Fusion 360: Krenov Inspired Coffee Table

this is fusion 360 fusion 360 is a fantastic modeling program and why am i using this instead of sketchup to create my drawing or my model here I'm not ditching Sketchup but I am acknowledging the fact that fusion 360 is fantastic it is it's honestly better than Sketchup but it's still lacking a few features that I want to seed however it's being developed quite well so fusion 360 is probably the way to go in my opinion for long term use for me for 3d modeling however if you just need something simple that's easy to learn that really works check out Sketchup it's it's just way simpler to learn than this one in my opinion so why fusion 360 as well well when I when I was in college I learned 3d modeling on SolidWorks and when I left college SolidWorks was it's obviously expensive it's a really in-depth program and not a lot of people have it so I transitioned to sketchup which is more readily available widely used and everybody can get now that fusion 360 is being developed more and more and more people are using it and it's a very powerful program I'm trying to dabble with it and because it is so much like SolidWorks the learning curve for me personally was very little so tremendous program before I start in on this model I'm actually going to recreate this model just to show you my workflow and maybe you can pick up on some stuff as I work but before I start I want to let you know a couple things that I'm going to be doing that I think that everybody should know as just far just basics okay if you first off let's our bus elections if you click and drag to your left you are creating a crossing meaning anything that crosses that boundary box as well as anything that touches the area inside will be selected so you see this this leg down here right it is not 100% in the crossing but it still will be selected because it is crossing and part of it is in the middle so if I let go you see that it is 100% selected however if I go from left to right that is a window and a win means everything has to be 100% inside it in order for it to be selective so this vertical divider the center divider it is not 100% inside it will not be selected and this leg is not 100% inside so it will not be selected if I let go as you can see right there this face was but not this whole component so window versus a crossing window versus a crossing use those and pretty much most most of your 3d modeling software is use this nowadays but definitely use those to your advantage and I will in this particular model the second thing is I use keyboard shortcuts a lot in Sketchup I still use them a lot in this program they will always save time and then also something that this program has that Sketchup does not is this very fast right-click menu I don't know what this is called but if you right-click anywhere you get a menu and if you go in any direction you get basically like a piece of a pie I don't like I said I don't know the technical term for this in this software but I call it a clock wheel 12 o'clock always repeats your last command 1:30 has a couple different features depending on where you are in the model if you're in a sketch the 3 o'clock is redo bottom right is a couple different features as well 6 o'clock is primarily sketch whoops and 7:30 is move copy 9 o'clock undo 10:30 is delete and of course 12 o'clock always repeats your last command this is very handy to wrap your head around and get used to and implemented in your workflow it saves you a ton of time rather than going up here into the menus every single time so with that being said I guess we can go ahead and start a new model so I'm going to recreate this like I said let's go to new design up here control s and save this as coffee table video and what that does is it basically renames my model up here and just like in Sketchup everything is based upon sketches so you have to create a sketch before you can create 3d 3d geometry from it and when Sketchup I'm gonna turn my origin on over here by hitting this light bulb in Sketchup what I typically do is create a rectangular prism that is the appropriate length depth and height of my project I delete those faces and make the boundary box of component so I can basically work inside that wireframe as my overall length depth and height I do something similar in this but not quite three dimensions just yet I always create a foot print foot print sketch on the bottom plane which in this case is the blue red plane so right off the bat I'll select this plane which is the bottom and go to six o'clock to create a new sketch our four rectangle and we'll use a center rectangle I always make my footprint centered on the bottom plane on the origin and I'll click and drag in this direction I'll say nineteen is my first dimension which is my width and tab 36 enter let's zoom out now fusion 360 has parametric modeling so you can set constraints here parameters if I go to create I'm sorry modify change parameters I can come in here create a new parameter and say length equals this value with equals this value height equals this value material thickness number one is this material thickness number two is this number of drawers is this blah blah blah you can set all kinds of user parameters right off the beginning as well as adds some based upon things that you model as you're modeling that might be a little confusing it's a trim it so valuable but I'll just skip that for this particular video and just focus on dimensioning things something you see here is that every single one of these lines every single part of this sketch right now is black that means it's fully defined and I want to make all of my sketches black and all of them fully defined before I'm done and the reason being is if it's fully defined than it is everything has an exact location in space and there's no arguing that because it is it's constrained and it is defined you cannot move that it is there the reason why that's valuable and that's important is if you get say 3/4 away through your model and want to change something from I don't know 36 inches in width and say uh-huh we need 38 inches in width if everything