360 LIVE: Lofting to new heights

hello everyone and welcome to another fusion 360 tech Thursday my name is Brad talus from Autodesk and wanted to welcome you to today's topic we're gonna be talking about lofting I'm gonna be showing you how I went about creating this part here and this is actually from a mostly printed CNC machine let me bring up a picture of it here in fact one of you on the live stream in a previous livestream mentioned this and I'm like okay I got to make one of these so we're actually going to be creating one of these feet you can see here in this image so let me jump back in here I also have helping me out today Aaron is helping me with the chat window so if you have any questions or comments please feel free to throw them out there what I want to talk about today is how do we go about creating this particular shape and you'll notice that it's kind of curved here from the side and it starts out as a square in the bottom but it ends up being a circle on the top and you might think well maybe you could just revolve a shape around but because it's square on the bottom and round on the top we're gonna have to use the loft command so let's dive right in I've also included the drawing in the description of this live stream now this isn't the most perfect drawing I just kind of whipped it out pretty quick but hopefully there's enough information here to allow you to try and recreate this particular part okay so the first thing I'm going to be in millimeters so I'm going to confirm that I'm in millimeters which I am and then I'm going to start by creating a component so I'm going to click on the new component and by the way I'm using the latest version of fusion 360 we just had a new update come out I'm loving it it's great so if your screen looks slightly different than mine it's probably because you have updated yes so I'm gonna create a new component and let's just call this bottom corner is the name of the part now why am i creating a component I'm only doing a single part right now but down the road I might want to include this in an assembly you know why I bring all those parts together so that's why I created it as a component so okay then I'm gonna start by creating a sketch and I'm gonna do the top plane so I'm basically going to start by drawing my rectangle so I'll click on the rectangle command and if you don't know this already it puts the options are the different kinds of rectangles over here in your sketch palette so for example if I do c4 circle you'll see all of the different kinds of circles here so our four rectangle I can see my two point three point and Center I'm gonna go ahead and do a center rectangle now all of the dimensions I'm typing in I'm getting off of the drawings and I'll switch back and forth between the drawing every once in a while so it says it's it's fifty three millimeters square so I'm gonna go ahead and type in 53 in both of those and we can see that it created a rectangle now just for your reference right here it says 53 and I put the little square icon so that means it's 53 in both the horizontal and the vertical dimension now in a previous live stream I mentioned that I keep my sketches fairly simple for example I don't do fill it's in 2d i do fill it's in 3d but in this case we're actually going to be lofting from one profile to another and so I need my profile to look the way I want it to be before I do the loft command so I am going to actually use the Philip command so I'm going to say fill it I'll select my two lines and the Filat according to the drawing is seven millimeters and so I'm just gonna hold down my control key and kind of continue clicking around and of course I get a phone call let me go ahead and select these other lines here so I'm doing a radius seven all the way around and now I'm done I'm gonna finish my sketch so what we basically did there was we drew the overall shape of the bottom so you can kind of see how it's a square bottom with fileted edges the next thing I want to do is draw the shape of the top which in this case is just a simple circle which is 35 millimeters in diameter I'm not going to worry about the hole through the middle quite yet we're going to come back to that I'm basically building the the overall shape okay so I need to actually let me jump back to the drawing sorry I need to draw this circle at the correct height and we can see here that the overall height is 40 millimeters so I need to create a sketch that's 40 millimeters from my rectangle so to do that we're going to use a construction plane and the very first one is called offset plane I'll do the offset plane allows me to pick a plane and then I'm just going to start to drag and you can see how it's basically going to create another piece of paper that we're going to sketch on at a particular height and in this case I want it to be 40 so I type in 40 and say okay and if I expand open my component here we can see our sketches and we can see this construction okay so then what's cool about this is I can just select that plane I just click on it once right mouse click and it shows me the commands that make sense I could create a sketch on that plane or I could offset another plane from that but in this case we're going to say create sketch and I'm gonna draw my circle now I started at the zero zero because this is going to help me out I'm just gonna go ahead and click there and now I can type in my diameter of 35 and if I wrote if I say finish and rotate we can see that that circle is now