360 LIVE: Laser Projector Build - Part 1

hello everyone and welcome to another fusion 360 tech Thursday my name is Brad talus I'm from Autodesk and this is gonna be a multi-part series I've seen some requests where people are like okay you show us how to create brackets and flagpole mounts and cardboard boxes and all that kind of stuff but what about like an actual product so I went looking around and found something that wasn't overly complicated it's one of these I actually had one of these in my front yard during Christmas but it's one of those laser light projector kind of the things and I was thinking you know this is a pretty cool product it's got some some neat fusion esque type features on it like patterns and Phillips and then what we're gonna do is we're gonna learn how to manufacture all of these parts and you'll notice it even has like a circuit board it's got those lasers in there I don't know if you can kind of see them some wiring a lot of plastic parts some injection molded parts and so I was thinking you know this might be a kind of a fun multi serious project so that's what we're gonna be doing I've got my friend Erin on the chat so if you have any questions or comments he'll be helping me out today I've also included the drawings in the description of the video and we're only going to do two parts today so I only have two drawings so far this series is going to be interjected with some other series make sure you subscribe to our channel as you saw last week there was an excellent live stream on the new electronic design that's added into Fusion and we're gonna do a couple more of those throughout the month also and we're gonna use it on this project so here's kind of like what we're gonna be doing and again this thing isn't totally finished yet but what we're gonna be working on today is creating the steak and the pivot mount on this particular design later on we're going to learn more about like you know how would you go about this plastic part and shelling it out etc we're gonna learn about reusing existing geometry to help us design the next part we're gonna learn some tips and tricks and some shortcuts which I know all of you really like so let's go ahead and dive right in so I am using these drawings and again they are linked in the description of this video and so I'm just gonna be referencing these so the first thing I do is I take a look at a drawing is I'm gonna be like what makes the most sense and I like to break it down into its simplest form so obviously we've got kind of a circular shape here and it's patterned or you can see there's multiple little support ribs here we've got this bottom stake part that's slightly tapered you can kind of see that here 91 degrees you'll notice I've added a comment that we're gonna add a very small fill it to all of the edges when complete except for the threads so you're gonna learn some tips and tricks on that this is in inches I know all of my metric people are gonna yell at me but so let's go ahead and jump right in so one of the first things I want to do is make sure that my units are correct so I expand open next to this little document settings gear and I show that we are in inches I like to do everything in components and with this particular design this is going to be really important and so again I'm going to emphasize I recommend doing components for everything that you design because it keeps track of your sketches your bodies your timeline is much easier to see and I just find it so much easier to manage you know more complex assembly so I'm going to create a new component I'm just gonna call it steak for now and so you can see that I have this new component and it's active the next thing I like to do as I like to hit save and the reason for that is it's gonna allow me to save it and it's gonna start my autosave so autosave doesn't start saving until you've saved it for the first time and then it's gonna autosave in the background so I'm just gonna give this a name I'll just call its take part and you'll see that that will go from untitled to take part okay and now it says version 1 so now my autosave has kicked in so another little tip that might help you out in the long run okay I'm gonna start again with the the basic shape so create a sketch I'll throw it on my top plane I'll use the circle or the C on my keyboard for circle and according to the drawing this is a 1.5 in diameter so I'll go ahead and do that and that's pretty much it I'll say finish sketch now here's another tip I don't know if a lot of you know about this but I could hit finish sketch and it'll exit out of my sketch environment it'll put me into my 3d environment well even inside my 2d environment I can just click on my profile right mouse click it shows me the commands that make sense and one of them is extrude so I'm gonna go ahead and say extrude and you'll notice that it basically finished my sketch for me so it just kind of saves an extra little step ok now I'm not gonna I'm not gonna jump back and forth to the drawing too much but I'm just referencing my drawing here so I'm extruding this shape up 0.1 according to the drawing and I'll say ok and this will make more sense as we go along okay so what I just basically did is I just drew this bottom disc right here it's 1.5 in diameter and you can see that there point 1 thick now I want to basically pattern I could do a copy and paste but I like to use pattern because maybe I'll come back and want to change the spacing or change the quantity so you can see that it says it's point six seven five for the spacing so I'll come in here and say create pattern and you'll notice we have three different kinds we have rectangular patterns circular or pattern on a path I could do a pattern on a path or I could even do rectangular and you're like well it's not rectangular it's in a straight line well you'll see that you don't have to do it in a full rectangle you can actually do it in a linear direction okay the important thing is you'll notice under pattern type you have different options faces bodies features and components now this is where it can get a little bit confusing what's the best method which way should I do this if I pattern components I'd have multiple bodies or multiple components and I could join them together I can also say pattern faces but then I'd have to manually select all of the faces but this features is a really powerful option and what that allows you to do is actually pick features from your timeline and pattern those so I'm gonna say features and then I'm gonna select that extrude feature and you'll notice is selected all of the faces for me okay so we're basically saying pattern the extrude that we did what's the direction I'll go ahead and specify pointing up and here you can kind of see the rectangular part well I'm gonna just start to drag up and it's only patterning in that direction I'm not gonna drag to the right and create patterns over here okay so you can see I've started to get a nice preview what that's going to look like I