360 LIVE: Laser Projector Build - Part 2

hello everyone Brad Tallis from Autodesk want to welcome you to another fusion 360 Tech Thursday we're gonna be continuing this multi-part series where we're gonna be learning how to model a multi-part assembly and in this case it's one of these Christmas laser projectors today we're going to learn about doing the front and the back piece and then next week we'll focus on the middle before I get started I have Angelo as my wingman today he's helping me out so be nice to him otherwise he won't help me out anymore so thanks Angelo and I'm actually gonna start out by I was looking at some of the comments you know in the previous livestream that we did and Mike be made a really good point and I wanted to share his observation with you he was going through and modeling the steak and then when it came to the point where we added all of the Philips to all of the edges he was having a problem that arose and unfortunately this is my fault I have some settings setup and unfortunately I didn't share that with all of you so thank you Mike B for bringing this to my attention let me show you what happened so he came in here to do the Phil it do the Box around the whole you know assembly or whatever the whole part and then set the size to be point zero one but I'm not gonna do it right now but it's gonna fail in fact you see couldn't be created now why is that you know I when I did it my demo it worked perfectly right and you know somebody else goes to do it and unfortunately it doesn't work perfectly so here's here's the reason why if I rotate to the back side you'll notice that it didn't select all of the edges in fusion is trying to create all of these Philips that join together and all that kind of stuff but why did it not select those in the back and the reason for that is in the select menu under selection filters there is an option called to select through and I personally have this turned on all the time what that means is it'll select all of the edges even if they're hidden or behind so for example let me do that again I'll draw a box around this I'll type in the point zero one and if I rotate you'll see in fact at the preview update it it actually selected through my design through my model and grabbed all of those edges so Mike you get a gold star for the day thanks for bringing that to my attention it's little things like this where I've been using it for so long that I'm just used to it working that way I'll also give a shout-out to Steve Smith he posted a picture of the project that he did out on the fusion 360 Facebook group I loved seeing those things so if you're proud of what you're doing post it out there I love to see all of you getting something out of these live streams so ok I'm gonna jump back to my camera here real quick this this part is actually fairly complex and I've uploaded it's in the description of the video I have created a link with all of the decals that we're gonna be using all of the imported models and I even included my outline I actually do create an outline and I put this in there now it's kind of worded more for me so you'll have to think like I do but feel free to download that outline also and step through it you know watch the video and then maybe you go through the outline and I talked about you know offset this face you know create these dimensions etc so all of that information is in the description of this video ok let's dive right in ok so the first thing I'm going to do is we're recruiting the case you know this whole thing right here and again the wing I'm creating it I'm not saying this is the perfect way or the exact way you should do it I'm gonna be showing some tips and tricks with this and what we're gonna do is we're gonna create the main body almost like a skeleton and then break that down into smaller pieces so I'm gonna start out very first thing I'm going to do is create a new component and I gotta call it case I think would be a good good word for this because it's kind of like the case and then I'm gonna go ahead and save my design and I'll just call this new case or something so it's being saved and you'll see that that will go from untitled to new case okay then we'll create a sketch that kind of defines the overall shape of the body and to do that I'm gonna create a fit point spline but I don't want to use some exact measurements so I'm just gonna quickly kind of mock things up I'm just gonna draw a couple quick lines purposely making them a little bit different size I'm not lined up again you'll see why here in a second I'll do something like that okay and what we're gonna basically do is create a spline that connects these three points but obviously I want to dimension this I want these lines to be the correct height and length so I'm going to say I want those lines to be horizontal or those points actually say to be on the same plane like so okay and then I can create my fit point spline so I'm going to click one point another point and then the third point now when you're creating a fit point spline you need to make sure that when you're done you hit this little green check box okay and notice these green handles these are your tangency and weight handle so you'll notice that it's trying to follow the spline and so it's a little bit more horizontal right here goes through that point and then it angles down through that point there okay now I can come in and start to dimension these so I don't want this guy to be 1.75 and you'll notice that you know some of the stuff will update as I'm going through here but watch what happens to the spline as I'm updating so I'm gonna say 2.25 for that one and then 1.5 for this guy here and you can see how sure enough that spline updated and then finally I'll add some locations some dimensions where these are supposed to be 2.5 and then one right here of 6.75 and now you'll notice that everything has went from blue to black meaning it's fully constrained now I'm going to jump to the drawing really quick this is also included in the description and so basically what I did right here is this is exactly what I just created so you'll see here's my first line here's my second line here's my third line there's the fit point spline and everything's dimensions so these are the dimensions I'm using to create what I just made okay in fact you'll notice that these drawings aren't fully detailed they're they're dimension just enough to get you to be able to create the parts using the outline that I've created for you so you know this one obviously has a lot more dimensions in it but what's neat about this is Fusion actually kind of solves the problem for us as we're going through it kind of fills in the blanks so you might say well that's not fully dimension well it doesn't really need to be in this particular case okay so now I'm going to just add let me add some more geometry here I'm just gonna maybe draw a line over and down a little bit like so and across so I get a you know a finished profile well you'll notice these lines are blue so I need to finish constraining those so let me throw a dimension of point five and a dimension here of 0.5 so this is the basic shape of the the main body okay I'll go ahead and select those two profiles and I'm gonna revolve around I could have done a loft with multiple profiles but in this case I find it quicker just to create a nice curve and then we're gonna revolve that around so I'm gonna say create revolve I already has the profile because I pre-selected the profile what's the axis so I'm gonna click on that line there and you can see that it's taking that profile and revolving it around that main axis I'll say okay and you'll notice I'm in this case component I'm gonna go ahead and expand this open I'd like to open up my bodies and my sketches folder or pull-downs and for whatever reason okay there we go and that way I can get to them easily so I can turn things on and off okay according to the drawing this front edge is chamfered so I'm going to go ahead and do the chamfer command of 0.35 now again and I've mentioned this in my previous live streams I could have created that chamfer in my sketch in my profile and then revolve that around but I like to let fusion do the hard work why do extra work in the sketches when I can just use the chamfer command and I can come back and edit that chamfer command much easier in the timeline then trying to find the sketch that was used to create that angled face so again you'll see me keep my sketches