is fully constrained and fully defined everything will every that you've already done we'll update accordingly if it's not you're gonna run into some situations where things just don't line up and you'll have a little bit of a headache on your hands sometimes control-z to back up so an example of that are four rectangle fighters draw a rectangle off in space all these lines are blue because their lines but who's to say this line doesn't exist over there there's nothing telling me where this particular line exists in space all I have is these constraints that are automatically made with rectangles which means this one is horizontal this one is vertical so I can't change the angle here because they're all they are already constrained now I can add dimensions to these and you know they'll start turning black and defining them in space like this one just turned to black now all of them turn blue when you hover over them but fully define your sketches make sure everything is black you'll have a lot less problems like I said this is my footprint so I'm going to open this window over here or this menu this is your feature tree that shows all of your sketches origin your your components your bodies your mates I'm sorry joints there mates in SolidWorks joints in this program so I'm going to click twice on sketch one and rename this footprint and in my footprint I want to show the overall size which is what I already have here but I also want to show the overhang so l4 line and up here I'm gonna have I'm gonna make sure that X is showing and that's going to constrain to this line and I'll draw a vertical line down here and as you can see this square popped up that means if I let go or click it'll change it to perpendicular that Square means that this line is perpendicular to this one that icon you can come over here and see perpendicular so that's this line it doesn't necessarily tell me where it's at in in this direction so deep dimension that lines already selected and I'll say from there to there is 0.5 inches that's my overhang our 4 rectangle and after the overhang this is where my leg is going to be 1.75 tab 1.75 enter again you can can set up parameters and all that - you know leg thickness or whatever one roll in 3d modeling as my dogs bark one more role in 3d modeling is never draw what you can copy okay it's always faster to mirror things to copy things to make rectangular patterns I'd never draw what you can copy so in this case I'm going to mirror this leg over to this side and then mirror both of them up to here and I need a mirror line so if I go are for rectangle and draw a two point rectangle from the center of a center point rectangle to the outside corner of that that gives me two mid lines now before I click I'm going to change that to construction so it doesn't change my my overall profile there I'll select that so it's constrained to the center it's constrained to this corner and we have horizontal and vertical constraints everything's black everything's good that means I can go to sketch mirror and use a window to select that overhanging or that overhanging line and this square over here and say mirror line right there press ok it mirrored over to here now we have this icon this is a symmetry icon no matter what I do over here it's completely updated right there if I change this to 10 it's going to change that one because this is symmetry based upon this line of this object controls need to back up now I'm going to go to 12 o'clock to repeat my last command instead of going up into the menu and I want to say this Square and this square lets mirror that along this line press ok everything is black everything is fully defined I have the location for all of my legs and I have the overhang on either side to create a 3d body out of this or component I can stop the sketch create a new component and then go to push pull or extrude and do that way or any time you're in a sketch if you go to one thirty on the clock wheel that is press pull so let's select that one and let's go in this direction let's just change this to 13 inches already that that's what I needed and there's a lot in this menu I'm going to get to in just a second but on this one all I want to do is change the operation to new component I want this to be my leg press okay now as you can see it got rid of my sketch because I created something from it anytime you do that it will get rid of that sketch if at first you don't turn the light bulb on so I'm gonna manually turn the visibility on with this light bulb and I'm going to double click on this component and rename it leg I could have when I created this oh here's something else that's cool you have history down here in the bottom left corner is your history you can roll back and see everything that you've done in your history and you can also double click on in each one and edit it so I can edit this this leg I can even say I'm gonna make all four of the legs but I don't necessarily want to make one leg component with four bodies inside it because if I update one body it's not gonna update all of them I'm gonna hit cancel here rather if I make copies of this and then update this component it will update all of those copies I'm not even gonna do that I'm gonna get this one completely done and then just mirror it so let's see where I was at oh also on sketches if you right click up here on your sketch and say show dimension all of your dimensions from that sketch will pop up and you can double click and edit those say 24 without editing that sketch you can update them on the fly and once again because everything is fully constrained fully defined everything else that was based upon that sketch was updated so this leg was moved into position control Z go back up alright again never draw what you can copy or never draw what's already there so I have the profile for my top but it's just not in the correct location that's that's that's fine no problem at all let's go to press pull and use a window to select all of this profile that I want down here on the bottom and instead of just you know setting this to 3/4 of an inch let's change this to new component instead of