Loft in Fusion 360: Beginner to Advanced Techniques

by the end of this video you'll know how to use the loft command in fusion 360 I'm going to cover many of the options in the loft dialog I'll also be walking you through both a beginner and a more advanced loft example with step by step instructions if you're looking for the advanced tips and tricks then you can skip ahead by using the time stamp but I have down below in the video description put simply the loft command is like connecting the dots using the law feature we'll join the selected profiles resulting in a solid or surface to start you should know that the loft command is available in three different environments we have the solid modeling loft command found under the create drop-down of the solid tab the surface modeling loft command found under the create drop-down of the surface tab and last but not least we have the forum loft command which is only available if you're in the forum or sculpt environment at their core all of these locked commands work similarly each la feature does have some small differences that I'll be covering near the end of this tutorial let's start with a basic loft project where I'll walk you through many of the options in the loft dialog I'm going to create a 100 millimeter center circle on the bottom XY origin plane we'll need to create the second profile on a construction plane since we don't have any other phases or surfaces to reference I'm going to create an offset plane 100 millimeters off the XY origin plane once the construction plane is completed I'm going to create a center rectangle off of the offset plane I'll use the dimensions of 100 millimeters in both directions at this point we have the minimum requirement for creating a loft in fusion 360 I'm going to activate the loft command from the shortcuts box where I'll choose the blue solid modeling version notice how the surface loft command shows up but the form loft command does not now the form or T spline loft will only show up in the shortcuts box if you're currently in an active form environment with a loft command active well first need to select our profiles the first thing to know is that the order you select the profiles does matter which we'll take a look at in just a minute for now I'll simply select both profiles here we have the most basic loft connecting a circle with a square which is a shape that can't be created with the revolve tool in the profile section of the dialog you'll notice a plus symbol and the letter X as you're selecting profiles you may find that you selected the wrong profile if that is the case simply select the profile you want to remove and then click the X or remove button if you want to add more profiles you can hit the plus symbol or the Add button and click the sketch profile that you would like to add the next item you should be aware of is the end condition there are six different end conditions with the availability depending on what type of geometry is selected I've put all six types and their descriptions on this tutorials resource page at product design online.com / 20 - that's product design online comm / - 2 if I click on the default of connected you'll see that I only have one other option which is the direction I'll go ahead and look at this from the front view so you can see what happens as I change the first profile to the direction option notice how the loft goes from having a straight and efficient line to having an angled line the direction option applies an angle measured off of the sketch plane this option is always available when the loft profile is a 2-dimensional sketch the default connected option simply connects the profiles in the most efficient manner which is why we have a straight line from the circles edge to the edge of the rectangle if we don't want this to simply be a straight line then we can also define the guide type by defining a guide rail or a centre line you can also drag around the default rails that were created between each profile I'll be walking you through adding custom rails with the next loft example so for now let's take a look at using a centerline to further define a loft I'm going to hit OK to close the loft command I'll hide the body and create a new sketch off of the XZ origin plane because this plane is perpendicular to the two profiles and directly in the middle of each profile on this center plane we can sketch out any sketch geometry as long as it connects from the bottom profile to the top profile the key takeaway is that your centerline sketch geometry must be connected to the center point of all the profiles that you're connecting because I created both profiles off of the center origin point the center point was automatically projected if you don't have a Centerpoint to snap to you will need to either project one or you can always create one with the point sketch feature I'm going to connect the profiles with the three-point arc tool making sure it snaps to each Center point after finishing the sketch I'll drag it to before the lot feature in the timeline I'll double-click on the lock to edit the loft and I'll select the centerline rail type after that we simply need to select the centerline immediately after the loft we'll just based on the centerline as you can see this is a very simple way to further define your loft results let's now take a look at why the order of selecting the profiles matters and then I'll walk you through an advanced loft example I'll click OK to update the loft I'm going to create a new offset profile off of the top base of the model I'll create a center circle on the construction plane and then I'll finish the sketch once again I'll need the loft command at the end of the timeline so I can reference the sketch that I just created after re editing the loft command I'm going to clear out the center line as that doesn't connect all three profiles so I can no longer use it I'll then click the plus symbol in the profile section and I'll select the top circle profile notice how this connects all three profiles and creates a nice transition from one shape to another generally you'll always want to create your loss by starting at one end and then selecting the profiles in order as you work your way to the other end watch what happens to this loft if I were to click the middle profile last you'll see