simple and I'll use commands like fill it and chamfer on the 3d model I'm gonna go ahead and since I'm kind of working on this area right here and go ahead and create some fill it's in this case their point zero five according to the drawing on those two edges there so you can kind of see how we rounded those off a little bit and again I'm just grabbing all of this information off of the drawing I'm not gonna keep going back and forth to the drawing unless it's necessary okay um which I'm gonna go back to the drawing right now now I want to create this curved section you see in the back right here okay and so let's do that I'm gonna create a new sketch now I get this question every so often should I go back and edit the original sketch or should I create a new sketch and this honestly is up to you if I were to go back and edit this sketch I wouldn't really see what the 3d model looks like because I'm going back in time before any revolve extrude cuts or anything like that has happened however if I create a new sketch I'm gonna say create a sketch on this front plane you'll notice I see my 3d model and so again it's really up to you on what you want to do if you want to see the 3d model create a new sketch if you're okay going back in time and working with something that's even before it was created that's totally fine also there's really no right or wrong answer here I'll go ahead and I'm just gonna create a kind of like a centerline that kind of cuts through the center here and I'm gonna turn that to construction so I select it I say construction and now you can see it's a dashed line it's not an actual object line I also want to project some information now here's another tip I can select specified entities or the whole body and the whole body kind of does like a silhouette so watch what happens you know it's not letting me pick edges or anything like that just gonna click on the whole body I'll say okay and you'll notice that it projected the whole body okay let me undo that I'm gonna do the project again but this time I'm gonna say specific entities and I'm gonna click on the same thing I'll say okay and I'll turn off the body and notice I have a slight difference result it's not a closed profile and this specified entities is looking more for like edges and because that was a revolve there's really only one edge on that revolve and so you can kind of see it didn't create this one down here so if you ever do a project and it doesn't seem to project everything that you want do the project body instead hang so another tip hopefully you guys find that useful okay what I'm gonna do now is just kind of mock up my curve actually you know what I like before I'm gonna do that I want to create an offset of this line down about half an inch half an inch not five inches minus 0.5 so I have my centerline and then I just created a line that's half inch below that and I'm gonna use that when I create my three-point spline right here and I'm gonna go ahead and snap to this edge and you'll notice when I get near that edge it turns from a plus two across like a little X and that means it's going to create a coincident constraint automatically on that edge I'll say okay and there's my three point spline again I'm going to kind of constrain it by adding some dimensions so I want this point to be from here I want that to be over five point two five and so you can kind of see how that updated my spline a little bit and then I want this distance let's make that a little bit larger let's make that like five point five and you can see because that point was coincident with that spline even though I moved it over it's actually following or staying coincident with that spline kind of a neat little tip there so I'm gonna go ahead and finish my sketch now the reason I did a we're gonna use that profile basically that that spline to split this body it's gonna come under modify split body what's the body to split and then what's the splitting tool and I can actually click on that spline and it's kind of hard to see here but it's basically taking that shape and you know it's gonna use it to cut away so when I say okay watch what happens to my bodies over here when I say okay I now have two separate bodies now we don't need this little piece that we're getting rid of so I'm gonna right click on body 2 and say remove now you'll notice in there there is also delete please don't use delete I use removed 99.9% of the time delete if anything was referenced from it and stuff like that it would kind of mess up your timeline so remove basically says okay I created the body I'm gonna actually remove it and you'll notice it even created something in the timeline so I could always come back and re add it in there if I want to if I were to suppress that that body would come back okay but it's basically removing it out of our design I think that's the fastest and simplest way okay so we got kind of the basic shape I'm gonna add a little more detail to it I know there's a fill it on the front and the back edge I think they're about point one according to the drying so you kind of see it creates a nice fill it on that back edge and I'll do the same thing on this front edge create that point one fill it say okay and if I were to create a section analysis let me go ahead and create a section analysis through the part you'll notice that it's a solid body okay it's one big chunk of material well I want to hollow this out so I'm gonna use the shell command okay it's asking for a face to look into well this is actually open in the design right now it's closed I'm gonna click on that face and then I'm gonna start to drag now it's kind of hard to see but if I rotate we're now looking inside the part we're shelling it out in fact it's supposed to be 0.1 okay now let me turn that analysis back on again and sure enough you can see that we've shelled the part out and it has an equal wall thickness of 0.1 so I really like using that analysis it really kind of shows what's going on so again using the shell command we opened up we looked into this face right here and then we hollowed it out to be point 1 inches okay moving on now what I want to do is now I'm going to split this into three bodies and this is that example I gave earlier where I need to create a sketch well I could come back to this sketch here because this actually has enough information that shows the whole body so I am gonna this time go back in time and edit that sketch I'm just gonna draw a rectangle like so I don't care what size right now I'm just gonna mock it up then I'm going to come in and add some dimensions so this is supposed to be one point three wide and it's supposed to be 2 inches from the front edge okay so you can kind of see how it's now moved it in the correct location now you'll notice that the width of it is constrained but the height of it isn't in this case it really doesn't matter I know some people like to have their sketches fully constrained and I could absolutely you know add a dimension in here and say make that you know five and a half if I wanted to but you know in constraint you don't constrain it's other things but in this case it's basically being used to just split the body what matters is the width so I'm gonna go ahead and say finish now my sketch went away and this is the exact reason why I like to unfold my bodies folder and my sketches folder because I can very quickly come in here and toggle these on or off so all I have to do is turn that sketch to which was right here turn it back on okay modify split body kind of like what we did with the back of the part what's the body to split that's the body what's the splitting tools I'm gonna click on this rectangle you'll notice it selects the whole thing so I'm gonna go ahead and click on that watch what happens to my bodies over here when I say okay I now have three separate bodies and to keep things clear I'm going to rename these I'm gonna change this one to front I'm gonna rename this one to back and I'm going to rename this one to mid please please please name your body's name your parts so it's easy to find okay if I want to find the mid one that it is right it's labeled mid okay okay so here's where I think it's gonna get kind of so we started with a basic shape we started with that curve we revolved it we've added a little bit of detail to it kind of the main design and then we've sectioned it into three separate parts or we've split it into three separate parts now we're going to work on each of