can specify the quantity so in this case I want to do five and then you'll also notice we have extent and we have spacing so extent would be you know it from the bottom to the it needs to be you know five inches you would say five and it would fill in in between or if you know the spacing at which we do because of the drawing I could come in here and say point six seven five and you'll see how my pattern kind of shrinks just a little bit and I now have a quantity of five then you'll notice there's little check boxes on each of these and that's this suppress and what this allows you to do is you could actually turn any of those on or off it's kind of a cool way to create you know complex patterns and then remove maybe a couple of the features out of there in this case we don't need to something's gonna go ahead and turn that off and say okay and now I have all these little disks or wafers and if I expand open my stake component and I expand open the bodies you'll notice that let me click on the down arrow you'll see I have multiple different bodies okay now we're gonna fix that here in a little bit so now what I want to do next is let's go back to the drawing I've created all of these little disks now I want to go ahead and do the thicker one on top you can see that it's a little bit thicker than the rest of them so let's jump back into fusion and I'm gonna say I want to create another extrude so I'm gonna come in here and say create extrude now it's asking for the profile so I could have created another sketch you know offset plane or something like that according to the drawing but check out this neat little tip I'm gonna expand open my sketches turn on that sketch and here's my original sketch okay so that's my original profile I'm gonna go ahead and click on that now if I were to start to extrude it's gonna start way down here in fact it's going to cut through my other geometry but check this out instead of starting at the profile plane I can come in here and say offset plane and according to the drawing it's going to be three point four or five so I'm going to type in three point four five and notice what it's doing now it's using my existing profile so I didn't have to draw another sketch or create an offset construction plane or anything like that and it's basically saying use that profile but start 3.45 away from where that plane actually is and so now we're extruding up here and I can type in the correct distance which in this case is point two in fact actually according to the drawing three point four five goes to the top so I'm going to say minus point two let me show you what I mean by that so you can see here's the three point four five goes to the top of that part and so we're basically putting a profile plane there and then extruding down point two okay so I'll say okay I get another body that's added in there so the next thing let's look at the drawing again one more time let's go ahead and put these ribs in here okay now as I was messing around with this and trying things out I tried using the web command and the rib command which we have in here but neither of them worked in this case and the reason for that is typically you'll notice for example like the web it's looking for like an interior void like a shelled object for example and and rib is looking for a single part and here I've got multiple parts and when I did get it to work they actually had square corners and they didn't follow the shape of this circle so I ended up having to actually draw a profile which is fine and I want to reuse my existing sketch so here's something kind of interesting I don't do this all that often but there's some really powerful commands in here my sketches at the very beginning in time and we've done some downstream processes but remember my sketch it only was a circle well I'm gonna go back and edit that very first sketch and let's just draw some lines on here so I'm gonna I'm gonna purposely draw off to the side like so and purposely draw to the side like so okay then I can come in and say I want that line to be coincident with that point and I want that line to be coincident with that point and you'll notice they turned from blue to black which means they're fully constrained and then I don't want them to be object lines so I'm gonna select them and turn them to construction so I'll go ahead and click on construction and you can see now they're like light pencil lines okay I want to basically create that web looking shape it's basically looks like a big plus so instead of drawing a bunch of lines I'm gonna use the offset command so I could click this existing line and I want to offset that point zero five okay because it's gonna be point one for the total width so I said point zero five I'll do the same thing here I'll say mine is point zero five and you'll notice that it's created those lines I'll do that again I'll do an offset here I'll say 0.5 sorry point zero five and I don't know if you saw that little trick that I just did here I'm just right clicking and dragging straight up and it's gonna repeat the last command that I'm doing so if I right mouse click you'll see this blue radar we call this our marking menu and you'll notice if I drag straight up it's repeat the last command in this case it was repeat the offset so if I just right click and drag straight up it's gonna repeat my last command so it's fast away instead of having to go into the menu or anything like that sorry - point zero five say okay and now you'll notice that I have these black lines now I could come in and trim these little segments out of here but there's no need to and like I showed before I can actually select my profiles in here all right pre select them then I'm going to right mouse click and say extrude and it brings me into my 3d workspace but in this case you'll notice it's not showing any geometry right now why is that well look where we are in time we're at the very first step we actually haven't extruded our part yet so going back in time kind of messing around with your timeline is really powerful but it can also be a little bit confusing so why are we not seeing it so in that example I don't want to pre-selected my sketch I'm gonna say finish sketch now I can see my all my parts but I can also see my sketch so now I'll select it because we're at the end of end of our time line right there so I'll go ahead and click these guys here right mouse click I love the right mouse click it shows me the commands that make sense in this case extrude and I'll start to drag to kind of give it its shape and now you'll notice it's wanting to cut that away we'll fix that here in a minute I want it to go all the way up to this face so again instead of typing in a dimension I can just click on that face and it's gonna extrude the correct distance now obviously we don't want to cut through I want to say join and here's where the magic happens watch what happens to all my bodies over here so I took my profile I said extrude I'll say ok and it's all one Adie now because they joined