How to Surface Model a Detergent Bottle in Fusion 360

by the end of this video you'll know how to surface model a detergent bottle in fusion 360 hey there it's Kevin Kennedy and welcome to the product design online YouTube channel where I demo all things fusion 360 if you're new here be sure to hit that red subscribe button and go ahead and comment below and let me know what you plan on using fusion 360 for to get started you'll want to download the demo file that I've linked to below in the video description once you upload the demo file to your data panel you'll want to double click on the file to open it up then you'll see this template of sketch geometry that I've gone ahead and prepared for this demo this template is essentially a reference image that has ellipses at each point of the bottle where the curvature changes and throughout this demo I'll show you how will reference the sketch geometry to surface model this bottle design now the first thing you want to do is switch to the patch workspace which includes all the surface modeling tools to switch to the patch workspace simply click on the workspace drop down list and select patch more often than not a surface model is built with the loft or sweep commands therefore you'll need some sort of reference geometry and you'll find as you continue to do surface modeling that the more complex a design is then you'll typically need to have more reference geometry before we start any work on the model we'll want to activate the detergent bottle bottom component by clicking the activate component button that appears when you hover over the component name I'll now proceed to create the body of this bottle by activating the loft command from the create drop-down menu it's important to note that the loft command in the patch workspace does differ from the loft command in the model workspace as we loft the surface geometry you'll notice the patchwork space creates surfaces with no thickness whereas the loft command in the model workspace already has some thickness to it with the loft command active we'll have to select the profiles to connect I'll hit the Home icon next to the viewcube so I can see all the different profiles then I'll start by selecting the bottom profile and I'll proceed by selecting the four profiles above it by selecting them in order one by one you'll notice that the loft command is giving us a preview of the body now I've also gone ahead and created some guide paths for us to reference to select the guide paths I'll select the plus button for the rails section then I'll zoom in just a bit and I'll select the guide path on the right hand side and you'll notice the model immediately updates based on the contour of the guide path with the rail section still active I'll select the guide path on the other side now I'll select the front face of the viewcube to make sure that the loft profile looks like the intended shape now since everything looks good I'll go ahead and click OK to confirm the loft command at this point I want to show you guys the surface that the patch works based loft command just created I'll toggle open the component in the fusion 360 browser next I'll hit the light bulb icon to turn off these sketches and be construction planes making it a bit easier to look at the model if I now soom in at the top of the bottle you'll notice that the surface has a gray outside and a yellow inside which means that this is a surface body you can also confirm this by opening the bodies folder in the fusion 360 browser and you'll notice the surface body icon to the left of the name now surface bodies technically don't have any thickness to them so we'll need to turn this into a solid body that has some volume to it however before we do that we'll proceed by cutting out the hole for the handle I'll hit the front part of the viewcube to view the model directly from the front then I'll hit the light bulb icon next to our surface body to hide this and get it out of the way for now what I'm going to do is create the ellipse shape of the handle and then I'll make it three dimensional and we'll trim the hole away from the main surface body I'll select the ellipse command from the sketch drop down menu and I'll select the xz-plane I'm going to zoom in a bit then I'll just guess the center point and I'll click to set the center point after that I'll drag my mouse cursor out and I'll click again to set the major axes of the ellipse lastly I'll click a third time to set the minor axis of the ellipse now I'm going to repeat these steps to create a second ellipse a bit larger than this one the outer ellipse will help us create the curvature between the handle and the bottle I'll now need to extrude the ellipse profiles I'll select the extrude command from the create drop down menu and I'll have to make sure that the sketches are turned on I'll select the outer lips I'll change the profile direction to two sides so it extends through both sides of the bottle and then I'll change the extent selection to all for both sides 1 and side number 2 now you'll notice that we can't hit the okay button and that's because the body we're trying to extend to is turned off therefore I'll select the light bulb to turn on the surface body and I'll unselect the profile and I'll reselect it and now you'll see that the okay button is visible I'll go ahead and click OK before moving any further I'll rename both bodies in the fusion 360 browser so it's easier to select the correct one later on I'll click once pause for a second and then click again and I'll type out bottle bottom for the second one I'll type out handle reference I'll also make sure that only the handle reference surface body is turned on for now next I'll toggle open the sketches folder I'll rename the last sketch handle and I'll hit the light bulb icon to turn it on at this point we have part of the hole for the handle but we want the surface to be nice and smooth so we'll have to use the loft command again to create another surface body I'll select a loft from the create drop-down list I'll select the edge of the outer ellipse then I'll select the inner ellipse sketch geometry and I'll select the corner of the viewcube to view the back of the model which will allow me to select the other edge of the outer lips and then you'll see that the loft is completed finally I'll make sure that the chain selection and close options are unchecked that the operation is set to new body and then I'll click OK before moving any further I'll change the name of the most recent body to handle hole at this point I'll turn the bottle bottom surface body back on and will now need to use the trim tool to trim the hole away I'll activate the trim tool by selecting it from the modified drop-down list with the trim tool active I'll select the handle whole body in the fusion 360 