the shape folds in on itself creating unrealistic geometry which in many cases fusion 360 won't be able to solve in the case that you selected profiles out of order or if you decide to add profiles later on then you can always reorder the profiles without having to re select them you can either select the profile order from the drop-down list on the model or by selecting the order in the loft dialog let's now take a look at lofting a more complex object I'll walk you through an ergonomic handle with spots for each finger to rest I'm going to hide the basic loft component and I'll create a new component for the handle I'll first attach a reference image to help recreate the contour if you're looking to follow along I've placed the reference image on this tutorials resource page at product design online.com /to to I'll attach the image to the XZ origin plane and then I'll calibrate the image to have an approximate handle height of 125 millimeters I like to start the first profile off the bottom origin plane so I'm going to re-edit the canvas image to adjust the position so it aligns with the bottom plane I'm also going to Center the image to the origin point for the first profile I'll create an ellipse on the XY origin plane I'll make the major access 40 millimeters and the Minor access 30 millimeters one thing to understand with more advanced lofting is that you'll often want to break the lofts into sections I'm going to break this handle into three main sections for the first loft I'm going to law from the bottom of the handle to the middle of this top curve for the second loft all off from the middle of the top curve to the beginning of the nozzle finally for the third loft I'll create the large area of the nozzle I'm going to create an offset plane 110 millimeters from the XY origin plane the handle gets smaller towards the top so I'll create a second ellipse making this 135 millimeters at the major access and 25 millimeters at the minor axis I'll finish the sketch and we're ready to create our guide rails I'll then create a sketch from the EXCI origin plane as I want these rails to be defined in the center so the shape is symmetrical however it's important to note that rails do not need to be created directly in the center as these center lines do similar to center lines to create guide rails you can use any of the sketch geometry the key takeaway is that you'll always have to make sure that your guide rail touches every single profile this can't be stressed enough I often see beginner struggling to get their loft to work because the rails aren't snapped to each profile for example if you have five profiles it needs to touch all five at some point in our case we only have two profiles so I'm going to use the spying command to trace the handle shape starting at the bottom I'll make sure that it snaps to the major axis of the ellipse now if you're creating a guide rail and having trouble getting it to snap to a profile then you have a few different options you can project the point create a construction line create a sketch point where you want it to snap or you can always use a coincident constraint after the fact to force it to stay together in this case the start of the spline snapped into the major axis of the ellipse so I'm just going to trace this image placing points at all of the vertices once I get to the top you'll see the end of this wine is not wanting to snap to the tapa lips I'm going to simply click to place the point and then I'll use a coincident constraint to force it to connect with the endpoint of the major axis because I'm going to create a second loft on the top of this one I'm going to also add a vertical constraint to the spline handle so the exterior geometry ends up with a smoother connection to the next loft I'm going to activate the loft command so we can see how the guide rail works I'll select the bottom profile as the first and then the top profile as the second at the moment we have a nice straight handle with a small taper to add our guide rail I'll simply click the plus symbol for the rail section and I'll select the spline geometry notice how the loft shape now zigzags and follows our desired shape however I don't want the back of the handle to have the same zigzag effect as the front so we'll need to create a second guide rail I'll hit the cancel button in the loft dialog so we can create a second spline for the back I'll retrace the back silhouette once again making sure that the starting and ending points of the spline snap into each profile if not I'll force them to with the coincident constraint you once again I'll also add a vertical constraint to the handle of the top spline point I'll reactivate the loft command and this time I'll select both guide rails notice how the contour of the handle is now further defined with the help of rails if we wanted to we could continue to add rails on the sides of the profiles in fact we could technically add as many rails as we would like so long as they all touch every single profile within our loft for now i'll click the ok' button to confirm the loft so we can look at creating the second loft to finish off the handle when working with the lock command it's a best practice to break the object into sections that could be lofted individually this will give you more control and make it easier to create guide rails as they won't have to touch as many profiles typically when you start a new loft from another you'll want to project the surface geometry I'm going to select the top surface and I'll project the ellipse geometry onto the surface I'll also create a construction line running across so I have the endpoints to connect the rails to then before we create the next profile I'm going to first create one of the guide rails I'll then use the guide rail to create a construction plane for the next profile I'm going to trace the bottom of the shape using the spline tool in the coincident constraint to force the points to snap to the first profile I'll also make sure that there is a vertical constraint add it to the first spline handle so the geometry has a nice transition from one loft to another after that's complete I'll create a construction plane on the end of the guide rail using the option plane a long path from that plane I'll then create a new sketch where I'll create a two-point