them all together and also notice how nice you know this this web basically is nice and curved it kind of joins with all those little disks and that's why I ended up drawing the profile okay I'll turn off that sketch down there I don't mean to see it right now but you can see pretty quickly we created what looks like a complex part using just a couple commands what I might do now is I'm still kind of working on this webbed area right here so the next thing I want to do it's kind of hard to see and that's why I did the two views here there's some added material in here to add some strength for the hole and the and the threads that are going to go in there so the next thing I'm going to do is basically draw that profile and you can see that it's one point three in diameter in that case okay according to the drawing so I'll go ahead maybe I'll create a sketch on this top face do a circle type in the diameter of one point zero three I'll finish my sketch and let's go ahead and extrude this so I'll start to extrude down now you'll notice I didn't put the hole or anything like that in there and again because it's cutting into the geometry it thinks you want to removed or cut away material but in this case we actually want to join material and I want to do the point zero nine the core I'm sorry point nine so I'll say minus point nine and you can see how that extrudes down okay and again I'm gonna join that together I'll go ahead and reuse that sketch so I'm gonna go ahead and double click on that sketch and what I want to do now is add this little peak I think it's kind of like an alignment arrow that lets you like point the laser in the correct direction so you'll notice I basically all I did was give you the distance from the bottom of the circle to the tip of the peak no angles or anything like that so let's see how we can go about making that guy so what I'm going to do here is draw a line again kind of from the bottom and I'm just gonna randomly pick some distance I'm just going to click up there and say okay okay now I like to draw off to the side that way I can physically see the changes happen so when I come in here and say I want this line to be coincident with that point I can physically see it move over I can physically see that it went from unconstrained to constrained okay then I'll come in here and do a line now we've shared this tip in the past if you get near a circle and then you click and hold it actually creates a tangent constraint for you automatically and you can kind of see that icon at the end of my line it's stayin stuck to the circle and then I'm just gonna go to that point I'll do the same thing over here I'm just gonna click and hold it's gonna create a tangent constraint for me and then I'll just go to that point so there's my peak now all I have to do let's throw a dimension on here I'll grab that line and that line is supposed to be one point seven and watch what happens to the peak you'll notice that the lines still stay tangent because they were constrained to be tangent and the length is now one point seven okay and notice now they because I've thrown a dimension on there they're fully constrained whereas before they weren't because I could have changed that where that peak location was but by adding the dimension it did and strain it okay also pre-select these guys I'll say extrude and start to drag down and you can kind of see it's adding that geometry again how far all I have to do is just click on a face and it snaps the correct distance I use that snap to a face all the time like if I were to click there you'll see it's gonna snap to that face so it's a really powerful tip I'll say okay and I'll go ahead and turn that sketch off now here's another tip when I'm helping out customers and stuff like that I might say turn off your sketch they end up turning off the sketch here and that does work but then when you go to create another sketch you'll get that visibility warning or whatever so I usually turn off the individual sketch and leave my sketches turned on okay okay so now the next thing we want to do is put that threaded hole and I'm gonna use the hole command to do that so or the h4 shortcut you'll also notice that we have a thread command that is more for like bosses or existing holes I'm going to use the whole command and they've added some thread stuff in there so for example you can kind of see I've got simple counterbore countersink I've got simple tap types simple clearance tapped etc taper tapped thread offsets everything it's really kind of cool so I'm just gonna go ahead and pick a point a random point okay now in this case I have a really small circle and according to the drawing it's an actual 3/4 by 12 so instead of having to look things up I'm actually going to click on this tapped and notice what it gives me it actually allows me to pick threads so you can see Acme screw threads ANSI metric gia dinh JIS ISO etc so I'm gonna do the unified screw threads the designation are the size I'm sorry I'm going to do a 3/4 so 0.75 okay and it gives me a live preview what that's gonna look like then I also want it to be 3/4 12:00 so I'm gonna come in here and say 3/4 12:00 but you'll notice it's in the wrong location so I'm gonna grab that little round dot and you'll notice I'm gonna move away there's two dots on the screen right there and all I have to do is get near that bottom dot and that bottom dot is the center of this circle the other one was the center of the face because we have this little peak here that's why you saw that second dot but it automatically caught to the center for me I didn't have to add any dimensions or references or anything like that ok then lastly you'll notice it says modeled if I click on modeled it'll actually physically model that now again this is personal preference you know if you're gonna 3d print it you might want it modeled if you just want it as a reference you could leave it and it's almost like a sticker or a decal to make things more interesting I'm gonna do modeled now I also want it to be countersunk or counterbored I should say so I'm gonna say counterbore and here you can see I can type in what the diameter of my counterbore is and again according to the drawing and fortunately I already had it filled in but it's point eight and then I can specify the depth so for example if I say point 1 you can see that it's gonna counter bore down point 1 and according to the drawing of the counterbore is point 2 9 deep so you can kind of see it's going to create a counterbore and then start those threads so it's a really easy and fast way to create complicated geometry I'll just go ahead and say okay so you can kind of see the final product but what that's gonna allow it to do is allow the other part to screw in and basically you know seat at this particular height for example before it bottoms out into the bottom of the part and you'll notice that it created a feature in the timeline so I can always come back and make changes to this if I needed to okay we are moving along we're