setting this to our material thickness for the top which is 3/4 I don't want to do that because it's it's not in the correct location so let's change this back to 0 so we can see what's going on where do we want to extrude from or press pull let's start from an object not from that profile plane what object we want to start from the top face of this leg that's what we're gonna start and it's a kroff design so I want half of an inch gap between the top of the leg and then the bottom of the top assembly so if I go to offset I can change this to 0.5 the direction is one-sided we can see the arrow going in the appropriate direction if by chance this is going down you just type in a negative value for your distance and it goes the other direction the distance 0.5 inches and this creates an operation I'm going to change this to new component a new component that is 0.5 inches away from this face up here press ok I'm going to change this component by clicking twice to top now again with this history based modeling because this was based upon the location of this top face I can go back over to here and change the height of this leg just just to show you 2 inches press ENTER and see what it did it everything is based upon this top so everything updates that's parametric modeling is fantastic I love it control-z to back up all right at this point we can let's see we can work on the bottom or the top and I'm just gonna go with the top so let's hide it this footprint sketch let's click this face right here and go to 6 o'clock to create a new sketch our 4 rectangle from this bottom corner and I'm just gonna go in this direction I can't automatically constrain to this bottom quarter automatically off of a sketch so I'm just going to drop it press escape and select the bottom point of this line hold shift or ctrl to select this bottom point on the component and say that those two points are coincident coincide and how are we pronounce it and that brings this or turns this into a black line because it says that this line exists exactly right here based upon those two points this one's blue because I don't know exactly how much it is in this direction what I want to accomplish with this sketch is to create a thickness profile for the bottom side and the top side of the top box as well as the vertical side vertical side and vertical divider so I'm just going to offer act we'll draw some rectangles in here off of this corner down to this bottom line off of this corner down to this bottom line one somewhere in the center doesn't really matter and then one from this corner over to this side and one more once again from here to here D for dimension and I'm going to set a first dimension of let me back up this one because I started at this point I don't want to do that just yet I want to show you something so I'm gonna back up and redo that last rectangle off a rectangle I'm just going to say up here somewhere to this bottom corner gain for dimension now I'm going to set this dimension between these two at 0.75 inches again I could use material thickness whatever I wanted to do here as a parameter but just to show you I'm gonna set one at 0.75 wait a minute so this I just noticed I set the wrong height here some of you may have picked up on that this should be this thickness of this component should be 0.5 inches so I don't know if I can do it inside a sketch can't I let's double click extrude the top nope I have to stop my sketch first let's go back to extruding the top I did type in the wrong distance that distance is point seven five something we may have caught that brush okay now let's go back to the sketch and double click this icon to edit it so now my point seven five should line up perfectly with here again I could set a parameter here to material thickness and I would not have to worry about things lining up but I'll cover that in another video in this case I just want to show you how you can link within sketches so this is my material thickness but every single one of these is the same thickness as well so I can go deeper dimension from here to here and instead of typing in a dimension I can hover my mouse over here and it says d13 I can either type in d13 or I can just click on it and it'll type for me d13 I'm actually gonna select that and copy it really quick but if I type this if I put d13 and press Enter it says FX 0.75 this means that there's a function here this dimension is equal to this dimension over here if this one changes so will this one so I can say this to this control-v to paste enter same thing this one to this one control whoops that wasn't the right one ctrl V to paste diva dimension from here to here ctrl V to paste so that means if I edit this one to say I don't know one every one of the other ones will edit as well control Z to backup so I still need to add a couple more constraints or dimensions to make everything fully defined diva dimension in between here and here is 4 inches that's my drawer height I can change my drawer height and any time and everything else will update and now I want this one to be perfectly centered there's a couple different ways you can do that but we can just go elf align and change this to construction and wait till we get on this line the triangle the pop up that triangle means it's the midpoint I say midpoint from here midpoint to there midpoint from here midpoint to there and then escape select this one hold shift select this one and say that those two lines are equal and if they are equal then this one's perfectly centered now everything is black everything is fully defined we're good to go I can start pulling parts out of this I can go to 134 press pull and I can say that all of this is my top but remember never involve what you can copy it's easier to copy things so I'm gonna hit escape and just just stop this sketch really quick I am going to use this sketch to locate this though so this is a component I'll go to 730 which is move slash copy I'll change the object to components I'll select this component and I'll say the move type is point to point so from this point to this point I want that to move but I don't necessarily want to move the