those individually so you can kind of think of the case as the top level and now we're going to work on the children of it so basically like the front and the back etc so to do this what I'm going to do is we're gonna work on the front to start out with I'm going to right mouse click on it and say create components from bodies and you'll notice that it took it out of there and it created a component it called it front and it's it's own individual component now but what's cool is it's still kind of linked to this case so if I were to go back and edit the case you know like change the shape of the spline for example it would affect the front also so this is what some people call top-down design okay so I'm going to go ahead and turn off these other bodies I don't need to look at them right now so here is our shelled out front component okay now the first thing I need to do is I need to change the thickness of the wall in in the actual design in the actual part it was a little bit thinner than the rest of it so I'm just gonna click on this inside face and say press pull or I could come under modify and say offset so if you're looking for the command it's actually called offset and if I grab this you can see I can drag that and make it thinner so you can kind of see how I'm changing the thickness there and in this case I need to go minus point zero two I'll say okay and here's the other thing I like about working with components here's the timeline for everything that I'm doing with this particular component from time we created it as a component we did an offset okay then we're gonna do a sketch we're gonna do Philips we're gonna do stuff like that okay I'm going to zoom up here let me show you where's the front part we changed to the camera really quick so we're gonna be creating these little screw hole things you see inside those little screw boxes that's what we're gonna be creating right now so I'm going to create a sketch on this inside flat face I'm gonna say create sketch okay and I want to put one of those bosses in the middle between these two edges right here that you see okay well there's no like center point or anything like that so I have to create that automatically so I'm gonna project so I'm going to hit P for project and this time I don't want to project the whole body I'm gonna just do the specified entity so I'm gonna click on this face and it projected that face and I'm also gonna project that line cuz that line might actually help me so if I were to expand this open let's let's unfold these guys a little bit okay and I turn off that body and it's a little bit hard to see but you can kind of see it projected these lines right here okay then I can come in zoom up here and create a construction line so I'm going to say line construct I'm just gonna go from one point to the other point and you'll see that it's snapped and it's black which means it's fully constrained and what's nice is now if I create a circle I want to make sure I turn off construction if I get near the center of this line you'll see it'll snap automatically you see the whole triangle that means it's going to snap right to the midpoint and then I can type in my circular sizes here so point one and click in that same spot and say point two and I now have that profile okay then I need to extrude this now you'll notice that it's kind of hard to pick all of these right so I'm gonna go ahead and click and hold and it lets me grab these profiles so I'm just gonna click and hold because some of these profiles are behind a 3d body I'm gonna grab all of those and say extrude now some of these tips I've shown before like clicking through to grab other geometry etc so if I'm going a little fast on those it's because I've shown them before hopefully you know of those tips I'll specify my distance of 0.67 5 according to the drawing but you'll notice that it's red well it's because it's actually cutting away well we want to join that together now I also want to add some draft to this and I've mentioned this in my last live stream I could do that right here but I don't like to because not only would it taper the outside it would also taper the inside and if I ever wanted to come back and change that taper angle I have to know that I did it in the extrude so I'm going to use the draft command instead so let's go ahead we typed in our distance we told it to join we'll say ok and you can see that we created that nice-looking standoff okay and then like I mentioned I'm gonna come in and use the draft command so I'll say Draft what's the plane so it's asking for a plane what do you want to basically hinge around so we're gonna hinge around this plane here and then it's asking for a face I'm going to go ahead and grab that face and if I can extend this you can kind of see what's happening here it's basically hinging around that plane so that's what that is asking for and we only need to do like 1 degree of draught in this case and there we go we've added some draft to that in fact if I were to look straight at it you can now see see that draft right there okay obviously in fact I looked at the chat and somebody said I smell a circular pattern yep you guys are ahead of me here we need six of these so I'm gonna come in here and say create pattern circular pattern okay now by default this is usually set to faces and I could come in here and select all those faces but I'm much much rather change this to features and say I want to pattern that extrude and I want to pattern that draft angle also so I'm gonna select both of those in my time line as those are the features what's the axis I just have to click on a circular edge and let's tell it to do six of these guys so I'm gonna say ok and it patterned the extrude and the draft all at the same time pretty quick okay the last thing I need to do is you'll notice that these pieces actually like indent in so there's like a little recess in here and then this little edge here kind of slips underneath it so that's what we're gonna be creating next and I thought the easiest way of doing this is I mean there's multiple ways I could create a revolve with a profile and revolve it around but check this out here's a neat little tip I'm gonna create an offset plane from that face and I know that it needs to go in minus point two okay and so you can see that that plane is now inside that body then I can come in here and say split face not split body because that would actually remove the whole ring off of it right I'm gonna say split face will click on that face what's the splitting tool it's gonna be that plane and I'm gonna say okay and notice what it did let me turn off the construction you'll notice that line doesn't exist on the outside it only exists on the inside because we only split that face then if I come in here and I say either press pull or offset I can say offset this face and watch what happens I'm pushing that face in and let's go the correct distance in this case minus 0.02 we just created that recess in there in fact if I turn on the analysis again real quick you can kind of see that let me go to the front there's that recess I notice when I get really close I get kind of these jagged lines because this is a long curve so if you see that it's just the number of faces or liberal lines representing that for you okay so I could have done it revolve but that would have had me create another sketch I'd have to draw a rectangle I have to dimension it a lot kind of stuff it would work but this case I was able to offset point two and then offset that face the crack distance point zero two so hopefully you found that useful okay actually according to the drawing that was the last thing so what I'm gonna do now is change the appearance of it so I'm gonna hit a for appearance and I showed this in my last live stream we're gonna be using the same material over and over again so I added it to my favorites so if I click on favorites you can see this blue plastic someone's gonna drag that on there and if we zoom up you'll notice it's got that oops bumpy texture and stuff like that and it's the correct color so let's go ahead and save that say okay and pretty much in about you know 20 minutes we created this part okay so I'm gonna continue on with the the back part we won't have time to do the middle part today but let's we'll see how far we get with this okay so we worked on the front right we made it into its own component we're gonna do the exact same thing with the back I'm gonna right click and say