LEARN FUSION 360 FAST! A Beginner Tutorial [step by step instructions, no prior knowledge required]

welcome to this fusion 360 beginner tutorial where we built the bialetti mocha pod it's a step-by-step tutorial and you will be able to follow along even if you have never opened fusion 360 or any other cad application before i recommend that you watch the entire tutorial first then download a free version of fusion 360 and follow the instructions step by step so the mock-up is quite a complex object consisting of several different parts so let's do not waste any more time and get straight to it this is what you see when you launch fusion 360 for the first time we start in the design environment it's one of many environments available in fusion 360 and we stay in the design environment to build our parts next to it we have the toolbar it's organized in different tabs and it almost looks a little bit like there is not that much to cover because how tidy and how well organized everything is but as soon as you open up the drop down menu you can see a long list of tools and features so i can guarantee that there is a lot to discuss and a lot to cover below the toolbar there is the still empty 3d viewport on the left we have the browser tree this one will contain all of our components bodies and sketches and at the bottom we have the timeline or the parametric history this one is also still empty because we do not have anything in the scene yet but it will be filled with all of the functions and features that we apply to our model when we now want to build something we cannot just place it somewhere in 3d space we have to start building it on a plane and therefore the scene is not completely empty we have this origin folder in it so when i click on the little eye icon next to it you can see that we already have three different planes three axes and this origin point right in the center of our design and when i now open up the create drop down menu choose the cylinder fusion wants me to pick one of these planes so i go for the top plane and i can tell that this one is the top plane because of the orientation of the view cube in the right hand upper corner and i can now start drawing the base of the cylinder right on the origin so let's enter a value of 3 for the diameter and something like 5 for the height when i now press the middle mouse button together with the shift key i rotate the camera around the model when i only hold down the middle mouse button i pan the camera and when i press the middle mouse button together with the shift key and the control key i move the camera closer to the object or away from it in my case this looks a little bit different because i'm using a space mouse so that's one of these devices that allow me to zoom rotate and pan the model simultaneously that's also the reason why it looks a little bit smoother on my end than it probably does on yours when you just use a regular mouse a few things have changed when i drew the cylinder before so let me hide the origin folder first and below it we now have a new folder that contains the cylinder as a body and we also have the cylinder icon in the timeline when i double click on it i can edit the feature and in case of the cylinder i can change its height and also the diameter by clicking on these arrows i can also enter the values over here in the dialog box i want you to take a close look at what happens in the timeline when i continue to adjust the model so i go to modify chanfer and this little c next to the name chamfer means that the shortcut key c is already assigned to this function so when i run the channel command next time i do not go to modify chamfer anymore i simply press c on the keyboard to bring up this dialog box then i select the top edge chamfer it like so confirm this command and a new chamfer icon appears in the timeline when i double click on the chamfer icon i bring up the chamfer dialog box and here i can lower the value to something like point 2 and confirm this now it is very important to understand that the chamfer command relies on the cylinder so if there is no cylinder then there is also no edge to chamfer and this also means that when i change the cylinder by double clicking on it and lower the height also the chamfer follows accordingly this interaction between functions in the timeline can be quite confusing at the beginning but i promise that it will make a lot more sense when i start building the first parts of the mokka bot next let's start with the bottom chamber or the boiler first i have just started a new design and before i built anything i go to assembly and create a new component so let's call this one boiler this component will contain all of the sketches and all of the bodies that make up the boiler so i make sure that this one is active you can activate components by simply hovering over the name and then check this little pin next to it this time i do not start with a 3d primitive like a box or a cylinder but with a two-dimensional sketch instead so i run the sketch command and like we already had it on the cylinder fusion wants me to select a plane where to place the sketch so i go for the top plane and this enters the sketch mode when being in sketch mode a whole set of new tools become available so i go to create down to polygon select inscribe polygon and create one next to the origin before i confirm this let's set the number of edges to eight and then i just click somewhere to place it when i now select a point i can move the whole thing around when i select an edge i can make it smaller or bigger and when i choose the center point of the polygon i can rotate it because the mocha pod is pretty cylindrical in shape and also quite symmetrical it makes sense to build it in the center of the design so i simply select the center point of the polygon and move it over until it snaps to the origin this at the same time applies a coincidence constraint to the midpoint so it ties the midpoint