first one I want to create a copy press ok now what this does is it puts another top in the exact location that I want it to but these are copies so if I cut dovetails on one it's going to cut dovetails on the other copies of components if you copy bodies you're not gonna have that relationship so just to show that if I extrude this face you see the bottom one updating as well it is a copy of oh I hit my microphone sorry it's a copy of a component based upon that sketch now let's create the vertical sides by going to 134 press pull and use a window to select those right there I know that my dimension this way let's change the operation to new component I don't want to mention right there is 19 inches and I can just type in 19 inches but never type something in when you can select something else on the on the project that you need it to stop at so if I just for example let's type in 19 and leave it there and then change the footprint my width on the footprint which establishes this size to 14 then these are based upon that footprint sketch it's gonna update the 14 of this one's based upon the number that I put in it's gonna stay at 19 I want this to update as well so instead of typing in a dimension I will say the extent I don't want to say a distance and said to object what I want what do I want it to stop at I wanted to stop at that back point I can't select any point over here doesn't matter it's always normal to this sketch and new component press ok this new component I'll click twice and call this side as you can see I lost my sketch again so let's turn on sketch 2 and it's actually rename that box that's the top box so this side component let's go to we can select it or whatever and go to 7 o'clock which is move copy the component that I already have selected and point to point select from right here to right here create a copy but now we have a problem if I do it in this manner the inside face over here is going to now be the outside face over here because it's just a directional copy that's a problem because I'm going to be cutting the pins on the top of this board sometimes it's not a problem in this case it is we're cutting the pins on the top and bottom of this board and pins are directional the outside face needs to be the outside face over here it's gonna change sides so instead of simply copying from one side to the other I'm going to take advantage of the fact that my my original sketch was centered about the origin so instead of point to point I'm going to select rotate so my selection is still over there that the component and the axis is this Center axis with the green now the angle I'm gonna rotate this around just to show you actually it already created a side I did not want it to so let's hit cancel let's back up our history over here actually just selected that one and delete it you should not have created that copy right then so let's go to move copy once again select my component and I'm just gonna select this side and select rotate this is the center axis I want to rotate along and I can show you as I just move this around you'll see what's gonna happen if I go 180 degrees it's gonna put it on the other side but the outside face is still the outside face so that's what I want I want to rotate this 180 degrees and I want to say create copy press okay now you see it says side one side three that's because that's the third instance of this copy I just deleted the second one I don't know why I added that it was an accident but what this does is if I go to e for extrude this outside face you see if I if I modify the outside the outside over there gets modified so that's the position that I want it to be in I'll press escape to back out of that one last thing from the sketch is this center divider so let's go to press pull once again use a window to only select this and again change the extent to object and select an object in the back side over there change the operation to new component press ok the new component I'll click twice and call this man I can't think right now vertical divider that's the center this sketch I'm pretty much done with so I'm going to turn that off and now I can do all of the joinery and I can do every bit of the joinery the dovetails and the details the pins 1 2 3 4 those joints plus mortise and tenon 1 2 all based upon one sketch very handy and very cool so I'm gonna select this face go to 6 o'clock to create a new sketch and I know that I'm going to be doing some mirroring in two different directions so let's just go ahead and you are for rectangle change this to a construction from the center which is already based upon the origin here to this bottom corner over there again everything's black fully defined now I'm going to just draw one dovetail press escape let's see turn construction off l4 line and let's just draw one tail from here to here from here to here nothing really matters at this point from there there from there to there d4 dimension let's just say that this is I've already established three inches will work I'll just type that in d4 dimension and from here to here 75 degrees that looks appropriate but these are not identical I can cure instead of typing this out as that same angle and all this and centering everything about amongst the center line it's very easy to select this hold shift select this line and after I have two lines selected that I want to be symmetrical then I select the mirror line and then type click over here to symmetry so there you go when this angle is changed to meet this angle and then they're also similar symmetrical amongst this line they're perfectly the same distance that means three inches is already established one and a half inches from here to here everything's black everything is fully defined that is one tail so now what I'll do is I'll put a sketch and use a rectangular pattern this is it's such a cool tool in both sketches as well as you know three-dimensional stuff so the let's let's select the objects first use a window to select only those and it gives me two arrows here and I don't know which is which based upon these two which is the left and right which is up and down so what I always