above this other sketch okay now I'm going to talk about the loft command but you're gonna see some issues happen and we're gonna come back and continue with our sketch but under the create menu I'm gonna pick on loft okay what this allows you to do is to specify which profiles you want to loft and you'll notice as I get near this profile it kind of highlights I'm going to go ahead and click on that one and then I'm going to go ahead and click on this one and you can see that fusion did what I wanted it to it took this square shape with rounded corners and it moved it up or lofted it to this circular shape okay now the problem with this is if I look at it kind of like from the front it just went in a straight line and in our example it's got a curve to it we've got a nice transition and in this case we don't see that and that's why we're gonna actually have to add in some guide rails and what this allows you to do is actually tell it go from one shape to the other but follow a rail kind of like a train has to follow a train rail the loft is gonna have to follow that rail okay now I'm gonna show you some cool commands in here up here at the very top you can see the different profiles and it says connected but I can also say Direction and notice what we get we're actually kind of controlling the weight of this loft so I can sort of simulate that curved surface so if you don't really care too much about the exact shape of this you just wanted to go from one shape to another and kind of curve you can use direction instead of connected and basically what you're doing here is you're specifying how tight of the weight is that so you can see it goes straight up for a long time before it finally starts to curve over that's because we have a pretty strong weight right there but if I bring that down you can see how it curves a little bit smoother okay I can do the same thing with a second profile I'll say direction and we get this is kind of the same result you can kind of see how we can change the weight of this and make it go from the square quickly to the circle so that's what those options are now in this case I'm going to leave it connected and we can see that it's going to keep that straight edge which is not what I want okay so we're gonna create some guide rails so I'm gonna cancel out up here and basically what I want to do is to specify how they're gonna loft up what rail is it gonna follow so I'll go ahead and create another sketch and let's just do it maybe on this front plane right here and I'm gonna use a spline for this now if I get near this line you'll notice it catches to the line but it doesn't catch to the end point and I want to be very specific to catch to the end point of these okay this one it does but on this one it doesn't so we're gonna project some geometry so I'm going to come in here and say project I'll click on this edge here and I'll click on this edge here and say okay and now you can see those little round icons and what it basically did is it projected the very edge of the circle onto our piece of paper so you can kind of see the kind of turn it from the side there you go okay so I projected the sketch information on to my new sketch and now if I get near there you can see how it's gonna snap to that corner and that's exactly what I want okay so I'm gonna click maybe one point there another point here and then finally down here to kind of define the curve and when I'm done and I click that little green check box let's just zoom up a little bit you can see when you create a spline it shows you the end points which are these black dots and then you also see these green lines and these are our tangency weight and our tangency Direction okay now I want this to go basically straight up from this edge I'm going to purposely make it kind of at an angle here so I'm going to click on that tangent c line and click on horizontal vertical and now you can see that that tangency line is straight up and down so it means the spline is going to come straight up and then start to curve okay so I have the shape the way I want and I could come in here and move this point around I could tweak it a little bit but I like the way it looks right now actually and I want this to be on the other side so I'm gonna use the mirror command so I'm gonna say mirror it's asking for the object but now it's asking for a mirror line and you'll notice I don't have a line that I could mirror around if I did this one it would kind of flip up so I need to create one that's on to this you know basically the vertical line here so let's go ahead and create a line I'm just gonna get near this center point here and you can see it creates this snap guide it's kind of hard to see but there's a cyan line right there so basically saying I'm lined up perfectly with that point and I'm just gonna do the same thing here I'm just going to kind of come up above and click so basically we're going straight through the center of this part now I don't want this to be an actual object line so I'm gonna click on it and say construction I apologize I have my email and everything turned off but for whatever reason an email popped up and I see people like what was that that was an email so I apologize not sure why that showed up okay so I I turn this into a construction line you can kind of think of this as a light pencil line we don't want it to be an object line like a circle or a rectangle we just want it to be a reference like a light pencil line now I could come in and say Mir