to the origin when i now select one of these points here i can still rotate the polygon but i cannot move it around in space anymore you can unlose it again by simply selecting the coincident constraint and then by hitting the delete key on the keyboard and now i can move it around in space again so let me undo this by bringing it close to the origin until it snaps and in the next step i also want to constrain the rotation so i run the line command this time i start a straight line at the origin place it down here exit the line command by hitting the escape key on the keyboard and then i select this line and turn it into a construction line construction lines do not contribute anything to the actual drawing but i can still use them to drive the sketch so i select this line first go up to the constraints tool palette and pick the horizontal and vertical constraint and because of its current orientation fusion should automatically apply a vertical constraint to this line and then let's also tide a point of the polygon to the end point of this construction line this can be done by using the coincident constraint so i select this point here first and then the end point of the construction line and because this line has a vertical constraint assigned to it i'm no longer able to rotate the polygon i can still change its size though by selecting an edge and moving it closer or away from the origin and we can also constrain this behavior this time not with one of these constraint tools but with sketch dimensions so i select this tool choose an edge and add a dimension of something like 4.2 centimeters at the same time all of these sketch entities have turned from blue to black so this means that i have turned the drawing into a fully defined sketch and it also means that when you want to make any adjustments you have to change the dimensions or you have to delete some of these constraints i'm now ready to exit sketch mode this can be done by clicking on the finish sketch button at the top and when we take a look at the browser tree and open up our boiler component it now contains a sketches folder with the new sketch in it when you see this little red lock icon here it means that the sketch is fully defined and if you want to make any changes on the sketch simply double click on the sketch icon in the timeline to enter sketch mode again next let's run the extrude command and give it a height of 8 centimeters i also change the taper angle and set it to -8 so this makes the extrusion a little bit slimmer at the top and then i also make sure that the operation is set to new body at the same time a new bodies folder appears in the browser tree that now contains my extrusion and an extrude command also appears in the timeline behind the sketch icon again it is important to point out that the form of the extrusion depends on the sketch so when you double click on the sketch icon in the timeline and decrease the length of one of these edges exit the sketch mode then also the form of the extrusion has changed and i can of course also adjust the extrusion by double clicking on the extrude icon in the timeline and then i can for instance lower the height or adjust the taper angle and then the model updates accordingly now let me undo this a couple of times to get back to our initial extrusion and before i continue let's take a look at some of the reference images the bottom edge of the boiler is slightly chamfered and this can be achieved by drawing a new sketch on one of the side planes and then use this sketching combination with the revolve tool so let me show you how to do this i start a new sketch first and in case you have a hard time selecting one of the base planes of the coordinate system simply hide the body choose the plane where you want to start the sketch on enter sketch mode then show the body again and then you can continue drawing lines using any of these sketch tools now i do not start with a straight line or circle here because you can also use elements of already existing parts and project them onto the current sketch plane therefore i run the project command so i go to the create drop down menu down to project and include here i pick the project tool the shortcut key p is already assigned to it and then i can select entire faces edges and even points i go for edges select this one here first and the one at the bottom and when i confirm this you can see that now these two purple lines appear when i select one of them the projection constraint icon appears and when i hover over this icon i can see where the sketch entity is projected from i can also not adjust or tweak any of these lines as long as the projection constraint is still valid so i would have to select the constraint hit the delete key on the keyboard and now i can change and adjust these lines so this also means that as long as this connection is valid these projected lines change when i tweak the underlying geometry in this case the extrusion then let's turn the view perpendicular to the sketch plane this can be done by clicking at the look at icon over here then i run the line command draw a straight line so i hover over this projected line first until the cursor snaps i click once draw a straight line to the line at the bottom and click one more time to end the sketch when i now hide the body you can see that the area between these lines is tindered in a light blue color and this indicates that i have created a closed profile and that's exactly what i need for the next step so let me show the body again exit the sketch mode then i run the revolve command and because the sketch was already selected it's also already selected in the revolve dialog box for the profile so all that's left to do is to select an axis i go for the z-axis here and because the operation is set to cut fusion provides me with a preview of the resulting cut so i'm gonna keep everything as it is and confirm this when i now compare the chamfer with the reference