do is I just drag in the direction that I want and see which one updated this one updated so this one is my up-and-down direction now I'm going to zoom out just a little bit and drag all the way down here and that spacing actually looks really good but if I was to want only the start and stop I can also uncheck any instance in between but I can also say that I want this to be symmetric I want to be amongst both directions so that's that's three that's I want more than three obviously let's add four and it puts two on bottom one on top let's select five that looks good seven inches looks good as far as the spacing this gives me a pin in the middle that is smaller than the outside half pins which I actually like that creates a half pin on the outside that is a little bit stronger and it keeps this this pattern here this dovetail pattern kind of enclosed to the middle of the project it visually breaks up the outsides I like that so I'm good with that spacing I'm gonna press okay now I also want to modify to mirror all of this to the other side no sense in drawing it again so let's go to mirror and select all of this mirror line right there press okay and all of my dovetails are taken care of now both sides I want to do three mortise and tenon joints through mortises right in the middle where this vertical divider is and I can see the vertical divider sticking through so I can actually just click and constrain to it our four rectangle from here to here and from here to here D for dimension I want this one to start I guess 1.5 inches away I'll probably change this as I build because I don't know what actually looks good as I'm looking at it but just for this model I will say that that is 2 inches and we will say that this one is 3 inches we will select this line holding shift to select that line and holding shift to select the symmetry line and select symmetry so that one perfectly centers and then also let's grab all of this and say sketch mirror mirror line right there puts one down there where I want it press okay this one sketch has all of the joints it's fantastic let's go to stop sketch and we can see it all right there I'm gonna rename this to dovetails and mortise and tenon now let's make some cuts so I want to cut the vertical pieces first let's go to press pull and I'm actually going to go to the top view and if I am cutting the vertical pieces first that means I'm cutting the tail so let's select tails I'm going to cut the tails away from the vertical pieces and I'm also going to cut away the shoulders of the mortise which is all of this right here all of that selected and I'm going to go again never type any distances starting from this plane and I'm going to go to an object which is the bottom side of this face right here if the material thickness changes then this cut will change as well operation automatically pulls up as cut objects to cut I do not want to cut the top all I want to cut is the side in both vertical dividers so that I can press ok now I need to repeat that command once again you can see that I already cut these and it's showing up on that one so let's repeat that once again let's turn on our dovetails mortise and tenon let's go to press pulse go to a top-down view select only the tails the tails and only these shoulders of the Tenon's and this time we're going to cut the bottom sides so let's go or where we gonna start we're gonna start from the top of this piece and we're gonna end at the bottom of that piece we're cutting what are we cutting we are not cutting the top which is a horizontal piece we are only cutting the verticals press ok one final thing we need to do with the sketch is cut the pins off of the tail boards so let's go to press pull once again go to the top view and this time we're only selecting the pins which are these we're only selecting the mortises which are these and once again these pins now remember this is a copy down here so whatever I do to this top one this top piece it's gonna update right here so I can do all of this in one cut so I'm going to go from the profile plane to an object which is the bottom side of this piece and we are going to just the horizontal top not the vertical pieces at all press okay and just like that if I turn off my dovetails and mortise-and-tenon all of my joints are cut from one sketch pretty pretty nifty the cool thing about fusion 360 one of the cool things is it has press pull as well as extrude and in Sketchup presspull is actually extrude or push-pull whatever it is there's only one so in Sketchup if I was just trying to try and exaggerate these dovetails by extending them a little bit all I would be able to do is extend these and vertical lines easily any way I could I could go in there and draw out all that geometry may be time-consuming or whatever but in fusion 360 I can use the press pull instead of extrude and say this this this this this my computer lags a little bit when I do this so it's gonna take a little there's gonna be some lag when I select those and we're gonna say these are gonna come out point one two five inches and it extends that same profile rather than extruding that rectangle and you can see the shape is still that is still consistent so one one eighth of an inch press okay I'm gonna go to this other side and do the exact same thing select that that that that that that that that and that and let's go with 0.125 enter I'm gonna do the same thing with the pins really quick let's go to a top-down view and let's say this this come on Mouse maybe I don't have to do a top-down view my computer doesn't like this select those like so I like the look of exaggerated dovetails it just it just looks really cool in my opinion not the mortises 0.125 press ENTER and we'll do the exact same thing on the bottom really quick grab this this this this this this and type in 0.125 enter let's go to my home view here so it flips everything around and now my dovetails are nice and exaggerated and it looks really cool I want to take this a step further and I'm actually gonna champ for every single one of these and if I was to do a chamfer and Sketchup holy moly would that just be time-consuming and