and selecting delete it has to let me move this over just a little bit it has to heal so this face over here has to join up with this face over here so when I say delete you'll see it basically heals itself so you could just delete those extra faces if it happens at all and then lastly appearance will do that nylon again and we are done with our two gears and if I switch back to the to the camera here it's kind of hard to see but here's those gears that we just created right and then here's that drive gear kind of small but hopefully you can kind of see that a small hole going through the center etc so okay I covered multiple parts we did the heatsink we did a couple different kinds of gears using that FM gear plugin hopefully you found this official make sure your thumbs up if you liked it thumbs up if you didn't next week I'm gonna I think I'm going to be doing the circuit board I have to figure in the wiring we'll figure that part out again make sure you go out to our fusion 360 live YouTube channel and see all of the live streams that are happening and sign up for those if you haven't already or make sure your your online for those want to thank Jason for helping out and hope to see you on our next live stream thank you you

Channel: Autodesk Fusion 360

Views: 14,074

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

Id: BwKuMHuAC5o

Length: 76min 0sec (4560 seconds)

Published: Thu Apr 02 2020