images mine is a little bit too strong but we can easily adjust this by double clicking on the sketch icon in the timeline and then i decrease the angle of this line a little bit i simply select the starting point of the line and move it down along the projected edge like so and when i finish the sketch or exit the sketch mode then the model updates the chamfer is a little bit smaller and that's exactly what i'm looking for now let me repeat the exact same process also for the top edge so i'm gonna create a new sketch first again on the front plane i hide the body so that i can select the plane i show the body again and then i hit the p key on the keyboard to bring up the projection tool and i select this edge over here and this one i confirm this and now i run the line command so instead of clicking here i simply hit l on the keyboard a draw straight line and this time let's also use some dimensions so i'm going to bring up the dimension tool by hitting the d key on the keyboard and i measure from this point over to the origin so i click on the origin and apply a dimension of 3.5 centimeters then when i hide the sketch you can see that i have created a closed profile here again so it's time to exit the sketch mode run the revolve command again because this sketch was already selected it is already selected also for the profile in the revolve dialog box so i continue by selecting the z-axis fusion shows me a preview again and then i confirm the cut and because this one is a little bit too big i double click on the sketch i can in the timeline again and move this line up just a tad maybe that was already too much so let's bring it down a little bit and then i'm good to go and i can finish the sketch now we can not only extrude close profiles but also planar faces of bodies so in this case we can simply select the top face of our boiler run the extrude command type in something like 0.5 centimeters and confirm this then let's also add a fillet to this edge so that we have a smooth transition between the chamfer and the cylindrical extrusion so go to modify fill it again the shortcut key f is already assigned to the filler command i select this edge type in something like 0.5 centimeters and confirm this before we hollow the boiler in the next step it is very important to mention that we are currently dealing with a solid piece of geometry so this becomes obvious when i open the inspect drop down menu click on section analysis here i choose the front plane and then we can see that the cross hatching marks all of the areas that are currently made out of solid geometry and because the entire inside of our boiler has this cross hatching on it it means that everything on the inside consists of solid material i can now hide the section analysis again i also close the origin folder here and then i choose the shell command from the toolbar and all i have to do here is to select the top face the direction is already set to inside so let's add a wall thickness of three millimeters i get a preview i confirm this and when i now run the section analysis command again you can see that our boiler is hollow inside with a wall thickness of three millimeters all that's left to do to complete the boiler is to hide the section analysis again and then i will add a thread to this top cylinder so i select face first go to create choose the thread tool and here i check the modeled option first so that fusion gives me a preview of the spirals so let's add a few more by changing the designation value to something lower and then i also uncheck the full length option and limits the thread at the top a little bit let's try something like point one looking good and then i can confirm this before we continue let's save the design so i open up the data panel here i create a new project and call this my mocha pod then i double click on this folder go to file save and this is also my mocha pot fusion 360 is a cloud-based application so this means that you store all of your designs in the autodesk cloud and it sometimes also takes a few seconds to upload the model depending on how busy their servers are and how fast your internet connection is when it's done uploading this little icon appears next to the thumbnail and the title of the design when you click on it you get some additional information about who was creating it and you can see also what version is currently in use so there is only one version available because i have only saved it once so far but this list gets longer and longer each time you save the design then let's continue with the little safety release wolf that is mounted on the side of the boiler and for this reason i create a new sketch but this time i do not start on one of the coordinate planes but i start a new sketch right on a planar face of our model so i select this one first and instead of clicking on create new sketch i simply hit the l key on the keyboard which is the shortcut key for the line command to enter the draw mode then i start a line on the origin exit the line tool by hitting the escape key and then i turn this line into a construction line so you do not have to click the construction icon over here you can also hit the x key on the keyboard and then let's continue with another polygon and this time i do not go to create polygon but i hit the s key on the keyboard to bring up the sketch shortcuts menu and here i type in polygon and choose the inscribed polygon click on the end point of this line and let's add some dimensions already here something like 0.5 then i zoom in a little bit and i also apply a horizontal constraint to this top edge instead of leaving the sketch mode by clicking on finish sketch and then run the extrude command in a second step i simply hit the q key on the keyboard to exit sketch mode then i select to close profile and the extrude command runs automatically so let's add a thickness of 0.3 confirm this select the planar top face hit the l command again to enter