doing pretty good here I'll go back to my drawing real quick so I've pretty much finished everything that has to do with this top part the next thing I want to do is create the steak part okay now it's thicknesses are the exact same as the the ribs up here so I want to reuse as much information as possible so let's go back and turn on our original sketch one and there's the correct width but I need to add some more geometry to this so again I'm gonna go all the way back in time double click on my original sketch and I'll just create another circle in here in this case it's a one-inch diameter I'm gonna say finish sketch now you'll notice by adding that circle it didn't affect any of my downstream processes because we didn't use that circle to create any of this geometry but now I have the ability to come in and say I want to select these regions and you'll notice that it's basically defined by that one inch circle that we just added so I'm gonna go ahead and grab I might have to zoom up here all of these areas like so I'll right-click and say extrude and I'll start to drag down and it gives me a live preview of what that's gonna look like so again using the exact same sketch I started out with so he just speeds things up yes I could have created another sketch I could have drawn more geometry I could have reprojection a tree but there's no need to okay I need to set the correct distance and again according to the drawing it's four point six to five in the negative direction six to five whoops six to five okay so there I'm getting my steak well it needs to be tapered one degree and you'll notice in my extrude I have this taper angle so I'm going to type in one and you'll notice oops it extruder to tapered the wrong direction so I'm going to say minus one but watch what happens I don't get the result that I expected or want it's actually tapering every single face so yes it's doing the angled faces there but it's also tapering you know these little webbed faces so I can't really do a taper angle in my extrude also again personal preference I personally don't like doing tapers in the extrude because if I want to change it I have to remember I did it in the extrude so instead we're gonna use the draft command and I like to use the draft command because then it shows up as a feature in the timeline so everything is good here we're gonna join that together I'll turn off that sketch so I don't need it anymore then I'll come in here and say draft under the modify menu so it's asking for a plane and what this is basically saying is where are the angles gonna hinge around so I'm going to pick on this plane and you can kind of think of each of these edges having a hinge and the face is going to rotate around that hinge basically so that's our draft plane and now it's asking for the faces and that can be very specific I can say I only want these outside faces and again I like to pick through I'm just gonna click and hold to grab that hidden face I'm gonna click and hold to grab that hidden face I don't have to rotate around let's take a look at it kind of from the side here Oh already sorry it would look like this you know I've selected the faces and now that can come in and add my draft angle so for example if I say to you can see how those are drafted to degrees but the ribs are staying the same thickness which is what we want in this case according to the drawing we want one degree and I'll say okay so we just added some draft to the design okay according to the drawing we want to kind of sharpen the point so a 70 degree by a distance so I'm gonna use the chamfer command let the software do the hard work so I can come in here and say I'll click that edge and I'll say chamfer and by default that's usually set to equal distance and what that does is it does a 45 degree so I'm gonna go ahead and select all four of these and maybe you know that's what we want but according to the drawing we want it to be a little bit more steep so I'm gonna do distance and an angle because that's what the drawing gave me so let's do I'm gonna do a smaller distance let's just do a point one and then let's do a steeper angle let's do the 70 degrees 70 degrees and now you can see the steeper angle okay and as we start to drag this in you can see what that's going to look like now if we go too far you can see that it errors out because it's basically destroying geometry you can't physically do that so I picked a dimension of point eight three four six and you can see that's about as close as we can get to a sharp point and I'll say okay and we now have the start point okay the last thing I want to do now is according to the drawing we've we've added the start point there we've got the threads the counterbore everything like that so there really we're done with the design except for add the point zero one fill it's to all edges when complete except for the threads okay so I'm gonna jump back into fusion and if I were to say fill it draw a box around everything it would also select all of these edges inside of here and we don't want it to do that so what I can do is here's my whole feature I'm gonna right click on it and say suppress features and you'll notice it didn't remove it or delete it or any like that it's still in my timeline but it's kind of grayed out and you'll notice that the hole doesn't exist anymore then I'm going to come in and say fill it I'll draw a box around everything it's asking for the size so I'm going to say point zero one and this is really cool because really quickly it's selected all of the faces all of the edges and you can see that it's doing these really nice fill it's on all of those edges except for the threads right so I'm going to go ahead and say okay and instead of having to manually select all of those individual edges and a lot kind of stuff I just basically drew a selection box around the whole thing and you can see how we've knocked all the sharp edges in fact if i zoom up here notice the nice-looking you know five Phillips coming into one I think that's really cool-looking we fill it in and not to all the sharp edges off this part now I'm going to go back and unsuppressed the whole and let's take a look at what happens here okay I'm gonna zoom up and you'll notice that the threads are not fileted but you'll notice that the top of the hole is and you might be saying well I thought you turned that off when you suppress the hole and sure enough I did but when I did the Phillip command and I drew a box around everything in fact let me go ahead and edit that fill it again edit that guy you'll notice it says 113 faces and also 272 edges so by selecting this face it's gonna grab all of the edges necessary to fill it that face okay notice where it is in time it's the last thing we unsuppressed the hole so now there's a hole in there it goes and does the next few steps and now it gets to this fill it it says oh I have to fill it all of the edges that have to do with that face and so it actually fill it at the top of that hole for me so that's why you see