what's the object I'll say this line here what's the mirror line that guy there and we can see that sure enough it's gonna mirror this across I'll say okay and you'll see all of the icons saying that they're you know we've basically a mirror of each other I'm gonna say finish my sketch and we can see that we now have this guide curve on both sides of these circles now I'm gonna do the loft again and show you an issue so I'm gonna say let's create a loft what's the profiles these two are my profiles and we get that nice straight representation but this time I can come in here and say I want to add in a guide rail so I'm going to click on this curve right here and watch what happens it's kind of interesting in fact let me look at it right from the side here so it's taking that shape and following it up this rail right here and that's exactly what we want but you'll notice this little kink right here and that's because it's having to kind of pull the profile over as its lofting up so you can add more than one rail so I'm going to add in that second rail and we can see how it's gonna follow that and it's gonna follow that there however if we look at it from this it's more kind of a straight line so when you're creating lofts and you want to follow a very specific profile or path sometimes you might actually need to create a path on every single side so for example four sides because of this square shape again it kind of depends on what you're creating if I was creating for example like a whiskey bottle you know it could be just an elliptical base with a round top and I would just have one guide rail kind of showing the the side of the bottle for example but in this case I need to actually add in some more curves here now here's a neat trick I'm gonna go back to my sketch and I don't have any dimensions on this anything like that I just went basically by the shape now it would be very difficult for me to recreate this spline on another sketch because who knows where that point was or anything like that because I haven't dimension it so what I'm gonna do is actually just select these lines right mouse click and I'm gonna say copy I can actually copy sketch entities so I basically copied that into my clipboard now I'm gonna come in and create a new sketch oops didn't mean to do that I'll say create a sketch I'll say on this front face here or the side face I should say and then I'm just gonna right mouse click and say paste now in my case that came in kind of upside-down for whatever reason not sure why but I can rotate it now here's the catch notice where this little icon is where it's going to allow me to rotate it and it's gonna rotate around that point well I want this to be very precise so I'm going to have it around the Centrepointe because I know that's symmetrical so I'll click on this set pivot click on that point and you can see how this little Triad moved from over here to right here now the one thing if it remembers when you're done with that you have to say hey I'm I'm done I've set my pivot so I'm going to click on the checkbox and you can see how it goes away but now when I rotate it's actually going to rotate around that middle point right there and I say rotate 180 degrees I'll say ok and we now have the exact lines all the way around so I'm gonna go ahead and finish my sketch and we can see how I was able to recreate so I basically drew one of them and then mirrored it then I selected both of those copied it and then pasted it onto a new sketch and a totally different orientation so now I know that those are correct so let's go ahead and do our loft I'll say loft our profiles I'm gonna add in some rails here so let's say this rail here that guy there let's rotate around and sure enough we can see how if we hadn't added these it it wouldn't have matched but now I can come in and add that one and that one I'll say ok and I've just created a loft from a square shape to a circular shape okay and it's nice and smooth you can kind of see how it's blending the the fill it out into you know this large circular area here so we get a really nice representation in fact I probably should have shown this at the beginning but I've already 3d printed it so we can kind of see this is what the the final product is gonna look like and so now what we're gonna do is we're gonna start adding in some of the details like the the holes and the slots etc okay so the next thing I might do is put the I put the major stuff on first so there's a big hole that kind of goes through the the middle of this so let's create a sketch on that top face circle command and again because I started kind of at the origin everything is symmetric off of this so I can select that middle point and this is 22.5 I'm sorry 23.5 according to the drawing okay now in some of my previous live streams I've talked about sketching and I've gotten questions in the chat and follow-up emails where people are like do you sketch everything on one plane and do a kind of a complex sketch or do you do multiple sketches and I personally like to do kind of the multiple sketches and we might run into a situation in this example and I'll show you why I like to do the multiple sketches so you know I could have you know put this circle on my original sketch that was on the bottom and then extruded it up but I don't know I kind of like to keep these separate sketches so that way I can go back and find them easier so I'm gonna select this and say extrude and I'm gonna start to drag down now here's a neat trick