browser then I'll need to select the front face and the back face of where the hole should be and I'll click OK in the trim dialog box now you should now be able to see all the way through the model if you still see a face on the front or the back side then you'll want to go back a step and redo the trim tool being careful that you select the front and back faces now looking at the model you'll see we've got the handle completed but we still have surface bodies so we'll want to turn these into solid bodies first we can get rid of the handle reference surface body as we no longer need it however it's important to note that we cannot delete it entirely because our model does reference it what we can do instead is right-click on the body and select remove which will remove the body from the browser and you'll notice that the remove action is documented in the timeline below now we'll want to patch both the top and the bottom holes of the model so we can turn this into a solid and watertight model I'll select a patch from the create drop-down list or by selecting the patch icon in the toolbar I'll click on the top edge of the bottle and then click OK in the patch dialog box to confirm the results and I'll go ahead and repeat these steps for the bottom of the bottle now to save time I can select the edge first and right click and use the patch tool from the marking menu and I'll click OK to confirm these results as well you'll notice in the fusion 360 browser that each patch also created a surface body while holding down the shift-key I'm going to select all four surface bodies then I'll select the stitch command from the modify drop-down list after double checking that all four surface bodies are selected I'll hit the ok' button in the stitch dialog box the stitch command helps us stitch surface bodies together to make a single surface body or a single solid body if you take a look at the bodies folder on the left hand side you'll notice that now I only have one solid body I'll rename this body to bottle bottom and then I'll hide everything but the solid body by turning off all the light bulbs in the fusion 360 browser now that we have a solid body we can utilize the parametric modeling tools in the model workspace I'll switch back to the model workspace by selecting model and the workspace drop-down list for example I can use the Filat tool to smooth out the handle I'll activate the Filat tool with the keyboard shortcut letter f as in Foxtrot then I'll select both edges of the inner part of the handle and I'll type out seven millimeters to give this a nice smooth radius and I'll click OK I'll select the bottom edge of the bottle and right click and select repeat fill it I'll make this fill it five millimeters and then I'll click OK finally to wrap up this video I'll make the thread for the cap and I'll make the body Hollow I'll select the offset command from the sketch drop-down list which will allow us to create a circle a set distance away from the outer circle then I'll select the top of the bottle I'll select the edge of the bottle or the outer circle and I'll make the dimension two millimeters followed by hitting the flip button until the offset is on the inside after clicking okay I'll hit the keyboard shortcut letter e as an echo to call the extrude command I'll have to toggle the sketch folder back on by selecting the light bulb and then I can select the inner circle that we just created with the offset command I'll extrude this up by typing out 15 millimeters and then I'll click OK in the extrude dialog box for now I'll also turn the sketch folder back off at this point I can make the bottle hollow by using the shell command I'll select the shell command from the modify drop-down list once the shell command is active I'll select the top flat surface of the bottle then the shell command requires you to type out a dimension that the remaining thickness should be I'll type out two millimeters and I'll click OK I'll click the thread command from the create drop-down list and I'll select this upper cylinder that we just created I'll leave the thread type set to the isometric profile I'll set the size to 36 I'll change the designation to M 36 times 3 I'll double check that the thread is right hand and lastly I want this to be an actual modeled thread so I'll have to check modeled at the top of the dialog box I'll also uncheck the full length option and type out 14 millimeters before clicking ok in the dialog box I'll hit the keyboard shortcut letter F to call the Phillip command once again and I'll add a Filat of just one millimeters to this top edge so it isn't quite as sharp using these section analysis we can double-check that our body is watertight or solid yet still hollow on the inside I'll select the section analysis from the inspect drop-down menu I'll select the X Z origin plane and I'll just slide the arrow back and forth so you guys can see what the insides of this model look like if you're one of my subscribers that was asking for more surface modeling videos than I hope you enjoyed this and if you're new to surface modeling or have never done surface modeling before then I hope this gives you an idea of just how powerful it can be either way if you've enjoyed this video please give it a thumbs up and go ahead and comment below and let me know if you find these surface modeling tutorials to be helpful thanks for watching if you have any questions at all about this tutorial or fusion 360 questions in general then be sure to comment them below hit that thumbs up icon if you learn something in this video and click Subscribe followed by that little Bell icon to be notified of more fusion 360 tutorials

Channel: Product Design Online

Views: 31,759

Keywords: fusion 360, autodesk fusion 360, kevin kennedy fusion 360, product design online, fusion 360 tutorials, fusion tutorials, fusion 360 30 days, learn fusion 360 in 30 days, fusion 360 beginners, fusion 360 kevin kennedy, learn fusion 360 or die trying, fusion 360 surfacing, fusion 360 surface modeling, fusion 360 surface modeling tutorial, fusion 360 surfacing tutorial, fusion 360 surface to solid, industrial design, fusion 360 tutorial, product design

Id: 2MoecvL6eVA

Length: 15min 3sec (903 seconds)

Published: Wed Jan 23 2019

Reddit Comments

[u/tipsygelding]

I've always worked in the Model workspace and am not familiar with what the Patch workspace is useful for. Can't all of these steps be done in the Model workspace and you get a solid directly without the stitching step? When should the Patch workspace be used instead of the Model workspace?

[u/flangeboy]

Hey /u/productdesignonline . Thanks for a great tutorial. I've just used this to design a complex shape for a handheld product I am designing right now. It has made it so much easier. You are doing great work. Once again. Thank you.