create components from bodies and we now have this back component in fact I can fold up the front we don't really need to see it anymore and I can even turn that guy off okay so this is kind of that skeleton shape it's the basic shape of the part but obviously we need to come in and we need to add a lot more information in here so we're gonna be creating all these little ribs and we're even going to do the decals on the back and those recessed holes and a lot kind of stuff so that's what we're gonna be doing next okay so created the component we activated the component now I want to basically create those screw bosses so let's click on this front face here and create a sketch and everything I'm doing here is in that outline so if you want to re-watch this video later on and follow in the outline hopefully that will make sense to you let me jump to here so I'm going to be creating these screw bosses and these ribs so and you'll notice I even labeled things like mirror lines we're gonna mirror some things later on obviously we're gonna create one of them and mirror it over here we're gonna then mirror both of these down to here but you'll notice that it's not centered so that's why there's this little offset mirror line so again I'm just using this drawing to create my so I'm just gonna start out by kind of mocking things up I'm just gonna draw three circles I don't care about what size they are right now okay just something like that then I'll come in and add some dimensions so I'll start with this guy and it's supposed to be point three the next one is 0.45 and then this last one is 0.7 again according to the drawing okay so those are the circles that I want and then I need them to be located a certain distance from Center so I'll go ahead and place that there and that's one point oh five and you'll see it moves it over and then it needs to be a certain distance up okay so I'll come in here and say it needs to be point seven and notice it's fully constrained now it's constrained to that center point everything is dimensioned and everything looks good now I'm going to do something interesting here let me go back to the case and if we look in here in fact let me just make let's just do the back I'm just gonna isolate this guy real quick you'll notice that there's these support ribs and they're kind of stuck farther back in there I'm actually gonna create where these ribs are right now and then we're gonna come back and use that information later because they have to do with this particular feature and we're gonna be mirroring this feature I'm gonna add that geometry and right now okay so I'm just gonna again I don't care about the dimension or anything like that I just want to get these lines and you'll notice I'm kind of hovering over doing something like this you'll notice that they are not constrained which means I could move them around right I don't want that to happen so I'm going to come in here and say I want that line to be coincident with that point and you'll see it turn to black if I said I want that point to be coincident with that point it would bring that point all the way down I don't want that I just want these to be lined up with each other and now you'll notice that they're black okay and again this will make more sense later on but what I just did there is I kind of created the geometry for one of these standoffs now I want to continue that okay I want to mirror it over here but to do that I have to have a mirror line and I don't have a mirror line right now so I have to create one and I typically do my mirror lines as construction geometry because I don't want them to be an actual object line or that would affect my profile okay and then let's go ahead and mirror this over so under create mirror I'm just gonna draw a box around my geometry I don't want to go crazy I don't want to get all this stuff I just basically want to get that geometry there then I'll say what's my mirror line that's my mirror line and you'll see it's gonna mirror over to the other side and you'll see my little rib lines that we're gonna use later on are in the correct location okay now I want to mirror down and again I showed this in the drawing we're gonna basically create a line that's point eight seven five down from the center of these circles and mirror it across that line so to do that I need to create a line and again I have my construction checked so I'll click here and then point down and type in point eight seven five okay so it created a construction line down and then all I have to do is create aligned over like so and now I have that line that's in the correct location I'll say mirror I'll draw a box around the stuff I want to mirror what's my mirror line I'll click on that line there and we can see that we mirrored it down to the bottom pretty quickly now some of you might be saying well Brad I've watched some of your other live streams and you always say keep your sketches simple draw one of them and then use like the mirror command using features and I could absolutely do that but because this is a really kind of a weird curved surface and stuff like that I'm actually spending more time with my sketch and basically saying here's the four screw holes and I want them to go against this curved surface so again there's no right or wrong way but in this case I'm actually creating a more complex sketch that way if I ever needed to change you know the distances or whatever I could come back to this sketch okay so now what we're going to do is I can either say finish sketch I've shown this before if I say finish sketch it gets me out or I can actually click on my profiles so I'm gonna go ahead and grab these profiles then I can right mouse click now you'll notice it says extrude and it says extrude be careful the the tan or the orange whatever color you want let's extrude a surface so it would basically create a thin paper tube basically whereas the blue one is extrude an object okay like a profile so I'm gonna say extrude start to drag and you'll notice it kicked me out of my sketch and it brought me into 3d automatically so it just saves a little bit of mouse movement instead of having to say finish sketch and then come in and do an extrude okay now these are the holes so I want these to go all the way through so I could just drag and you'll see it cuts through like so but I want to be more precise okay so I'm gonna come in here and say go through all okay now why would I say go through all the reason for that is if I were to come back and change the shape of this curve in my skeleton model for example I always want these holes to go through all of it no matter what shape that is if I had only said you know extrude an inch and a half or whatever and we really kind of changed the shape of this it might not go through all of it so sometimes it makes sense to do this extent all okay I'm gonna go ahead and say okay my sketch turned off but again I just unfold these guys like so and I can turn my sketch back on there we go okay then I'm going to extrude these larger circles and here pay attention to what I'm doing here because I was trying to think of what's the easiest and fastest way of doing this and I could have created multiple sketches and offset planes and stuff like that but we're gonna use one command to do all of this stuff it's pretty cool so I'm gonna select these four larger circles and say extrude I'm gonna start to drag to tell it which direction I want it to go now how far do I need it to go well this is a weird curved surface in here so I'm going to say instead of distance I'm going to say to object and then I can click on that curved surface now you'll notice I get an error that says tool body failed and now you're like well what a great demo all right the reason for that is this option right here chain faces and it's kind of hard to see with the icon because it's highlighted but it actually shows kind of like a curved surface and it's only going to the front of it this one it looks like it's gonna grow to follow that curve so watch what happens when I click on that guy now you can see the other icon better so by doing this option what we're saying is to extrude to that surface no matter what the shape is and change you know follow the curvature and everything and you can kind of see that's what it's doing okay however these are too tall they need to start way down inside the model so this is where I would have had to create an offset plane and another sketch and a lot kind of stuff but