sketch mode and to start a new sketch and here i draw a straight line then i turn this line into a construction line again and when i now use the constraint tool i can type these points to the points on the extruded polygon i click here and here and here and over here and this automatically projects the points from the underlying geometry so this means you do not have to run the project command first you can simply use the constrain tools to project entities to the current sketch plane then i press the s key on the keyboard to bring up the shortcut menu here i pick the circle hover over the construction line until this little triangle appears so this marks the center point of the line then i draw a circle add some dimensions let's add a diameter of 0.6 centimeters confirm this select the circle go to modify and run the offset command and here i offset it by minus 0.1 centimeters then i confirm this i select the outside profile and hit the q key again to exit the sketch mode and to run the extrude command simultaneously and then let's extrude this guy by something low let's try 0.1 with a taper angle of minus 20. last but not least i also select the circle in the center run the extrude command again by hitting the e key on the keyboard let's also try something low like point three for this one and then i bring up the chamfer command by hitting the c key select a couple of edges and the top edge of this cylinder and let's try a very low value also here something like point one or even 0.05 and then i can close the chamfer dialog box now that's it for the bottom chamber and after a short break i show you how to build the little basket that takes up the ground coffee for the little basket i create a new component first so i select the top level component by hovering over the name and check the little radio button on the right then i go to the assembly drop down click on new component let's call this basket and as you can see the new component is already selected and the timeline is empty so let me close the boiler component and also height this one and then i start a new sketch on the front plane i hit l on the keyboard to run the line command and start a new straight line at the origin let's add a length of eight centimeters and then i'm also going to continue to draw only one half of the little basket and i'm not so concerned about any dimensions yet because i can still change and adjust all of the line segments later on so let's add a dimension at the top something like 3.3 centimeters then i also move these lines in a little bit let's add another dimension of 0.1 centimeters here and a distance between this line and the center line of about 3.1 centimeters of course i have already taken the measurements of the basket before so i know what kind of values and what kind of dimensions i have to use to rebuild this thing so let's also make this one a little bit shorter 3.5 and last but not least i'm gonna add another dimension at the bottom of point seven centimeters as you can see all of the sketch entities have turned black and this again means that i have created a fully defined drawing now i'm ready to exit the sketch mode again and choose the revolve command the profile is already selected for the axis i select this line and then i get a preview the revolve tool is currently set to 360 degrees that's what i'm looking for so i'm going to keep everything as it is and confirm the revolve operation before i hollow the basket i add a few fillets so i press f on the keyboard to run the filler command then i select these three edges and enter a value of three millimeters and then i can choose the shell command select the top face of this model and then let's try something low like point five millimeters looking good then i can keep it as it is and also perforate the bottom so i simply select this face hit the e key to bring up the extrude command and this time i simply move this arrow up a little bit so that the bottom part perforates this section and then i can confirm this and i have almost completed basket the last thing that's missing here is a small fillet at the top so i run the filler command again select this edge and add another fillet of around 0.2 centimeters now as you can see on the reference image there is a little filter inside the basket and in the next step we are going to create this filter so we will create a new construction plane first and you can go to construct offset plane then i choose the top plane here and offset this one by 5.2 centimeters then i simply hover over this plane right click on it create a new sketch and instead of drawing here something i simply project one of these already existing lines so i bring up the projection tool by hitting the p key then i select this line click on ok select the profile hit the q key to exit the sketch mode and to run the extrude command and then let's extrude this by something like one millimeter and before i click on ok i set the operation from join to new body then i click on ok and when we take a look at the browser tree in the bodies folder i now have a body for the basket and a separate one for the filter on the inside let's create the little holes of the filter next and for this reason i hide the basket so that we can focus only in on the filter i select the top plane enter the sketch mode bring up the shortcut menu choose the circle and draw a small one on the origin something like 0.15 then i select this one go to create rectangular pattern and here let's use only one direction so i drag this down and enter something like 2.3 centimeters and for the quantity i set this to something like 6 and then i'm going to finish the rectangular pattern command exit the sketch select all of these profiles then i move them down and instead of keeping the extent to distance i switch it to all and this perforates exactly the thickness of our filter so then i confirm this and now it's time to go to create again pattern circular pattern and this time