okay how far do I need to go well according to the drawing it's 40 right so I could type in minus 40 or I could just hover over this face right here and you'll see that it says snap to minus 40 so if I were to click on that face right there I don't even have to rotate it actually knows you're trying to go to a planar face you'll see that it'll snap to that minus 40 or what I like to do is instead of saying distance I like to change it to all and what that's gonna do is go through all of the part and what's nice about this is if I were to come back and change this in any manner like change the height for example it's always gonna go all the way through the part whereas if I had said only go 40 and then let's say we added five more millimeters down here it wouldn't have gone all the way through so this is another tip I personally recommend selecting all and there you can see how it's gonna go all the way through okay okay the the next thing I want to do now is maybe start working on kind of the slot feature right here so according to the drawing that slot sits on a shelf about 5.5 millimeters up from the bottom so again we're going to use an offset plane so I'll come in here and say offset plane I'll grab that bottom face and we're gonna drag up a little bit - 5.5 and it just created a plane that's exactly five and a half millimeters from the bottom of the part okay let's go ahead and sketch on here and I'm just going to draw basically one of these so again using the drawing I'm just grabbing some dimensions off of the drawing but I want to be very precise I want to be exactly in this corner so again I'm gonna create some geometry that's gonna help me out so I'm gonna just start with a line and I want that to be at 135 degrees I don't care how long the line is I just wanted to make sure I'm basically 45 degrees from the center again I can select on it and click on this little construction icon right here and it turns it into a construction line instead of an actual object line okay then I'll come in and start creating my slot and I'm going to do a center to center slot I'll just get kind of near this edge here click and click I know the overall diameter is 4.85 and I purposely you know created this a little bit larger than it needs to be in length the diameter is correct I got that off the drawing now I can come in and start to tie this thing down so for example I know the distance between these two points let's go ahead and place my dimension is two millimeters so we can kind of see how this slot got smaller and then I also know to know that from here to here is 25 millimeters printed it up pretty small 26 millimeters I need my glasses 26 millimeters and so you'll see how it moved that slot into the correct location so again I just kind of get it on the line where I want it I don't really care about what size it is then I can come back and start to tie it down with some dimensions there's also a larger slot that kind of goes around that so I'm going to do the slot command again Center to Center and now I know I can click those two points and in this case the diameter is according to the drawing 14 and I'll show you where I got this from and there we go we can actually see that this overhang is slightly but that's actually how it's designed so how did I do this so basically I used this detail view right here so we could see that it's spaced two millimeters apart the diameter of the slot the slot is four point eight five and the diameter of the larger slot is 14 and we can see that it's 26 millimeters from the center of the circle so that's where I got that information from so I'm only going to do one of these I'm actually done with my sketch okay so let's take a look at this and I want to extrude this smaller slot all the way through the part so I'm gonna I'm gonna go ahead and try and click on it and you'll notice that it's kind of buried by my part so it's trying to grab you know this front face first so I've shown this tip a couple times now but I use it all the time I absolutely love it if you click and hold for about a second you'll see that it allows you to kind of probe through so the very front face then it's like I almost like a laser shooting through it so the first thing lasers gonna hit is the front face then the profile and then the bottom face so again all I have to do is just click and hold with my left mouse button for about a second I'm gonna grab that profile I'm gonna right mouse click because all of the commands that make sense they're at my right mouse click so we can see I could extrude this so I'm gonna say extrude and I'm gonna start to drag now I want it to go through both so I'm gonna come in here and say symmetric and instead of distance I'm gonna say all and notice what it does it goes a certain distance in one direction in a certain distance in the other direction to go all the way through so again that all is a very handy command and obviously we want to cut so I'll say okay and we just created that slot that goes all the way through our part now you'll notice my sketch disappeared but it's very easy for me to come back in here and just turn that back on in fact you'll notice I usually have my sketches and my construction folders kind of unfolded so I can see and get in there very quickly okay so now I want to do the same thing with this larger slot so I'm going to click and hold and pick on the profile I'm also going to select this inside profile here so I'm basically saying I want to remove all of this material now