that edge fileted but it didn't fill it these because these weren't part of the selection hopefully that makes sense but it's I think it's a really cool feature okay so we are done so I'm gonna go ahead and hit save and it's gonna go from version one to version two I could have typed in you know final design or whatever another thing I like to do instead of kind of this plain gray I hit a for appearance and you'll have all of your appearances here now I messed around with a particular appearance to get it the way I liked and so I added it to my favorites so if I click on favorites you can see like here's my cardboard material and then here's my random textured plastic so I'm just going to drag and drop that on there and if we zoom up sure enough you can see it looks kind of like molded or injection molded plastic so how did I do that well you just you know pick a particular material you edit that material to whatever you want let's say I change the color then I can right mouse click and say add to favorites so really quick way to reuse you know because we're gonna use this color for the rest of the parts okay um I never know how long things are gonna take so we've got about 20 minutes left and I could either stop now and we do this next part the next time or I could start on this part which I think I'm going to do we might go a little bit long so I apologize I never know how long these are gonna take so hopefully you all can last a little bit longer than an hour this looks pretty complicated but it's pretty similar to what we did on the last part so I'm going to go through creating these ribs a little bit faster so but there's some cool tips and tricks you're going to learn with this particular design okay yeah and if you guys can't hang on for a little bit longer than an hour this is gonna be out on YouTube so okay so I started a new design and again first thing I'm going to do create a new component I'm gonna call this pivot pivot base I'll go ahead and save my design so my autosave is working and I'm gonna do the exact same thing I did last time create a circle that's the correct size now here's where the cool thing comes in it's the exact same size and shape of my previous part that I just designed I would love to reuse that but you'll notice I'm in a new design check this out I'm gonna go back to my stake part I'm gonna edit that sketch draw a selection box around it and I'm gonna do a ctrl C for copy okay or I can right mouse click and say copy then I'm going to jump over to my pivot base I'm in this sketch I'm gonna whoops right click and say paste and boom I brought this sketch from a totally different design into here and it's got everything that I need okay it's got my crosshairs it's got the outside diameter so I'm gonna go ahead and say okay and now you'll notice I'd have to select a lot of these interior things to extrude I want to extrude basically the whole shape so instead I'm just going to draw a box around the whole thing and say extrude and it's gonna grab all those profiles for me and it's basically gonna create that disc for me so point one I'll say okay that's part of my sketches right here right there I turn that back on I can still see it so I was able to reuse existing geometry and I hope everybody liked that so if you liked it throw a thumbs up out there I try and come up with new tips and tricks of the speed up your design so hopefully that helps yeah okay pretty much the same thing I did last time I'm going to come in here and say pattern I want to make sure features I want to extrude or I'm sorry I want to pattern that extrude feature tell it which direction pointing up tell it what the spacing is and in this case the spacing is actually a little bit different it's 0.5 and I only need to do 3 for the quantity I'll turn my sketch back on I think you guys see where this is going so I'm just gonna go ahead and select these profiles again okay I'll say extrude I like to start to drag to kind of get a preview and then it lets me snap to that underside of that face and we're gonna obviously join that together and I'll say okay okay now I'm gonna go ahead and edit the sketch one more time and I need to make sure I'm like correct drawing here sorry guys okay um what I want to do here is I don't need this circle in this design so I'm gonna go ahead and delete it and I'm going to create a 3/4 or 0.75 inch circle and I'm gonna use that now again I could draw a selection box like so and it's gonna select all of those profiles for me and I can say extrude so I didn't have to manually click in all these little individual profiles you know there's like probably what 8 or 10 of those in there so okay I'm gonna extrude this down this is where we're gonna do the threads and this is where you're gonna see the thread command come into play so I basically create this boss like so but then I want to thread it according to the drawing so basically we're gonna be creating this region right here actually this should show you really quickly but back to the drawing you'll notice that the threads do not go the full length so I extruded 0.75 but you'll notice this is a 3/4 12 but the threads are only 0.65 okay so I'm gonna come in here and say create thread I'll click on the faces that I want to thread we're gonna say it's gonna be modeled because that's cooler looking but then you'll notice it says full length I'm going to turn off full-length and now I get the option to just to define how tall the threads go okay so for the length it's supposed to be 0.65 so you'll notice it's going to go point six five up and then stop it's gonna be the three-quarter 12 because that's what the other one was I'm gonna say three-quarter 12 ANSI UN and everything else there looks good and I'll say okay so we've just threaded that part okay I know I'm kind of going pretty good pace here but then I did the exact same thing with this design that I did with the last design I kind of broke it down into its simplest forms so the first part was basically this webbed area here and I'm gonna say the second part is kind of this you know plastic area up here and so I broke it down into its simplest form so what I'm gonna do now is draw this area okay now here's another cool trick what I want to do is I don't have to draw another sketch I just want to reuse this particular shape and I want to extrude it up so I'm gonna start to extrude but you'll notice that it's joining it to the existing part and I don't want it to be joined I kind of want to work on this part as like a separate entity until I'm ready to join it so I'm gonna come in here and say I don't want that to be a new body okay and the overall height according to the drawing is 1.7 so watch what happens over here when I say okay I now have two separate bodies but I used the information from body 1 to create this other body so again didn't have to create a sketch I'm going to round over the top because it's base Klee you can kind of see their radius of 0.75 so let's go ahead and jump back to fusion I'm gonna go ahead and