crazy and insane not so much in this it's really cool it's go to modify chamfer and let's make sure we are on an orthographic view so we are looking dead dead straight amongst all of our lines and go to a front view now I can use a window to only select that and let's use a window to select that you'll see what I'm selecting in just a second if you can't already figure it out in your head here I'm only selecting the outside faces of the exposed geometry there so I select those and those and just that fast I'm going to put a chamfer on 176 edges and this is a full 1/8 of an inch they're proud of the surface by full 1/8 of an inch so if I just type in the point 1 2 5 it'll update and show me what that looks like I don't like I think there needs to be a little bit more of a step there so I'm just going to change this to about half of that point seven-five not quite half of it and 0.75 let's let's add a zero there so it makes sense there we go point zero seven five it looks really cool press ok so I'm gonna change back to perspective view I just think perspective looks more natural and looks pretty cool right so now we can work on the base for the base I'm going to add my footprint once again and because I'm going to I'm actually going to draw the rails based upon the start and stop locations of the feet on the bottom here so on this face let's go to 6 o'clock and draw a sketch this one is as confusing and and kind of crazy here but I worked out all the math so just bear with me I'm going to first l4 line create a construction line that is centered right here all the way down and just for consistency I'm going to draw it and drive one up I don't need one up as well but just for visual consistency and then our four rectangle and I'm gonna I'm going to make a rectangle like actually no turn off the construction off a rectangle a center rectangle based upon the center line here and I will just draw it like that let's grab this line hold shift and grab that line and say that those two lines the bottom side of the bottom is collinear I want that to remain right there my overall my overall height of this rail is three inches I do want an overall width of 0.75 inches and there's gonna be a kind of a crazy angle here before the actual rail starts that comes in contact with the top in contact with the leg so bear with me just a second this one makes make sense but this is gonna get confusing so I'm gonna draw a line even to mention the top of the rail contacting the leg is 0.75 inches away from the top of the leg and we need another our four rectangle Center rectangle on the centerline inside this rail this is going to be the mortise and tenon part deeper dimension from here to here is exactly 0.25 inches from here to here point two five inches this is all stuff that takes a little while to figure out but I've already got this in my head so I'll save you guys the the slow contemplating process here that's that's that's all good so now I'm going to draw another rectangle from here to let's say alpha rectangle another Center one on this and I'm going to draw it on to that edge up there this gets kind of confusing someone say that line and this line are collinear need for dimension from here to here is 0.125 and sketch an arc three-point arc that starts here this is basically trying to define the shape of this arc and goes there and if I drag it along this line you'll see a circle with a line on top pop up right here maybe you won't see it that circle in line on top says that is tangent someone drop that right there and from here to here circle with line on top is tangent that looks confusing but it makes sense in my head so let's go ahead and press pull everything is black everything is fully defined I'm going to start start the rail with the tenon joint so I'm gonna select the tenon that's the tenon profile where do I want to start I want to start this tenon profile from the outside of this leg because it is a through mortise and tenon joint and where do I want to end it I want to end it at the outside of this leg over here this is going to create a new component let's press ok let's rename this new component front rail let's rename that sketch we were just working on front rail let's also turn that sketch back on and we're going to add to this this is just a tenon that sticks all the way through now we need the actual profile of the rail so let's go ahead and create a new press pull let's select this geometry this geometry this geometry this added curve over here there's some more of it there's that and then there's that and all of that we want to start where the sketch is at and we want to go to an object which is the inside face of this leg that's not even there yet we're going to join this with another component it automatically decides which component you you want to join it to in this case it activated the leg I don't want to join to the legs so I'm going to turn the visibility of that leg off now it says we're gonna join it to the top I don't want to join it to the top let's turn the visibility of that off and then it says front rail so now we're joining it to the front rail that's exactly what we want two Tenon's already established let's press ok now let's turn those two back on so I can see what's going on and yeah that's the front rail but I'm not done with this sketch though I do need to make this this tenon I need to cut a mortise for it so I can do that from that sketch as well so on this front rail sketch we're going to press pull once again and this rail is in my way I can't physically select that profile however if I go over to the profile and then hold down the left click menu pops up I'll let go of the left click and then I can scroll through which one do I want and you'll see it highlight on the screen which one you want in this case this profile that's what I want to select and this way we're gonna go from that plane and the distance is to object what object we want to stop at this outside face it is a cutting operation because we are creating a mortise and the objects to cut all we're cutting is the leg we're just cutting the mortise and the leg not in the front rail press ok