check this out instead of starting at the profile plane we're gonna say offset plane and we're gonna offset into the part 1 point 7 inches and look what it's doing it's kind of hard to see cuz the sketch is sort of in the way that blue face but what we said is use this profile but start 1.7 inches into the model before you start extruding pretty cool and we obviously want to join that together so I'm going to say okay I'll turn the sketch off so you can kind of see what we did there okay and again this is all in the drawing here's that one point seven you can see there's the the thicker standoff right there so that's what we did hopefully you're fine finding this useful okay let's do the exact same thing this time with these middle circles I'm gonna go ahead and select those I'll say extrude tell it to start going that direction okay now I'm gonna do the exact same thing instead of a distance I'm gonna say to object I'm gonna click on this inside face and you'll notice it says tool body creation failed well we got that last time so I'm going to click on chain faces but you'll notice I get the exact same error and you're like whoa what's going on here well the reason for that is because this profile is actually inside here you'll notice the face I selected doesn't intersect in there I know that's a lot of information but if you ever get something like this any like why does this not work try something else so instead of the inside face I'm gonna select the outside face and notice if I change that from cut to join that actually works cuz it was able to snap to a face and it really doesn't matter that I selected the outside versus the inside in this in this example now these standoffs need to be where they're at so I'm gonna go ahead and say okay we'll turn off the sketch real quick and we've created those four standoffs and just like before I want to add some draft to these but I'm gonna have to do the draft as two separate steps okay you know I want to draft this to be one degree and I want this also to be one degree so I'll come in here and say draft what's the plane I'll go ahead and select that plane there what's the faces and I can actually grab all four faces at the same time and it remembered my last angle of one degree so you'll notice when I hold down my control key you can actually see the preview so there's zero degrees of Draft and then there's one degree a draft I'll say okay I'll repeat my draft command but this time my plane is gonna be here what's the faces I'll have to rotate a little bit so you can kind of make sure we're grabbing the faces here I think it's doing an autosave there we go I'll click those small faces there it remembers one degree kind of hard to see but if I hold down my control key you can kind of see that the preview changing ever so slightly and now those standoffs have one degree of draft okay so now what I want to do is I want to create these rib features because we're still kind of working on these little standoffs but you'll notice they're indented inside the part a little bit in fact according to the drawing they're one inch into the design well those lines are on this sketch so what I'm going to do is I'm going to create an offset plane we'll drag it in minus one and kind of see a nice preview it kind of shows what that looks like and then I'm gonna create a sketch on that plane so you'll see that that plane kind of cuts through one inch into the design what I'll do now is I'll project I'm going to use those existing jump pieces of geometry so it's kind of hard to see but notice when I hover over this line it's actually projecting it back to here so you'll see it projected that line there I'm just gonna quickly go through and grab these lines off the first sketch and project them on to that second sketch I'll go ahead and say finish and let's turn off that first sketch and now you'll see that those lines are actually farther back in the model so it's not having to recreate and remember what I did the reason I did it this way is I only had to draw two lines and then we mirrored that and we mirrored it again so instead of having to draw a whole bunch of lines I was able to reuse them and just use the project command okay okay I really like the web command let me say web what's the curve I'm gonna go ahead and click on that curve and look how powerful that is even though this line is really short because we have extend curves turned on it's going to grow and extend to the next surface automatically so literally I just click on these lines and you'll see how fast we're gonna create these ribs or these webs I should say so I'm gonna go ahead and click on all of these real quick like so and instantly we have those webs and they're all different that's why it was so neat to be able to just mirror everything it already had the thickness in there I mean I could make this you know point zero two and they would be thicker or thinner I should say I'm sorry so but they are point zero four I'll say okay and we now have those ribs are those webs I should say and there I could call them ribs but we call them webs okay hopefully we're doing okay and you guys are learning stuff I'm gonna go ahead and change the appearance since people like the the blue I'm gonna go ahead and drag that on there so we're starting to see when our part looks like so the next thing I want to do is work on this little arm right here that's going to attach to that pivot that we created last last time okay so again using some information from this drawing I'm going to create that okay um let's see where we're at here I'm just looking at my outline making sure we're doing everything okay oh okay so now what I want to do is actually I told you I was gonna create the arm I actually want to work on the back of this I like to kind of keep everything organized so we worked on all of these little standoffs the next thing I want to do is kind of finish what the standoffs look like on the back of this part and you'll see that here so you can see these little indentations and stuff like that so that's what we're gonna do next so what I'm going to do is I don't have a flat face back here to create a sketch on so I'm gonna use an offset plane and I'm gonna drag it back now I could just kind of guess but I like to go let's just go maybe we're almost at three and a half so let's just go - three and a half and I just created a construction plane that's exactly three and a half from that front face okay well sketch on this face and I'm about to show you a neat tip so I want to project these four circles so I'm going to come under here and say project now if I click on the edge of the circle and say okay you'll notice it did project that but I don't see a center point okay I'm gonna undo I'm gonna project again but this time instead of selecting an edge I'm gonna select the circular face and say okay and this time I see a center point so here's my little tip I like to project the geometry as much as I can so this is an edge I would say this is geometry this is a face right so the reason it probably didn't do a center point is because it's approximating this weird shape that's on a curve and sure enough it turns out to be a circle but by projecting the face it knows that that's an exact circular face so there's the exact center of that face so again just a neat little tip I like to project the geometry instead of edges if possible okay thumbs up if you like that one hopefully okay so I projected these circles now I'm gonna go ahead and again just mock things up I'm just gonna draw a couple quick circles here I don't care what size yet then I'll come in and say I want that circle to be exactly 0.5 in diameter and then I can come in and say I don't want these to be equal so I'm with that circle and that circle to be equal I can just click on these real quick so instead of having to type in 0.5 every single time and dimension every single circle I just did one and made them all equal okay here comes the fun part so now I want to extrude these in so I'm gonna select just the bottom circles first and say extrude okay now here's where it gets interesting I need to go a very specific distance and I'm not sure what that specific distance is but according to the drawing I give you the distance from this face right here so just like before I'm gonna say start but I'm gonna say from object and I'm gonna click on that flat face okay so it's gonna start there but then I want to offset the correct distance which in this case is one point