i set the type from faces to features i select the extrude feature for the axis i choose the c-axis and for the quantity i try something like 10. looking good and then we can also confirm the circular pattern command to fill the space in between i create a new sketch again on the top plane of the filter this time i select two of these circles and project them by hitting the b key to bring up the project command and then i create an arc between these circles so i bring up the shortcut menu by hitting the s key type in arc select a three point arc and the arc starts here and ends here and then let's also make the arc equal to the big cylindrical outside line of the filter turn this one into a construction line and then i draw a new line starting again at the origin and i place this in the center of our arc turn it into a construction line two and all that's left to do is to create another small circle at this point again 0.15 centimeters and now i go to create choose rectangular pattern again this time we can choose a direction so the direction is this construction line and our object is this circle and then let's see how many we can place so i'm gonna keep it 1.5 and let's try 4 for the quantity i confirm this exit the sketch mode again then i select all of these profiles extrude them set the extent to all close the extrude command and then i go to the create drop down menu pattern circular pattern the type is already set to features i select the last extrude feature for the axis we go with the z-axis again and for the quantity we enter 10. the filter is complete now i can show the basket again and zoom out a little bit to examine the entire model and i can also show the boiler component and before i move the basket in place let's take a look at another function that's available in the inspect drop down at the very end of this list it's called the component color cycling toggle and when you activate this fusion displays different components in the browser tree in different colors so this makes it a little bit easier to locate the models in the viewport and in case you are not happy with one of these colors you can always right click on the component and choose cyclic component colors to select or to choose a different color as you can see the basket sits a little bit too much inside of the boiler but we can change this easily and because we have created these parts in different components i can simply select or click one of these components and move it around in space and when i do this these two icons appear in the menu bar so the first one is the capture position and the second one is the revert position so when i click on reverb position these components move back in place and when i click on capture position it looks like nothing happens but when i switch to the top level assembly here and activate it you can see that at the very end of the list a new capture position icon appears now let me undo this as i'm going to use the align tool to place the basket right on top of the boiler so i simply select this position icon and hit the delete key so everything moves back in place then i hide the boiler and i run the align command so you can find it under modify align and now let's select this circle here then i show the boiler again and this time i select this top circle here and it gets positioned right on top of the boiler component so i'm gonna confirm this and i also capture the position when i now enable the cross-section analysis again you can see that the basket sits perfectly inside the boiler and there is still some room between the bottom of this bottom chamber and the bottom part of the basket so that the steam together with the water can flow up inside this basket and can go through the filter where the ground coffee is and then it can move up into the collecting chamber at the top that's it for the basket and after a short break i continue with the collecting chamber now before we continue to build the coffee collecting chamber i want to show you what parts we have here so there is this bottom ring and on the inside we have an additional thread a filter and a gasket and when i open up the top lid you can see a nozzle with an opening on top where the finished coffee comes out on the back we have a handle that is attached straight to the collecting chamber and this connection also serves as a hinge for the top lid so except the additional filter and the gasket at the bottom we are going to build everything else in the next 30 minutes let's start with the bottom ring of the collecting chamber first before i draw anything i make sure that the top level assembly is active then i go to assembly new component and let's call this one our collecting chamber as you can see a new component gets attached to the browser tree i'm gonna cycle through the colors so that we can distinguish these parts a little bit easier and then i start a new sketch on the front plane so let's hide these two components first then i select the front plane show both components again and when you take a look at the sketch palette over here you have the option to activate a slice mode so that you can see through both components directly onto the sketch plane then i continue with the line tool to draw the profile of the bottom ring so i start the line at the origin turn it into a construction line make it 9.5 centimeters long and then i continue with the line tool again and draw a couple of straight lines again i'm not too concerned about any dimensions because i can still add these dimensions later on so the top one should be 3.7 centimeters long this one here is 1.5 centimeters long the section here in between is three millimeters long not three centimeters 0.3 and this one down here is around 0.45 centimeters and then i have turned the sketch entities into a fully defined drawing and i also want to point out that i made sure that this line here is slightly overlapping the thread then i exit the sketch select the profile