Fusion 360 - Visualisation | Surface Patchwork (follow-up)

this is a follow-up to a previous visualization video where i talked about the surface patchwork approach if you haven't do watch that video so that the steps taken here will make more sense i will start with a picture of the model looking from the right start a sketch on the right plane and trace the outline as follows it is not necessary to import this picture to follow along just a sketch of the rough shape will do as mentioned in the previous video we will not be tracing the full external outline but rather a portion of it for those following without a picture do make sure that you have the same number of vertices and also make sure that this line is vertical extrude this profile symmetrically i'm going to make this shape more interesting by drafting these two faces go to modify draft select this face to define a pool direction and select these two faces to be drafted i shall add a 5 degree draft next i feel less to these edges these feeders will play an important role when it comes to lofting as we shall see later since we are going to create a patchwork of surfaces we need to convert this solid body into a surface body activate the surface tab ctrl select these faces and simply press the delete key this will delete the surfaces and the solid body becomes a hollow surface body we will proceed to build this surface start a sketch on the right plane make sure that this line is vertical also we want to align these two pairs of points horizontally we can either align them using the horizontal constraint or draw a line between them and add a horizontal constraint to that line for the line at the top let it extend beyond what is required and we will trim that later make sure that the surface tab is still active go to create extrude and extrude the surface out symmetrically just make sure to extend the surface until it fully encompasses the existing body and affiliate to this corner of the surface to add a filler to a surface body you can use the same fillet command as you would for a solid the purpose of this fillet is to have matching vertices with this edge of the previous surface body here in order to trim this surface to get this final surface we have to do it in two stages one from the front and one from the top let's perform a sketch on this face let's draw a vertical center line for mirroring from the origin we want to project this edge onto the sketch plane press p for project when you hover over the edge you can see a preview select and hit ok draw the rest of the lines as shown use the left click and drag method to drag our tangent arc continue with the line that is tangent to the arc and the line at the top edge mirror the entities go to modify split face all faces will split select these three faces for splitting tool click on the select box and select the sketch lines we can only do this for half of the sketch as the command does not allow for selection of separate sketch entities repeat this for the other side in this case be sure to select these three faces as the faces to split we shall create a sketch on the top face again use this sketch to perform a split phase make sure that the surface tab is active ctrl select these faces and delete let's compare the chain of edges on this surface body and a chain of edges on this surface body you can see that each vertex has a counterpart this is not absolutely necessary but it does help with creating a better quality lofted surface since this model has a plane of symmetry along the right plane we will create a loft on one side and mirror it we need to create a series of profiles for the loft we shall define this as a starting profile let's create a sketch on the right plane this starting profile is essentially a straight line that joins these two edges to create anchor points for the line go to create project include intersect if we hover over this edge you will see a preview of the projected point in ray click here to project that point do the same for this edge these are the points where the edges intersect with the sketch plane join these two points with a line we can draw the rest of the profiles without actually leaving the current sketch turn on 3d sketch turning this on will allow you to sketch outside of the sketch plane use the line tool to join the corresponding vertices make sure to snap the line properly to the vertices by looking over the snapping square icon before clicking we will sketch in this line also even though it is not part of the loft we will make use of it to perform a patch later next go to create loft select the profile sequentially click on the select box for rails uncheck the chain selection option and proceed to select this chain of edges this will form the first reel click on the add option to add a second rail and proceed to select this chain of edges for the continuity option leave both as connected as we want an angular look to our design somewhat like a chamfer next go to create edge uncheck the training option and select these edges to create a patch surface go to create mirror select bodies as the type and select the surface bodies to mirror select the right plane as a mirror plane operation select new body the body is not fully enclosed just yet there is still an opening at the bottom just use a patch command to patch this up this is now a fully enclosed surface body to convert this into a solid go to modify stitch select all the surface bodies and stitch them into one single solid

Channel: Fusion 360 School

Views: 2,753

Keywords: fusion 360 loft surface, fusion 360 delete face, fusion 360 patch, fusion 360 stitch

Id: o0Z32cgxXt8

Length: 10min 57sec (657 seconds)

Published: Sat Dec 12 2020