I don't have to do that but just for me personally it's confirming that I'm gonna be cutting everything away I mean for example what if our extrude had a 1 degree taper or something like that it would create these weird slipper phases but in this case I'm saying remove this whole region this whole area all at the same time so right mouse click and say extrude I like to start to drag we can visually see that sure enough that's gonna cut some material away how far let's just say all again and it figures out how far it needs to go to go all the way through the part and I'll say ok and sure enough it removed all of that geometry I'll turn off my sketch and we can see that we got that kind of neat little pocket area now I only did one of these and I actually want to pattern these around but I'm actually gonna add in a small Filat so let's go ahead and say fill it I'm sure I want to make tangent chain I'm just gonna grab that edge there and according to the drawing it says all Philips are one millimeter unless otherwise specified so I'm going to type in one millimeter and say ok now you might be saying well I've watched some of your previous live streams Brad and you said you know save your Philips till the end you know do the major stuff first and then do the minor stuff at the end but what you're going to see here is we're actually gonna pattern not faces but we're gonna pattern features so we're gonna pattern the slot the big huge extrude and the fill at all at the same time so it's gonna save us some time in the long run so check this out I now have my finished corner here I can come in and say create a pattern and I want to do a circular pattern and right here you'll see by default that's usually set to faces and I could have come in and elected all of these faces but I run the risk of missing one or making a mistake okay so I typically like to pattern features and features are what's in your time line so for example I could pattern of the fill it I could pattern that big extrude and I could pattern the small slot all at the same time so I actually selected all three of these features in fact you see it says three selected what's the axis will select this cylinder as the axis and it gives us a preview by default it's set to three now I wanted to change this to four so I'm going to up that to four and now you can see how it's gonna go in the corners however according to our part here you'll notice that there is not one in this corner here where the slot is so we're actually going to only have three but there's an option in here called suppress and you'll notice that it's checked and all of these have a little checkbox next to them so I can come in here and uncheck one of these so we're still patterning for quantity but we're only going to display three of them I'll say okay and very quickly we created these little slot pockets all the way around the part except for over here where we're going to do the nut and bolt where it kind of connects so that is why I actually did the fill it before I did the pattern so we were actually able to pattern that philip feature also kind of handy okay hopefully this is making sense and in your learning stuff I can see lots of questions in the chat and Aaron's busy typing away so I appreciate your help there Aaron the next thing I want to do is to create basically this this region right here so what it is as a screw is gonna go through there and be tightened down by a bolt and it's gonna pinch onto some circular tubing so we can kind of see that it's gonna be about fourteen millimeters wide and we can see that and the drawing the hole that goes through is point I'm sorry three point seven five now what's gonna be interesting is I put a dimension here that says seven millimeter diameter coincident with edge but I also threw a dimension here and this will make more sense once we get creating this but I want this hole to be in a very specific location but I also want it to be you know coincident with this edge here so let's go ahead and take a look and if I turn on my origin we'll see that I don't have a plane that's in the correct direction I need to be going across here somewhere okay so I want to be able to create a plane so I'm going to come in here and say plane at an angle but this requires through an edge or an axis okay so I'm not coming here and say axis through a cylinder so I'll go ahead and click on that cylinder and you can see how I'll put a line down through there I'll go ahead and say okay now I have a line that I can select plane at an angle so notice how it's asking for a line I can click on this line and sure enough it's gonna put a plane through that line but I can specify what the angle is so you can see how we can rotate this plane let's just go 45 degrees so we're now slicing through our part at 45 degrees and that's exactly what I want to do here I'll go ahead and create a sketch and you can kind of see our part looks a little bit different because we're looking at it kind of in a orthographic you know direction now here's another tip I want to project some geometry so I'm gonna say project and I want to project this curve right here but you'll notice when I click on it it actually does not project that edge okay it projected the top and the bottom and some of the other geometry but it doesn't project that edge and that's because of the direction that we're facing here so I'm gonna undo and show you instead of project here we're gonna say intersect now let me show you before I do that what's