eight five so you'll notice the preview now so what did we do the sketch is right here okay that's where the sketch is I told it go from this face come forward an inch point eight one point eight five inches and then start your extrude and how far it really doesn't matter in this case okay because I didn't have a flat face in here somewhere to say okay put my sketch there and extrude it out I'm having to reference actual geometry and again this is in the drawing here's here's that one point eight five it's kind of hard to see but it points to that indentation right there and then the next thing we're gonna do is two point four so I'm gonna do the exact same thing we'll turn on our sketch I'll select these guys say extrude and again play with this you you kind of have to see it happen to understand what's going on so instead of it starting here and extruding I'm saying start from this object right here this face okay and then offset two point four so you can kind of see it's now offsetting two point four and then it's extruding some distance and again I just have to go far enough and you can see how tight that curve is so we'll go ahead and say okay and we've now created those recesses in there automatically pretty cool okay we're gonna go a little bit over we're almost done probably about another ten or fifteen minutes I noticed a lot of you didn't complain last time hopefully that's okay if you have to drop I understand this will be out on YouTube you can watch re-watch it on YouTube so all we need to do now is create that arm so let's go ahead and create a sketch on this front face and I'll go ahead and turn off those other sketches so I don't need and what I want to do is I want to grab some information so I'm gonna use that project command again which I absolutely love project this time I want to grab the whole body so I'm going to say body I'll say okay and you'll see that it but projected that shape right there for me if I had just said this face it might not have projected that that edge then I need to create a 3-point rectangle a very specific distance and a very specific angle so to do that I'm going to just create a line and I'm gonna click somewhere on this curb you can see how it's snapping automatically to that curve okay then I can come in and dimension that line now you'll notice it wants to dimension it horizontally I want to dimension it aligned okay if I'm really careful I can get near it you can kind of see I can get the aligned but I can also right mouse click and force it to be aligned horizontal or vertical so I'm going to say aligned and now no matter what its gonna stay aligned and that needs to be 0.75 and watch what happens that point still follows that curve okay now I can do my rectangle and I'm gonna do a three-point rectangle from there to there and then the correct length which in this case is 2 okay so that's how I was able to create the correct sized rectangle in the correct orientation will use the revolve command again so I'll say revolve what's the profile that's the profile what's the axis this edge now you'll notice an error here but we're gonna fix that it's taking that profile in revolving it around that axis and it's the correct length so I'll go ahead and say ok oh and actually I lied let me go oops let me go back when you do this you want to make sure you say new body because I want to work on this part separately for a while and then we'll combine it to this body so instead of saying join I want to make sure it says new body which it did okay now you're all going playing screaming at your computer what about that ugly flat face how are you gonna fix that blah blah blah here's a cool trick if I go under the modify command replace face this is an underused command watch how powerful this is remember I have two separate bodies I have this blue part which is the back and then I have this body too which is the gray part so I'm saying replace face I want to replace that face there using this face here and boom I say ok you'll see it actually matches that shape so instead of like dragging it up and deleting faces using like direct editing I just used the replace face command really pretty powerful okay okay I showed this last week I want to create a round fill it here so I'm gonna say fill it what size I don't know I'm gonna say measure and I'm gonna click on that same edge and it's gonna figure out that that's a point seven-five radius to round the whole thing over so kind of a quick way to round the whole thing which is pretty neat now I only need half of this guy so I'm gonna use my famous split body command here is the exact reason I want to keep this as a separate body for now I don't want to split the blue part so I'm gonna split that guy what's my splitting tool we'll use the the front plane because since that slices right through the middle and we'll say ok and now I have three bodies but we don't need this guy so I'm gonna say remove and it's gone ok so pretty quickly I created that armed right there I'm gonna go a little bit of an accelerated pace since we need to kind of finish up here I need to create a hole on here so I'm just gonna click on somewhere on the face right mouse click and you'll see it about 4 o'clock is that Holcomb and or I could go create hole exact same thing okay so I'm gonna come in here and say I'm going to say create a hole and it kind of just randomly puts it on that face if I grab this blue large dot you'll notice there's two dots in the blue this one is the center of the circle this one is the center of the whole face so obviously I want this guy right here I want it to be point two in diameter and I just wanted to go all the way through doesn't matter so I'll say okay and we just quickly created a hole I could have done a sketch I could have created the circle I could have dimension the circle could have a hit extrude cut I just find this to be so much faster and it's a feature in my timeline that I can come back and edit okay I want to shell this guy out so just like before click on a face right mouse click it shows me the commands that make sense and one of them is shell I can start to drag to kind of get a preview what that's gonna look like it needs to be point 1 thick but I noticed that it's also shelling it right up here and I don't want that so I'm gonna hold down my control key and I want to select that curb face but it's kind of buried so I'm gonna click and hold and I can probe through so there's that curb face so if I keep going you'll see it selects all these other faces etc I just want that one it so now notice it's shelling the front face and that top face of this little stand off of this little arm I'll say okay and we've now shelled those guys out again I'm just using information from the drawings so you'll notice that there's circles that need to go around so I'm gonna continue on here I'm gonna create a sketch on that face I'll project maybe this little let's do that entity I'll project that guy there now notice this time it did put the center point because that's a perfectly flat circle it's not on any curved surface so that one worked and I could just snap to that circle there and snap to that circle there and you can kind of see we're just gonna continue with that profile extrude I start to drag in the correct direction I'm gonna say join how far I'm gonna say to object and just click on that curved face and it's gonna take that profile and extrude it back to that curve like so okay looking pretty good here okay there are some little ribs inside there so I'm going to do those again I'm gonna go pretty quick because it's really similar to what we did before you'll notice there's these two lines right here I actually want to grab those lines I'm gonna project you know all those features like so and then I'm going to draw a line up here something like that and another line down here something like that okay I'm gonna use these lines for my ribs well obviously they're not the correct direction so I'm gonna say perpendicular that line and that line and now you can see it's perpendicular that line in that line they're perpendicular and then same thing with the coincident I want that line coincident with that point that line coincident with that point so I just created in the correct direction what that should look like there's also some ribs up here so I'm just going to draw a line I want that to be parallel to this line here I'm just make sure I'm looking straight on and then I can dimension that line so I'll