select that and say fill it now how big do I need it to be well I could type in point seven five or check this out and then I say measure okay then I'm gonna click on this edge and it figured out what the radius was of that edge and filled it in for me automatically again I could have typed it in but instead I let fusion do the hard work I might have accidentally typed in you know 0.76 or something like that or whatever so kind of neat little tip I like that one okay now obviously this part looks like it's kind of like a split in half and we don't even need half of it so I'm gonna use the split command because this is all one shape okay so I'm gonna come under here under modify inspect it's a split body what's the body now because we didn't join them together this is a totally separate body what's my splitting tool I'm just gonna go ahead and click one of these planes now you'll notice they're buried so here's another trick if you zoom out you can actually click on it right or you can click and hold and select it in there so you can see it's gonna basically split that body right in half I'll say okay and now I have three bodies we don't need body five so I'm gonna right mouse click on it and say remove please don't use delete in fact I I wish that we didn't have this command obviously it's in there for a reason but what remove does is it removes it out of our design but you'll notice it added a feature into the timeline that we said hey we removed that body if I had said delete it would have physically deleted that model but if that model was used for creating other sketches or lining things up and you said delete all of your downstream processes could fail and/or get warnings and errors and it's such a mess to deal with so always always always use remove if you can okay so I now have you know half of this body there and I'm gonna take a look at the drawing real quick we're actually doing pretty good on time we've actually might believe it or not might finish this at the top of the hour what I wanted to do now is I'm kind of again working on this top half and there's this little standoff where a threaded thumb screw is going to go into so you don't want a thumb screw into a curved surface so they added this little standoff there so you can kind of see it's a radius of point I'm sorry a diameter of point eight a diameter of point two five going through and it's just basically at the same plane as the outside edge so I'm going to need to create a sketch that's over here somewhere and I don't have a flat plane there there's one here but I have to know the exact distance and a lot kind of stuff and I'm bad at math so we don't want to do that so I'm gonna come in here to the I'm sorry construct a menu and there's a cool command in here called tangent plane I'm just gonna go ahead and pick on that face and you'll see that it's actually going to put a construction plane on that face at whatever degree I want it to be at and it's gonna stay tangent to that surface okay really powerful construction plane now in this case I want it to stay at zero but it's exactly at the edge of that this surface right here it's touching it it's tangent to it now I can create my sketch again I like to draw things kind of off-center a little bit and watch it go into place so I'm gonna say 0.25 I'll repeat my last command and this one is 0.8 I remember correctly okay then I can throw some dimensions on here now according to the drawing those holes are located off the bottom of this part right here so I'm going to click there and I'll click there place my dimension and it's supposed to be two point zero five up so I can see that that moved up and I want it to be in line with this point right there so I'm going to kind of drag this across a little bit to get it maybe a little bit closer and I could say I want that point and that point to be vertical with each other so I didn't even have to throw a dimension on there I just said this has to be centered right and now you'll notice this fully constrained I'll click on that face I'll say extrude I'll start to drag and I'll click on that face for it to go the correct distance okay now you'll notice I only did the small hole because I obviously couldn't do that the large one that's the same time and it went away but all I have to do is turn that sketch back on and now you can kind of see why I keep my sketches folder opened up I could just get to these really quick now I'll click on that profile I'll say extrude but as I start to extrude it's instantly cutting into my geometry and I want it to be an actual extrude and how far do I need to go well here's another neat little tip I'm gonna say instead of distance I'm going to say to object what's the object I'm going to pick this curb surface so it's going to go as far as it needs to go to touch that surface and there you see sure enough it is and instead of a cut we want to say join and so I get that result there it's taking that profile and extruding it as far as it needs to go to physically touch that heart and we're gonna join it together where we are okay let's turn off my sketch still working on this upper area here the next thing I want to do is I want to shell it out so I'm gonna go ahead and click on this face right mouse click and shell is one of the options I can do so I'm gonna say shell and I like to start to drag to kind of see what that looks like okay now I see an issue notice that it's also shelling right here I actually don't want that face to be there so I need to add in that bottom face right there so I'm gonna select it and now watch what's happening in fact if I were to turn off body one you can kind of see it's now shelling not only into the part this direction it's shelling into the part from the bottom also so in this example I did have to select two different faces to shovel this part out and we're gonna go point one and I love our shell command I mean notice because we put the hole through there already it's adding this automatic boss around there for me which is kind of cool so let's go ahead and do that okay hopefully Aaron's having fun with all the chat and people learning things so the next thing I want to do is start working on all these teeth okay and you'll notice I give some some details here the angle of the teeth and how many they're evenly spaced you'll see some diameter 1.5 1.3 in there so let's go ahead and create a sketch on that face and I'm going to draw a circle that touches and you'll notice it's snapped to that circle there and I'm going to grab and snap to that circle there also okay now I'm going to draw just one tooth so I need I need some information here so I'm just going to draw a line like so construction line then I'm just going to come in and draw an angled line that touches this outside circle so I'll go there and there you know again I over exaggerate now I can come in and add a dimension so from that line to that line that's supposed to be one point nine one degrees and watch what happens to my line it it updates it moves it turns black