going to happen so this piece of paper is slicing through our part right here okay and I want to come in and say project intersect and notice here it's asking for some geometry so I'm going to go ahead and click on this geometry and you can even kind of see the preview there it's going to project the whatever's intersecting through that plane and now it did create that edge because I used the project intersect so very handy command most people use project works in a lot of situations but in this case intersect is actually quite useful okay okay so let's go ahead and let me just look at it straight on I'm gonna go ahead and draw my circle here and I'm just gonna draw it out here in space a nice start to drag it into location so I know that this is three point seven five and then there's a larger circle that goes around it and it is seven okay and then I'm just gonna get this sort of where I want this to go something like this okay now I gave a measurement of ten point five down but I also want it to be a coincidence so what I'm going to do is to create a point and you'll notice I can create a point on this line so I'm just going to click somewhere on that line and that point is now on that line then I can come in and say I want my circles and that point to be horizontal with each other so now watch what happens when I drag this point you can see how the circles are staying in line with that point and my point is staying on that edge which is kind of handy okay and then the last thing is I want this to be coincident with that point so I'll come in here and say coincident that and that and there we go so we basically know that this circle is cutting through this edge and it's in line horizontally so basically that this is like the center of the circle on the edge is what's happening here so let's go ahead and throw our dimension on here so I'll say from that edge to that point and that needs to be ten point five so watch what happens that point slides up the edge there a little bit but it still is coincident so I know that my circle is exactly where I want it to be and I know that was a lot of information there but basically I want this little tiny bulbs right here and I want it to be perfectly lined up ten point five from the top okay so I now have my sketch so again things are buried so I'm just gonna click and hold and we can see I can probe through and grab that profile and I want to extrude that profile I'll say symmetrically through all okay we can see how that's gonna extrude or cut through our part okay I'll say okay my oh my sketch went away but again just hit the little light bulb right next to it and now I want to start creating a little bit more stuff to be removed so I'm gonna click and hold this profile I'll grab this profile here also make sure I got both of those I'll say extrude and again I'm going to slice through now notice this is an object line so here's a catch this is an object line and so it did not grab all of my profile and grabbed a little part of it I need to grab that guy also and I'm gonna say let's go all in this case say okay so I'm basically building half of this and the reason for this is it's gonna be hard to see but I actually have I'll show it over here we're slicing through a round profile on one side and then we're actually going to create a recess for a nut to get trapped in there you can kind of see it in this preview here so we're gonna put the head of the the bolt through here and then the nut over here and it's gonna help keeping it from turning so I'm going to basically build half of this at a time so I use that profile of machine through and I grab the larger profile to give me that that bigger recess and then finally I want to add in kind of this section here to give it some meat to bolt against so let's do that again I'll come in here and grab these two profiles I'll say extrude and let's go to the left and according to the drawing it's seven millimeters so it's 14 total so I'm gonna come in here just say 7 millimeters like so and say ok and so I've created that side now this side over here I want to do that hexagon shape now what I'm about to show you is what I mentioned earlier on where I I said I like to do multiple sketches because sometimes your right might run into a situation where you don't get the results that you would expect instead of doing one complex sketch I like to do multiple sketches and what I'm about to show you is the exact reason why okay so I have a sketch right here and I'm gonna go ahead and say edit sketch because I want to add some more stuff to it so I'm gonna say edit sketch and notice what happened my hole has gone away now why is that well that's because the sketch is way back here in time so I'm down in my timeline you can see that there was three steps after this sketch so it's not showing me those three things and I personally like to see what my part looks like okay so let me show you what I mean as soon as I say finished sketch I see all of this information so because I came back and edited this sketch it's not gonna show the downstream features that happened after that sketch because we've gone back in time right okay so how do we get around that well I can just come in here and say let's create a sketch on that face and that sketch is now created after this other stuff and now I can visually see everything and again this is personal preference but I I kind of like to see what's going on here so now I can come in say polygon and I'm gonna do a circumscribed polygon I'll