go from here to here is supposed to be 0.5 and there's another one over here I could have drawn it but let's just use the mirror command so I'll say mirror using that as my mirror line so it's like reflecting along that line I now have these little line segments that are gonna help define those ribs okay now I accidentally made a mistake I put them on this front face and they were supposed to be farther back so what I can do is I can create an offset plane start to drag back and I think they're supposed to be minus 0.1 1 5 back ok then I should be able to come in here and say redefine sketch plane yeah I see this is I was afraid of I created that after that so I'm going to actually have to create drag this in front so now my plane is before I created this sketch and I should be able to say redefine sketch plane and click on that offset plane you can see I don't know if you saw it but those lines kind of jumped back a little bit and instead of being on this front face they are now back on that plane so instead of having to undo and redo and I'll kind of stuff you can always come in and redefine your sketch plane I'll say that I purposely made that mistake right no so neat way I mean obviously going through I was rushing and put it on the wrong plane but I was able to redefine that very quickly easily okay so let me turn off that construction plane will create those webs again I'll click on that boom it creates those webs and I can click on all of these at the same time okay and there we go now if I were to try and click on this guy notice what it's gonna do it actually fails and you might be saying well why would that fail well the reason why is because there's no boundary for it to go to you can basically imagine that this part doesn't exist because they're not joined together so before I do these two lines up here I'm gonna have to join or combine the parts together so I'm going to go ahead and accept that okay cool ribs there we go no then I'll come in here and say combine that part in that part we want to join them together so watch what happens over here we now have one single part I'll turn that sketch back on and now if I create that web you'll see that sure enough it knows where to go to so it can actually stop at that curb surface I just love that web command it's it saves so much time with complicated ribs and webs of stuff like that okay now you're probably saying well what about all those teeth and all kind of snaps well we're gonna go a little bit longer on this I apologize but we're doing okay what I want to do is finish up with this little indent thing here and then we'll create those little teeth I need to recess a nut on here but again I don't have a flat plane so I'm going to say construct and I'm gonna say tangent plane because this is a curved surface I'm gonna go ahead and click on that and said basically I want it at zero degrees okay so Angelo just sent me a message saying what about drafting these ribs so it's the exact same thing and I won't spend too much time here but if I say draft and I click on that face there and then I say I want to draft that face and that face you'll see I can actually you know add draft to those faces you know and and I you apologize I'm not doing that on every single thing here I'm not an injection mold specialist or whatever I know you have to have Draft on all these faces to make them come out of the injection mold but I was showing you you can add draft and here's how you do it you guys will have to take it to the next level and do it on all of the features otherwise it would take way too much time so a great question thanks for asking that okay so I created ace we turn on my construction plane so we could created the construction plane that was tangent to that curve surface let me expand this guy open turn off the old one turn off that old sketch so it's basically just sitting right there so now I can create a sketch on that face I'll go ahead and project and because it's curved I'm gonna go ahead and project that face there and you can see it created that center point for me and then I'm gonna use the polygon circumscribed polygon command what this allows me to do is it's gonna basically create the shape of a nut for me automatically and I know in this case the radius is what it's asking for is point one seven you know I'm just gonna go ahead and say okay you'll notice that the nut is kind of rotated I don't I don't think that looks all that great so I'm gonna come in here and say perpendicular I want this line to be perpendicular and you'll notice as I hover around it's actually finding you know lines from the ribs for example so I could go ahead and click on that and you can see how it rotated that nut shape to be perpendicular with that other line then I just have to select this guy extrude again using the information from the drawing we extrude it in minus point six five it actually goes pretty far into the part I'll say okay and there you can see sure enough you're gonna see where it goes inside there also pretty cool so use the tangent command for that so okay now here's where we're gonna join this to the other part now I could draw the tooth and pattern it like we did last time but why not reuse something we've already created so I'm going to expand open my data panel and here's that steak pivot that we created last last livestream I'm gonna say insert into current design in fact even before that I'm gonna go ahead and save just so I have we've done a lot of stuff so now I've saved so I'm gonna go ahead and now insert into current design and watch what happens it's actually gonna bring this model in now it's rotated the wrong direction so I'm gonna rotate 90 degrees okay kind of snap to 90 degrees and then I like to sort of get it kind of close to where it needs to be it doesn't have to be exact and then I'm going to use point to point I'll grab that point there that edge is gonna actually line up with that edge there and you can see that it positioned the part right where it needs to be I'll say okay and then we're gonna use the combined command what's the target that's the target what's the tool this is the tool and instead of joining them together I want to cut so we're going to use the information the tea from this red Park and it's gonna basically in engrave embed whatever term you want to use into the blue part I'm gonna go ahead and say okay and if we turn this guy off we instantly have teeth okay now I could have recreated the pattern that's totally fine but I just wanted to show how you can use existing geometry to help with your design okay now I don't need this anymore so I'm going to right click but you'll notice that I don't see remove in here and that's because this is a linked component you can see that by that little chain link right there so I'm gonna break the link and now when I right-click on steak pivot I can say remove so I removed it out of there pretty fast okay okay so we're pretty much done with that arm the last thing is there is a cool plug that plugs into the back it's kind of hard to see here then I downloaded off of grab CAD and so we're gonna bring that in but you also notice it's recessed a little bit so we're gonna do that real fast so I'm gonna go ahead and I'm just gonna use maybe this same plane right here so I'm going to create a sketch on that face I'll draw a circle somewhere here that is 0.875 in diameter line that up with the vertical point right there so it's lined up vertically and then I need to dimension it and you'll notice I don't have a point that I can dimension to so I'm going to have to project that circle and now I have a point so I'll say from here to here and again this is where it gets kind of hard so I'm going to right mouse click and say I want this to be a vertical dimension and I want that to be 0.1 and there you can kind of see how that updated okay I'll click on that profile I'll say extrude now this is gonna be kind of weird I actually need to add some material to the inside of this part here so I'm actually gonna drag into the part a little bit and instead of cutting I'm gonna say join and I want to basically offset this to be like I'm sorry I want it to go let's see to the height of the short stand-up I knew there we go I'm gonna click on that short span off there this is why I create notes so I knew the exact distance so you can see in this case it's 0.15 so we use that circle we're adding some material in here okay and then I'm actually going to add even more material so