and now we have a mortise cut into this leg you can see by different profile faces here so that's that we're done with the front rail profile sketch however I do want to add a cutout so this angle right here right this this angled face this arc that's gonna be a cove cut on the table saw and I want a compound of that with another kind of Cove cut in this direction on the bandsaw so I'm gonna select this face go in this direction oh I'm sorry select this face and go six o'clock to create a sketch our four rectangle constraining to this point and then constraining to this top edge and then deeper dimension from here is that dimension is three inches and we're gonna sketch an arc I always want to say a four arc but in this program its appearance not arc so from here to here is my arc and I'm gonna bring it down to this line so it's tangent on this bottom edge never draw what you can copy so l4 line to create construction line based upon the center point of this rail press escape go to sketch mirror I want to mirror all of this based upon this mirrored line press ok press pull and I want to cut this and I want to cut this from the plane to the object which is this back face and I want to cut objects to cut should only be one yeah I don't have any options here so I'm only cutting this rail Oh sometimes I don't understand this part chain faces I'm not exactly sure what this does but sometimes you'll notice like yeah that that's what I want to cut but it's not it's not working with this operation so if you extend the faces I haven't quite figured out that or taking any time to figure out what it does but it changes this to make it cut objects to cut now we are only cutting the front rail press ok so now I have that compound angled curved compound angle curve compound curve I guess two directional curve so there's that the the front rail and this is the front rail arc sure we'll call it that I just need to make one more short rail this short rail super easy I'm going to grab this 6 o'clock to create a new sketch are for a rectangle actually l4 line to create a construction line based upon this center point our four rectangle and we're going to do a center rectangle we're actually going to do tool and one large one control-z to back up I forgot to turn construction off our four rectangle from the center up control ctrl Z to back up I guess it won't let me back up this construction for some reason let's just turn that I'll just delete it alpha rectangle from the center point there to there and we're going to do another one that is perfectly centered inside it and this one we're going to say this line and this line are going to be collinear I want the top of this rail to start where the bottom of this rail is defo dimension and this one is going to be a height of I think 1.7 five which I got the wrong one there let's just do this sometimes you got to do things in the right order it gets kind of crazy oh I see what's going on this Center one is constraining to this these diagonals let's just go ahead and delete that we will delete all of those points as well so now deeper dimension from here to here is 1.75 enter that looks more appropriate and I think that's the same distance right here 1.75 all right now my material with is 0.75 inches you know what I lost my Center constraint let's just back up and punt let's grab all that and delete it our 4 rectangle from these Center let's grab right here and say that D for dimension this is 0.75 inches this is 1.75 and now where do we need to go in this direction this line and this line are collinear I just botched that now let's do the mortise and tenon joint powerful rectangle our full rectangle Center rectangle from here and I'm not going to select these inside lines once again instead I'll just drop it and say D for dimension right here to here point to 5 inches from here to it's actually drag it on the inside and then say from here to here is 0.125 enter sorry that was way more confusing than what it needed to be now let's press pull and select just the tenon for the tenon we're going to start from an object which is the outside of this leg and we're going to go all the way to an object which is the outside of this leg and we are going to create a new component press ok this new component is the short rail I guess I should rename front rail to long real because I am going to mirror it and the back all right so this is my short rail tenon let's rename the sketch to short rail let's turn it back on let's go to press pull and let's add this profile around it and the distance is going to be to an object which is right there we're going to join it and again it's telling me to join to the leg I don't want to do into life so I'll turn the visibility of that off it gives me this rail so I'm joining it to the rail that's exactly what I want let's press ok so now I can turn the leg back on and at this point at this point I can start mirroring stuff I don't like this is one thing that I do not like about fusion 360 is mirroring mirroring components in my opinion should most definitely maintain all the property linking in between so how do we get this leg over here let me show you something if I m4 move and if I go to component we're gonna select that component point to point if I say move this leg to that point and say make a copy see what it's going to do it's going to create an exact copy of that component I'm gonna turn that short rail sketch off and if I edit this component it's going to edit it as well over here because it is a copy of a component let me go ahead and back up our history here that's what I want it to do however if I go to modify I'm sorry create mirror and I want to mirror a component this component mirror plane this plane press ok this in my opinion should most definitely be a copy of the component and it should update automatically it doesn't instead of just saying it has a designation here that this component is a mirror so if I edit this one it doesn't edit that it drives me nuts I wish that mirroring worked just the way you copy and flip and Sketch up if you copy a component and then flip it in Sketchup then that is essentially making a