click here I just have to get near this edge right here for the correct diameter I'm just gonna go ahead and click and to finish my sketch okay now I can go ahead and notice also because this is on a separate sketch it's not bringing in the circle for me so it would have split this into multiple little sections so another reason why I like to do multiple sketches instead of one complex sketch so let's go ahead and extrude this guy actually you know what I'm gonna do here's a neat trick I apologize I'm getting ahead of myself here what I'm about to show you I think is really really handy and I haven't shown this in previous live streams but I'm gonna show how you can actually extrude from an offset so so check this out I'm gonna extrude this circular profile first of all so I'm going to click and hold to grab that profile and this profile here okay and we're gonna extrude that the seven millimeters just like we did on this other side so I'm gonna come in here and type in seven and we want to instead of cut we want to join okay now the interesting thing here is my hexagon shape is way back here we're gonna figure that I hate out here in just a second but I now have created this main shape now I want to extrude my hexagon profile but it's kind of in the wrong location but check this out and I say extrude and I'm gonna start to drag okay and I'll change this to all and you'll see that a little slice all the way through but I don't want it to destroy this whole region right here that I just created so that's where this start comes into play so you can see it says it's gonna start from the profile right there or I could say offset how far do we want to offset seven millimeters so what it's doing is it's using this profile but offsetting seven millimeters and then doing the extrude and this is a really kind of a cool trick like I said I don't know if I've shown this before but it allows you to instead of having to create another sketch on another face or whatever you could have a more complex sketch right here and then offset at seven millimeters and then do your extrude I'll say okay and we end up with this particular shape which is exactly what I was looking for okay so the last thing we need to do for this part is to create the slot that goes through it because it basically gets pinched together around you know some circular pipe so we can see that that slot is 1.5 wide so I'll just jump over here and you can't see it but remember we created that plane on this axis well I'm just gonna come over here and turn it back on again it's still there we can still use it so I'm gonna click on it right mouse click and say create a sketch now what shape do I need this to be well it can be as simple as a rectangle so for example I'm just gonna get near the center line here and just do a big shape like that well click on it will say extrude now I want to go symmetric in both directions so I'm going to say symmetric and I know that the overall length or the whole length is 1.5 so when you change the symmetric it gives you this measurement option of 1/2 length or whole length so right now it's a 7 1/2 length if I typed in 1.5 this is actually 3 millimeters right because it's going 1.5 in one direction and 1.5 in the other direction however if I change it to whole length you can see how that got smaller and now it's 1.5 for the whole length but notice how simple of a profile we used right we're just trying to create a slot through there so I just used a rectangle I'll say okay and we're pretty much done the last thing if you want to I could come in here and say you know fill it for example now these are 0.5 so I'm just gonna grab a couple of these edges to kind of help smooth the transition you know from from this part to the surface there or whatever and I could put a fill it on this top edge here if I wanted to you know one millimeter fill it oops type in one and a little blend on the top and I'll say okay and there we are there's my finished part not an overly complex timeline but we used the loft command to create that shape going from a square to a circle okay I'm going to point out a couple really quick things here let me let me jump into one of these sketches something we just added and I've noticed I've seen this in previous live streams is they wish that they could turn off dimensions well guess what now you can actually turn off your mentions so I should find a more interesting sketch or whatever yeah for example this guy here let's turn off the body so you kind of see what's going on I can come in here and turn off my constraints and I can turn off my dimensions so it really cleans things up so I don't know if you've watched Aaron's video where he talks about what's new in the latest release but if you haven't I highly recommend you go out and watch that I hope he's already linked to it because there are some really cool stuff in that video and I'm actually going to be highlighting some of that in upcoming live streams so with that I hope you found this livestream beneficial make sure you subscribe leave comments thumbs up thumbs down whatever you think let me know other topics you want to see I've been getting some emails from some people requesting some some topics of stuff I love seeing what you're all doing with fusion and I hope to see you on a future livestream thank you

Channel: Autodesk Fusion 360

Views: 54,818

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

Id: mhXDtfej-yc

Length: 55min 18sec (3318 seconds)

Published: Thu Mar 14 2019