circle with the first point starting from the end of the slide I'll make the circle 35 millimeters in diameter to help ensure that the rail snaps into the circle I'm going to create a sketch point where the rail should connect then I'll create another sketch on the XZ origin plane where I'll create the top rail once again making sure that the spline points snap into the lips and circle respectively if not I'll use the coincident constraint to force them to snap together I'll also add a vertical constraint to the bottom spline handle at this point we're ready to use the loft tool I'll select both profiles starting with the first one on the existing surface then I'll select both guide rails before clicking the ok button you'll also want to decide if you want this second law to create a new body or if you want to join to the other locked body you'll see that we can also create a new component use the loft tool to cut away bodies or the intersect option which removes all the material from the solid that does not overlap the new feature for now I'll set this to join and I'll click OK lastly I'll create one last offset plane off the top surface I'll set the offset distance to 45 millimeters I'll first project the other circle to this sketch ensuring that we use the same center point I'll then create a new circle with a diameter of 75 millimeters I'll also create two Sketch points on the circle so it's easier to connect a guide rail well then need to use the three-point art tool to define the guide rail I'll also use the coincident constraint to force these lines to connect you repeating the loft command we can create a third law that finishes off the overall shape of the handle and nozzle looking at the model there are a few things that we should do first off it appears that the transition from this first law to the second Loft is not completely smooth as you can see this crease in the middle now this is caused by the width of the shape having different geometry near the meeting point to fix this we would need to define a few more guide rails for each loft making sure that they're parallel at the meeting point I would also then apply Phillips to this model where the second loft and third loft are joined further smoothing out the transition as well as adding a Filat to the bottom edge of the handle to finish out this tutorial I want to show you the differences between the surface and form loft commands I'll drag the timeline marker to just before the first loft command and I'll turn the original sketch geometry back on so I can reuse it this time I'll activate the surface lock command from the shortcuts box watch what happens as I recreate the loft at a distance everything seems to work the same however you'll notice as i zoom in that this only created a surface body which is represented by the thin grey and yellow surface with surface lofts the ends won't automatically be sealed off and you'll have to use the patch command to do so other than that the surface loft command follows the same rules and best practices as the solid modeling loft command before I show you the form loft command let me know which loft command you find yourself using the most by commenting solid or surface down below in the comments while you're at it click that thumbs up button to let me know if you're learning something in this tutorial I'm going to undo the surface loft command so we can take a look at the form loft command to access the form loft command I'll enter the form or sculpt environment to start the loft we'll need to follow the same steps as the other two loft commands once the loft is created this is where the form loft command becomes different notice how I have all these T spline faces that are connected to make up the body the difference in the form loft command is that we can define the number of faces in each direction we can also define whether the faces should be uniform which is the default option or we can set this to the curvature option where the number of faces adapts based on the defined curvature I'll click OK to complete the loft at this point you're left with the T spline body that can be manipulated just like any of the other T splines in the form or sculpt environment for example I can drag over the front edge of the shape to select it I'll edit the form and I'll drag the planar Direction icon towards the left to alter the handles thickness a few other things to note with the form loft command is that it won't be recorded in the timeline below as everything is simply created under the form icon along with that you'll see that the form Loft only allows you to create a new body or component as you're not allowed to cut or intersect from any of the form bodies to summarize the loft command is available in three different formats solid modeling surfacing and sculpting the loft command is commonly used to bridge the gap between sketch profiles be sure to break complex objects into multiple lofts which will make it easier for you to avoid common loft errors last but not least I want to give a shout out to Jim Ferguson for supporting all of the fusion 360 content that I make if you have found my tutorials to be helpful in any way then consider supporting by becoming a patron or by making a one-time donation on my buy me a coffee page all of the contributions help me keep the website up and running and will help me continue to invest in more gear so I can continue to create high-quality tutorials as always I truly appreciate you taking the time to watch this tutorial if you haven't already click that thumbs up icon to be part of the product design online community be sure to subscribe and check us out on patreon by clicking that patreon logo right now

Channel: Product Design Online

Views: 60,214

Rating: 4.9460154 out of 5

Keywords: fusion 360, autodesk fusion 360, 3d printing nerd, how to basic, how to, 3d printing, 3d modeling, fusion 360 woodworking, 3d printing for beginners, loft, loft in fusion 360, using loft in fusion 360, fusion360, free cad tutorial, free cad software, mechanical engineering, 3d printer projects, 3d printers for beginners, 3d printer software, loft cad 3d, fusion 360 loft rails, fusion 360 loft tool, fusion 360 loft along path, fusion 360 loft hollow, product design

Id: Mimbq-k2dWg

Length: 24min 38sec (1478 seconds)

Published: Fri Oct 18 2019