mirror and that maintains all of the features of that I wish that there was either a flip command or a mirror that key kept those kept those relationships but it simply doesn't so that being said you need to back up my history and I need to make all of the adjustments to the leg before I mirror it I can copy it in this case to all four corners using a few different methods because this particular leg is the same in both directions this outside this inside face is the exact same thing thing as the outside face it gets problematic though if there's different features that are based upon newer features in the model and you have to anyway I'm not going to confuse anybody here so before I do the mirror let's go ahead and create a chamfer top and bottom so let's zoom in here modify chamfer select only those edges select only those edges and type in point two five inches enter that makes the let it just sets the leg off looks really nice and now I can take this this leg and I can go to modify I'm sorry create mirror mirror plane right there press ok twelve O'Clock repeats these two components you know what I forgot I forgot the rail let's back up once again now create mirror which components this one and this one I want to select this mirror plane press ok repeat that last command components I want the front leg the front leg the front rail and this leg over here mirror plane this back one over here press ok so now everything is done that is the model and as far as speed goes once you get used to this pretty much the same speed and Sketchup as well as fusion 360 however I got a lot more options in fusion 360 so that's cool I'm going to press a for appearance and I'm using a 4k monitor and fusion doesn't scale windows that well so I'm being cut off right here but if I type in mahogany I'm gonna grab this one and then I'll select let's see I'll select the top top side side vertical divider and I'll drop mahogany on those because cannot be assigned at face level these are components vertical divider side side top and top I will grab unfinished mahogany and drop it off at these components and there you go now the leg short rail long rail short rail leg leg leg long mirror all the base all of that is going to be maple if I type in maple and I'll go to unfinished maple drop it off over here that's what I'm gonna use I'm gonna use mahogany for the top and maple for the bottom fusion 360 has a built-in rendering option that is fantastic and it gives you a real life view of what this is going to be so without getting too complicated here I can just set this in place where I want it and then go to render and this menu and change the lighting and all this and then just either right click and go to render or just just render in place and this may actually crash my computer but it's going to render everything and then eventually you can output an actual photo realistic image which I'll just display on the screen right now because I can't use fusion my recording software in render at the same time so there you go this video I think turned out a little bit longer than what I wanted but I guess that's a good little introduction to the walkthrough of my workflow walkthrough of my workflow anyway if you have any questions leave them in the comments let me know what you would like to see in fusion 360 would you like a full blown course on how to do a lot of stuff with the basics with some advanced stuff I don't know just let me know what you'd like to see fusion 360 is a fantastic program it's yeah I just like it a lot hopefully you guys can use this to your advantage take care have a great day and I will talk to you next time so I actually started editing the video and then I realized that I never did show the power of parametric modeling and Sketchup adding these sketches yes I did not go to input any parameters however all of my sketches were completely fully defined before I left that sketch that means if I go to update something it's going to update as well so I've got the footprint sketch activated and I right clicked and said show dimensions so now I can go back to my very first sketch the very first one and changed this dimension to say I don't know maybe I realized that I don't quite have 36 inches of available space let's just say we have 33 inches of available space instead of modifying everything that I've already done to reduce three inches from the total length by just type 33 press Enter everything should update and there you go everything updated accordingly because all of my sketches were fully defined and that is one of the very amazing benefits of parametric modeling so 45 inches the only the only thing that I didn't really do is on these dovetails I did a linear pattern rectangular pattern based upon a set and number so if I expand these out there's gonna be bigger pins I think that's going to be the case so let's go to i guess 25 inches for the width and at that point if it ever updates yeah these outside of pins I'll need to add another will add another feature in add another instance into that rectangular pattern if I want to keep that same three inches in width of course you can set that three inches in width with a parameter to update and blah blah blah but that is one of the very awesome benefits of parametric modeling you can when you're also when it's all said and done you can go ahead and make updates on the fly and everything else updates accordingly so anyway I thought that was a very important important of me to include that and let's change this down to nine and they were you everything updates accordingly I thought it was important for me to show that because I did mention it a couple times in the video again I want to drill it in your heads always make all of your sketches fully defined before you move on to the next sketch anyway that's it for real this time you guys take care have a great day and I'll talk to you later

Channel: Jay Bates 2 - Vlog and Non Project Videos

Views: 52,347

Keywords: jayscustomcreations, update, woodworking, jaybates, vlog, fusion360, fusion 360, krenov, coffee table

Id: J22j8RfETjs

Length: 55min 32sec (3332 seconds)

Published: Fri Feb 23 2018