Surface Modeling with Fusion 360

hey everyone fusion 360 evangelist Taylor Stein here and in this video we're going to be looking at the surfacing tools inside of fusion 360 and seeing how we can use them to create this bottle design so let's get started for this design I'll be using a reference image in this case a hand sketch to really kick things off under the insert drop down menu I'll choose attach canvas and select a plane to place my image on next I'll choose the image and you'll see that fusion 360 brings it in I'll scale it up so I can see what's going on and I can drop the opacity a little bit next I want to make sure the box for display through is checked this way if I have any solid geometry in front of the canvas I can always see it through anything that might be in its way I'll hit OK and now we can see that we have our sketch what I want to do is calibrate this so that I know it's the right size to do this I'll right click on my canvas in the browser and choose calibrate I can select two points on my image and enter a value let's say I want the height of this bottle to be around 200 millimeters I'll select these two points and type in 200 and my image is now scaled up the last thing I want to do is position the bottle on the origin properly I'll show my origin and you'll see that it's right in the middle to move it up I can right click on my canvas choose edit canvas let's move it so the bottom is on my bottom plane that looks about right and I'll move it over just a little bit that way next I'll use the sculpt tools to really create a free-form surface that captures the design intent I'll choose the create form feature and create a cylinder I'll create it on this bottom plane centered on the origin and sketch out its diameter next I can look at it from the side make it roughly the right height let's increase the diameter a little bit next I can change the amount of faces that I have going around the diameter let's drop that down to about six and I can make sure that I have symmetry on this way anything that happens to one side of the form is reflected on the other that looks good to me so I'll go ahead and hit OK next what I can do is select these edges and move them until they're roughly in place I don't have to match my sketch perfectly but I'm gonna use it as a starting point I can choose edit form and use any of these manipulators that I like until I have the form the way that I want it I'll go ahead and use the rotate manipulator to add an angle to this I'm going to go ahead and angle these as well I'm going to work my way around the model really trying to scale up these edge loops really matching up to the sketch I have behind it I'll go ahead and grab this bottom loop out here scale it up you can see my sketch wasn't exactly perfect so I'm going to move it until it's flat on the bottom let's go ahead and select these two edges over here I can move those in a little bit let's go ahead and do that to all these over here what I'm going to do next is once I have the surface already done I'm going to add the small details in the patch workspace so what I'm really doing is just making sure that I have the geometry looking roughly the way that I want it here if I hide my canvas I can see the form there and it looks good to me so I'll hit OK next to finish sculpting for now I'll choose finish form and you'll see that we're back in the model workspace with a patch body I can tell because it's colored silver and orange here and also if I open up my bodies folder I have this orange icon right here letting me know that it is indeed a surface body next I'll enter the patch workspace by choosing model selecting patch you know so that I have tools here for creating surfaces I'll start by creating a sketch to add some the finer details that we need I'll show my canvas and create a sketch on this plane right here now I want to have what few curves up here that represent this minor split up here as well as some curves down here to do this I'll use the spline tool under sketch I'll choose spline and I'm going to draw a two point spline right here and a three point spline right here I'll hit escape to stop drawing more splines and what I can do now is adjust the tangent handles until I get this curve looking just the way I want it I'm going to draw this spline until it really matches the top of this shaded region right there you can move the control points around I can move the handles as well that looks good to me it'll do the same for this bottom spline over here I want to make sure that I have as few control points as possible so that I'm guaranteed a smooth curve all the way throughout I don't want to draw this curve with ten control points those things are going to get really out of control it's not going to look the way that I want that looks good to me so let's go ahead and draw one more spline down here I can right-click and go to the 12 o'clock position and draw one more spline down here hit escape and move these handles around till I get it looking just the way I want all right so that looks good to me so we need to do now is add one more spline down here now I could draw a second spline but because I want this to be a perfect offset I don't want to I ball it what I want to do is use the offset tool and do it right to do that under the sketch drop down menu I'll choose offset select this curve and I can move it down to see that this is the positive direction let's move it down by two millimeters that looks good to me I'll hide my canvas and choose stop sketch now to make things easy I want to make sure that I'm working on just half of the bottle and then we can mirror it at the end to do this under modify I'll choose split body select this surface as the body to split and for the splitting tool let's go ahead and select this work plane I can left-click and hold and let go and then choose this work plane right there I can go ahead and hide this back surface I don't really need it for now and I can perform two more splits with these top curves again under modify all choose split body this is the body that I want to split and this is the splitting tool you'll see that I don't have to create any surfaces all I have to do is choose it as a splitting tool I'll show my sketch and repeat that split body command this time splitting this body with this curve over here if I hide my sketch you'll see that we have three surfaces right here we're ready to create some more splits this time instead of splitting the body what I'm going to do is create some surfaces just from these curves in the model workspace you're probably used to needing closed profiles for extrusions but here in the patch work space you can extrude just curves to do that under the create drop-down menu I'll choose extrude and select these two bottom curves I'll drag them out until they extend all the way through my model and this is known as over building that looks good to me so I can hit OK and now I can use these to trim away the material that I don't want