which means it's constrained and then I need to do a dimension between that two line I could mirror it but I gave the dimension of three point eight two degrees and so you can see that comes back also and it's fully constrained okay I'm going to say finish sketch in this case and I need to extend this profile into the part now you'll notice yes I drew these circles but then I also drew this tooth because I'm gonna come back and use that tooth a little bit later but I put it both on one sketch because they're kind of similar they're kind of defined on the same thing so instead again of having multiple sketches in my time line I'm trying to keep it as simple as possible so I'll come in here and say extrude I'll start to drag backwards now you can see it's wanting to cut into there well we're gonna say join and how far we're gonna say to object I'm just going to go ahead and click on that curved surface there and kind of hard to see with all the blue but it actually extruded all the way back to that back surface I'll turn that sketch back on I'll zoom up here and I'm going to go ahead and extrude the tooth now it this is a really kind of a tiny tooth and so the distance is point zero one so you can kind of see that now again you might ask about you know this could I do this taper angle 45 actually - 45 to create the the peak and you'll notice that it actually doesn't go to a sharp edge so let's try - 60 or something like that but the issue is it's tapering down the top and the bottom also and I don't want it to do that I want it to be straight out so again I'm not going to use the taper angle in this case I'm just going to go ahead and extrude straight out point zero one then I'm going to create a chamfer so I'll say chamfer let's go ahead and do both of these edges and in this case instead of distance at an angle I'm gonna say two distances and what this allows you to do is to basically specify two different distances and I'm gonna go ahead and grab these arrows so you can kind of start to see what's going on here okay so for this for this distance here let me change this so I can see yeah that's the the bottom one I know that that's gonna be 0.1 I'm sorry point oh one in depth right because that's how thick my tooth was so that's that distance then this other distance you can kind of see as I'm going down because this is a tapered tooth you'll see that's gonna leave a little bit of a sliver and if I go too far it basically errors out so I'm gonna go to a very specific distance okay like in this case I could say point zero two five or I could say point zero two four and you'll see it leaves a little bit of a face there but that's okay let's just get it as small as we can I'll just say okay like that and I just created one tooth hi now I there's again multiple ways I could have created this I could have done a profile and swept it along a path I'm not saying this is the only way to do this okay we're getting pretty close we're gonna go a little bit over but hopefully you guys can hang on so okay obviously I drew one I'm going to reuse that let's say create pattern circular pattern again I want to make sure I'm doing features and I'm going to do the extrude feature and the champ for feature at the same time what's my axis I'll probably just click maybe like the cylinder here what's the quantity well in this case it's actually 46 and you'll see it gives me a preview what that's gonna look like and once again I'm probably not gonna suppress any of these I'm just gonna turn that off just to kind of speed things up and I'll just say okay and instantly we have all of these little grooves teeth by using a pattern very very fast way of doing it let's look at the drawing so we've created that honestly all that looks left to do is these little webs that are in here and you'll notice that they're recessed back a little bit that's kind of why I did this detail it's kind of hard to see in the shaded view so it's recessed back and I know I gave a dimension not sure exactly where I'll have to review my drawing I might have to re-up load my drawing okay so let me jump back in here I'm going to create an offset plane and it's minus 0.1 and I think it is on the drawing I just a little bit rushed I don't want to have to hunt it down so you'll notice my plane is kind of small if you get near the corner you can actually drag the planes to be bigger so if I just grab the corner I can make that plane bigger if I want to you don't have to it's not necessary but if it's just something you want to make a little bit bigger you can just grab the corners so I'm going to create a sketch I'm going to draw my lines now I'm just gonna kind of draw a line like this now you'll notice that I have to hit this checkbox and then I can come over here and draw a line and if I don't hit that checkbox it's wanting to continue this line well here's where that marking menu comes back into play notice at three o'clock it says okay okay so check this out I've drawn my line I'm just going to drag to the right and I'm said okay I'm finished with that that line so same thing here I'm just gonna draw a line drag to the right and I'm out of that I don't have to hit that green checkbox every single time okay I just drag to the right and we're done I'll do the same thing here I'm in again I don't know where these lines have to be I'm just kind of drawing where I think they should be and then we'll come back and fix this in a little bit okay notice these lines are blue they're not fully constrained but if I came in here and said horizontal vertical and went that point to be horizontal vertical at that point you can see that I'm now constraining these lines because if I didn't I can move these around right yep they're nice and vertical but I want them to be in line with that center point so that's why I'm adding in these constraints like so okay okay on down here there are some dimensions so I'm going to say dimension right here so maybe I'll click that center point I'll click this line and according to the drawing that's supposed to be point one seven five 0.175 and you see they've kind of went up a little bit that's okay I'll do the same thing here Rock sorry I'll do a dimension from here to here and that's supposed to be point two two five according to the drawing now it did move these so I'm going to move them back because we're going to use the web command and I don't want them to be in the correct location kind of in this void I'm going to move that guy down I'm gonna move this guy down and now I have these dimensioned I want them over here so we'll do the mirror command that line and that line and I could just pick for example that line there cuz it's right down the center and I'm gonna mirror that over I went through that pretty quick hopefully you all understand sketching and adding constraints and having a fully constrained sketch so if you need to review that you can always where you rewind the video so I basically have these weird line segments kind of floating in space here is where the web command