I'm going to click on this face here say press pull and we're gonna add 0.1 to make that a much larger shape okay let's make more sense here in a moment it's kind of hard to see inside the model so I won't show it on the video I'm going to turn on my analysis and here's what we just did okay I had a profile and then I extruded it out a certain distance to be in line with these guys but you'll notice it because of the curved surface it left this weird shape here which obviously is a big no-no we're gonna use that powerful replace face again what's the source face that what's the target face that and you can see how it filled that in and while I was in the section view so now you can see this is all a big chunk of plastic right there okay I'll turn our sketch back on grab this profile extrude or press pull doesn't matter I just need to go out this direction okay and if I were to turn on the analysis again you can kind of see here's why we did that offset okay because it basically extruded straight back and we would have blown a hole through it so we extrude it straight back and then we offset it 0.1 to give it some thickness there so that's why we did that okay then I'm going to create another hole so I'm gonna say hole because we need a place for that part to screw into so I'm gonna drag to that center point there and specify it to be 0.3 say okay we now have when we turn off my sketch the indentation we've got an extra material on the back etc and again yes I could add graph to that and I'll lock in this stuff but I'm not going to in this case so you'll notice over here I have this component and I'm just gonna right click and say insert into current design so again I got this off of grab CAD I could have gotten it off of a manufacturers web page or something like that I'm gonna rotate it to the correct 90 degrees let's drag it kind of over here a little bit and I'm gonna use that same point to point now what's neat about this component it's actually a waterproof component so this little ring right here is actually like a rubber gasket so it's gonna get compressed so I'm gonna click on that edge there and that edge there and you can see that it lines it up let's turn our analysis back on and we can see it sure enough that fits through the point three hole that we made and then this nut will tighten down and basically compress this whole thing together which is kind of cool so instead of having to model that we just brought it in okay okay we're gonna go in an hour and a half I apologize hopefully hopefully this is a beneficial I'm running to take but man when you're doing it live it never seems to go as smooth okay the last thing I'm gonna do here is I want to add those little tiny Phillips to these edges but like just like last time I don't want it to do it to the teeth so I'm gonna suppress those teeth so when I say suppress features you'll see that those teeth go away okay um thanks Angela Angela was like keep going man okay so now I'm able to add these Filat so I'm gonna come in here and say fill it let me drag this out to the side I'm just gonna draw a box that kind of encompasses everything that I want like so and I'll do the point zero one fill it and you'll see pretty quickly it gives me a preview what that's gonna look like and it fills all of those edges I just find that so so powerful okay now I'm gonna unsuppressed those teeth because I didn't want those guys fileted right so I'm gonna come in and say unsuppressed but watch what happens when i unsuppressed that I get an error and it doesn't fill it all of those edges and again it has to do with like all this little geometry and all the kind of stuff so to me it makes more sense that I should have done the fill it's before I had created these teeth so I'm gonna drag my timeline marker before that combined okay I'll create my fill it so I'll do the exact same thing I just did so I'll draw kind of a box around everything we'll do the point oh one everybody's happy I'll say okay okay then I'm gonna drag to the right and look what happened the teeth went back in and my Philip's worked so this one here is the one that failed so I can come in here and just delete that out of there okay so to solve this problem what I ended up doing was I tried doing the Phillips and I realized it didn't like it because of the combine so I just went back in time then I created my Filat and then I was able to do my combine so you might have to do this everywhere so often okay pretty pretty powerful okay I also want some small phillips on all of these edges back here and that could take some time so here's another neat tip I'm gonna say fill it now by default tangent chain is turned on now I could click on each of these individual little edges but I can also click on a face but notice it kind of highlights everything I'm gonna turn off tangent chain and now it only highlights this face I'm gonna go ahead and click on that face and say point zero one and look what it did it's kind of hard to see but it fileted all of the edges that are touching that face so I only had to click once right in fact I could do the same thing I could come in here and say you know what grab that face and it's gonna fill up the inside and the outside edges of these flat faces I'm just going to go around and click those real quick now you'll notice just trying to grab edges first so I have to make sure I find someplace that doesn't have an edge and then I'll do the same thing there I'll say okay and we fill it in all of those edges very quickly and easily using a face instead of an edge okay I'm going to do the exact same thing for that offset for the lip to go in there so we're gonna create a plane we'll drag it in - point - split face not split body but split face that inside face what's the splitting tool that guy there I'll turn off that plane and I can either use offset or press pull and you can kind of see I can go in here and say - point zero four again all of these dimensions are on the drawing but you can kind of see how we created that indent so we've done a lot with this model I mean there's a lot of geometry going on now so pretty pretty proud that we did all this in about an hour and a half for both parts the last thing and this is more for fun than anything I included the decals for you so if you want to come in here and say insert decal you can actually upload them into your project so here's the logo there's a laser warning I can conforms label so for example I'm gonna click on the star shower logo what face do we want that to be on I'm gonna click on that a face there and then it will let me position and scale and rotate if I need to so I can kind of rotate that for example I'll say okay we've just added that decal there and we'll add the laser radiation one don't look into laser with remaining.i I always like that one I like to look at it straight on now I'm kind of looking where it needs to be I can position it like that I can scale it up because this one's a fairly large decal I'll say okay and then finally one more decal the conformed decal on that face rotate that guy around and make him a little bit smaller and place him between these two screw bosses like so when I say okay now when I rotate around those decals are on that if we rendered it you would see those and just like in the actual model you can kind of see there's those decals there and stuff so I didn't do the embossing the button on the top just FYI I figured I'd get the major stuff here so anyways I apologize for going along I hope you found this beneficial please download the outline and the drawings that are in the description of the video and try and create this you know throw it out into the Facebook group if you finish it and you're proud of it and stuff like that I love seeing those comments Thank You Angelo for helping out I do go and review all the comments so I'll try and answer those I really like other people saying hey you should you could try doing it this way you could try doing it that way know for example ablaze banks I know he watches a lot of these and he has some really good feedback so definitely come back every so often and read the comments in these videos and you'll learn something not just for me but from the whole community so with that have a wonderful rest of your day and we'll see you next week thank you you

Channel: Autodesk Fusion 360

Views: 20,745

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: lQNLlAYEHgg

Length: 94min 3sec (5643 seconds)

Published: Thu Feb 20 2020