to do that under modify I'll choose trim first I need to choose my trim tool which is going to be this surface and next if I stop moving my mouse you'll see it says select blank areas to remove that's going to be this thin region right here I can hit OK and you'll see that it gets rid of that surface right there I'll go ahead and hide this body body 6 let's do one more trim with this bottom surface down here this is my trimming tool this is the surface that I don't want anymore I can go ahead and hit OK let's go ahead and hide surface seven and my sketch and you can see what we're left with next if I look at my canvas you'll see that I have this offset surface in here I don't want this surface to extend all the way in I want just a slight offset from that I'll hide my sketch we can create that offset surface under the create drop-down menu let's choose offset this is the surface that I want to offset from and I can offset in its the negative direction so let's go by negative 4 how about that you can hit OK and I can hide this surface up top to see our smaller offset surface in and now we're starting to have the geometry that we see in our sketch the next thing I want to do is really extend this surface in its natural direction keeping this edge tangent to it the directions already heading in so to do that under the modify drop down menu I'll choose extend and this is another way of overbuilding these surfaces and then trimming them afterwards this is the edge that I want to extend and I want to extend natural so it's going to continue in the direction that's already heading and I'm going to extend until I ask this edge right here 20 looks good to me so I'll type in 20 and hit enter and now we've over built that surface the next thing we're going to do is sweep a profile around here to add an intersecting surface and then we can trim them out to do that I'll choose create sketch and let's sketch on this plane back here I'm going to go ahead and hide this body and I'm going to project in the intersection of these points under the sketch drop-down menu I'll choose project slash include and intersect and let's project in these three points right here I can go ahead and hide that bottom surface actually or show it rather and I can draw some lines with the line tool I want to make sure that it's anchored on this point right here I'm going to draw it until it goes in like that I'm going to sweep this around but first I'm going to draw one more curve over here at this point I'll choose a three-point arc so arc three-point arc for the slight groove I'll start it on this point have it end on this point and just draw on this arc over here I don't extend it so much that it cuts through the existing geometry so I'm going to add a small arc something like this with a large radius that looks good to me so I'll choose stop sketch and we're ready to perform our sweeps another great menu I can choose sweep I'll deselect these and I want to perform a single path sweep so the profile is just this line right here and the path is this edge right here I don't want the entire loop so I can uncheck chain selection and just select this edge right there so you'll see that it sweeps this line all the way around this path keeping it perpendicular the entire time that looks good to me so I'll hit OK I'll show my sketch one more time and now we can perform one more sweep this time using two rails instead of just one under create let's choose sweep I'll change it from single path to path and guide rail for the profile I'll select this arc for the path I'll choose this edge and for the guide rail I'll choose this edge over here it doesn't really matter which one is the path and which one is the guide rail in this case being that they're all the same distance from the line if they were different it would matter but in this case it doesn't really matter I'll hit okay and there you see we create that surface go to my home view and everything looks nice from this side but I rotate around you so that we have some trimming to do over here to trim this up I'll go ahead and choose trim from modify I'll select how about this surface as my trimming tool and this as the surface that I want to get rid of so I'll choose that and I'll perform one more trim over here this time with this surface as my trimming tool in this as the excess surface that I want to get rid of so now you can see I have all the surfaces correctly in the position that I want them all that's left is to mirror all of these across cap the top and bottom and then stitch it together so we have a solid model so that we can 3d print this out let's go ahead and do that to mirror them under the create drop-down menu I'll choose mirror I want to mirror bodies so I'll select that here from the pattern type and I can drag a box over all these surfaces to select all five of them for my mirror plane that's going to be this work plane right here I'll hit OK and there are all of our mirrored surfaces let's go ahead and create those patches on the top and bottom the create drop-down menu I can choose patch I'll uncheck the box for enable chaining and I'll select this loop right here as well as this one and you'll see that surface is created rotate to the bottom and let's create one more patch go ahead and select this edge and this edge and that patch is created and it looks like everything is in place for our final stitch stitching everything together really well dull the edges and creates a solid model assuming everything is perfectly watertight so let's see how it works out I'll choose stitch here from the modify drop-down menu and instead of selecting all of these surfaces I can again drag a box over all of them to select it the green lines indicate where the edges are going to be welded or stitched together and the operation is going to result in a new body which is exactly what I want I can hit OK and there's my solid body now if I want to add any features to this in the solid modeling workspace I totally can all I have to do is switch from patch to model and if I wanted to add a slight fill it to this top edge under modify I can choose fill it and I can add a slight fill it here to the top how about two millimeters and just to show you and prove that it is solid let's go ahead and do a section analysis so under inspect I can do section analysis let's go ahead and go from this plane right here and you can see that this is indeed a solid model so there you have it there's a simple surfacing workflow inside of fusion 360 I hope you learned something new if you like these kinds of videos be sure to give it a thumbs up if you have any questions leave them in the comments section below and if you want to reach out to me directly you can always tweet me at taylor underscore Stein thanks for watching

Channel: Autodesk Fusion 360

Views: 866,267

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, surface, trim, offset, surface modeling

Id: NypRE2aFhh4

Length: 13min 35sec (815 seconds)

Published: Fri Jun 03 2016