really shines okay so I'm gonna say web and I'm gonna go ahead and click on that line and notice what it did I mean it's even going back into this little recess and everything like that think about how complicated I have to do some weird extrusions and they probably come out through the back of the park so this web command is extremely useful the key thing is this extend curves if I had that turned off it's only gonna do the length of the line that I drew but because I have extend curves it's going to extend as far as it can so I'm going to go ahead and select all four of these and we now have those webs in there okay now I'm gonna click on this line but watch what happens when I try and add that in you'll see it says the curve you're trying to select is an intersecting blah blah blah and that's because of this extend curves so I'm gonna have to do these four lines separately so I'm going to do these up here I'm gonna say okay turn my sketch back on create a web now I can click on that line and of course it's complaining and I'm not sure why that's interesting let me say - next Wow okay that usually works not sure why it's not in this case Oh huh I dunno why I just figured this out okay so it says it does not insect intersect with a solid body guess what this is a separate body in fact if I were to turn that off it says hey I'm trying to intersect but nothing exists so I am happy with how this looks so I'm not coming here and combine that body with that body we want to join them together and I don't need to keep the tool I just basically want to join these two bodies together I'll say okay and now we can see that that's all one body and if I were to come in and say web now it's happier I was like what am I doing wrong here okay so now it has you know it can go up to this curved surface it can come down to this flat surface and there we go okay I'll turn off my sketch and we are pretty much done with the design the last thing on the drawing is ad fill its to all the edges when complete except for the threads and the teeth okay throw a little bit of a curveball in here so I'm gonna do the exact same thing I want to add that fill it so I'm going to actually let me do these bigger Phillips first so I'm gonna click on that edge and say point zero five and I'll do that edge also and I get that really cool Filat that's kind of joining onto a curved surface looks really nice okay so now I want to do all my little tiny fill it's like I kind of go from big to small that's why I did those first obviously I don't want to do the teeth so I'm going to come in here and suppress those features including the extrude let me suppress that guy so now I have that simplified model I could suppress the threads but I don't need to in this case in fact you'll see if I come in here and say fill it I'm just going to draw a selection box that does not go down below those threads I'm going to just go to there we'll do the point zero five I'm sorry point zero one in this case okay and there it's filling all of those edges I'm gonna go ahead and say okay you'll notice it didn't select my thread so I could have suppressed my threads but in this case I didn't need to now I'll unsuppressed these guys I'll come in and say unsuppressed but watch what happens my Filat errors out I get a warning message and it says error and you'll notice that none of these Phillips showed up and this is red okay this happens all the time with customer I'm helping out with nobody why did this not work well in this case it's because there's all those little teeth and there's all these little edges that that were selected and now they're kind of like overlapped by these teeth so we actually need to change the order of when we're gonna put those fill it's on so I'm gonna come in here and let's just delete that fill it well I want to fill it all of these ribs and stuff like that they're in here so what I really want to do is maybe I want to move the teeth to the end of the timeline so I'm gonna select the extrude the chamfer and the pattern I'm just gonna click and drag to the end of my timeline and now notice there's my extrude my chamfer and my pattern at the end of the timeline okay they're actually created after we've created these ribs and a lot kind of stuff then what I can do is I'm going to drag my timeline before all of these teeth happen we'll do our fill it again just go in a box to kind of select what I want I'll do the point zero one I'll say okay so these Phillips were added at this point in time then we add the extrude the chamfer in the pattern so I'm going to go to the end of time and look what happened the teeth worked and my fill it's worked pretty cool however be careful okay we've kind of changed the recipe so I'm going to do some investigation you'll notice that I into introduced an error here so I'm gonna zoom up on my teeth and those look pretty good but if I take a look that there's there's a now a fill it on this edge and those teeth overlap that fill it now they used to go to a sharp edge right this this edge used to be sharp and it used to go right to here but now we fill it'ld that edge and then we did the extrude and then we did the pattern and so these are basically floating off of that fill it well that's actually easy enough to fix I could come into the extrude actually let me let me zoom up on the actual tooth up here just so you can kind of see what's going on here okay so I'm going to edit that extrude and instead of going just one direction let's have it go symmetrically both directions and you can see it's gonna go point one that way it's gonna go point one that way I'll say okay it'll do all of my downstream processes and now those teeth actually extend back to this edge which is what we want and you can see simple fix for a complicated problem a for appearance go to my favorites we'll drag that plastic texture on there and we are done I will say save I'll call this final so I do appreciate you guys hanging the extra 15 minutes I never know how long these take well you know when I practice them and stuff like that versus doing them live hopefully you found both of these parts beneficial you learn some tips and tricks I'm going to continue reverse engineering all the parts in this thing we're gonna probably do the body next and then we'll do some of the internals like some of the mounts the lasers the circuit board etc so keep an eye out on our live stream channel make sure you like and subscribe that way you're notified when these other live streams are happening we have a lot of cool stuff happening in fusion right now with all the electrical design we're actually doing live streams on Tuesdays and on Thursdays on some of these topics so definitely make sure you take a look at our channel Aaron again thanks for your help and I hope all of you have a wonderful rest of your day and happy fusion aim you

Channel: Autodesk Fusion 360

Views: 17,739

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: zeLAAkOQaFA

Length: 78min 2sec (4682 seconds)

Published: Thu Feb 06 2020