run the revolve command for the axis i pick this construction line the angle is set to 360 degrees again and for the operation i choose new body in the next step i create the thread on the inside of this bottom ring and we could use the thread command again but because i'm not going to 3d print or produce this model in any way it doesn't have to be that precise so i'm going to show you a little trick here i enable the section analysis tool first when i zoom in you can see that the bottom ring of the connecting chamber is overlapping the top of the boiler so i run the combine command as my target body i select the bottom ring as my tool body i select the boiler and the operation is set to cut and i also check keep tools before i confirm the combine command and when i now hide the basket and the boiler you can see that i end up with a thread on the inside of this bottom ring then let's also perforate the top so i start a new sketch on the top plane first and then we can use already existing geometry and project edges to the new sketch plane so i'm gonna hide the ring first bring up the project command select this edge confirm this then i show the ring again and use this sketch line to make the extrusion so i exit the draw mode by hitting the q key then let's try something like -3 millimeters and before i confirm this i want to point out that the new cut does not only affect the ring but it also cuts away a little bit of the basket and that's of course not what we want so i open up this objects to cut sub menu and uncheck the box next to the basket so that the new cut only affects the ring but not the basket and then i can confirm this show the boiler and the section analysis and make sure that everything fits nicely together now i'm ready to continue with the profile of the collecting chamber so i hide the section analysis again and start a new sketch on the front plane so let's hide the boiler first so that i can select the sketch plane and then i enable the slice mode in the sketch palette so that we can see through straight to our sketch plane and the first thing i'm gonna do here is i select this edge of the bottom ring hit the p key to project it and then i start with the line command and hover over this line until it snaps to the center draw a straight one at a length of 8.5 centimeters draw a horizontal one at the top this one should be 4.3 centimeters long and then a few more at the bottom so this one is one centimeter so in case uh you draw it slightly angled you can always apply a constraint to it by selecting the line and then hit the horizontal or vertical constrain and fusion automatically detects which one it should apply based on the direction i'm gonna create another one here and another one down here then i add a distance between the end point of this line and this point here by point one five centimeters and last but not least let's turn this into a closed profile by connecting the endpoint of the horizontal line at the top with this one down here and we can also select and turn this projected line into a construction line by hitting the x key and i also add some dimensions to this line here 1.6 centimeters and another 1.5 centimeters to this line so that we turn the drawing into a fully defined sketch instead of leaving the draw mode by hitting the q key i click on finish sketch this time because i do not need the extrude command but the revolve command next so i'm gonna run the revolve command the profile is already selected for the axis i choose this center line and instead of keeping the operation to join i switch it to new body so i keep the top part and the bottom ring as a separate body for the moment this will allow me to use the shell command on the collecting chamber later on without affecting the bottom ring together with a thread so i'm going to confirm this and when you take a look at the browser tree we have two bodies in the body folder one for the bottom ring and one for the collecting chamber so far the model is pretty symmetrical and simple but i'm gonna change this in the next step when i create the beak i will use the loft command and the loft command requires two sketches so i start a new sketch at the top plane first draw a straight line starting at the origin turn this line into a construction line project the circle and i'm going to create only one half of the profile because i will use the mirror command to complete the drawing so let's draw another straight line starting at the circle and let's also add a few dimensions from this point to this point i need this to be 2.5 centimeters and from this point to the construction line another 1.5 centimeters and then i can use the mirror command so i select the straight line first run the mirror command select the construction line as my mirror line confirm this and then we can use the fillet command in the draw mode so it's this one here to add a fillet between these two lines i'm gonna type in something like five millimeters and here i also make sure that this point is coincident with the construction line this turns the sketch into a fully defined sketch and then i can already finish it the second sketch has to be located a little bit below the first one so i select the top plane first go to construct offset a new construction plane by minus 5.5 centimeters right click on the plane create a new sketch and here let's also project one of the already existing lines i'm gonna take this one here then i hide the sketch that i have previously created draw a straight line again starting at the origin turn this into a construction line again let's move this a little bit closer to the circle here and then i draw another straight line make sure that this is not a construction line by hitting the x key on the keyboard and i add a distance here of seven millimeters and the distance between this point and the starting point of the construction line of 0.5 centimeters and then i use the mirror command again so i select the sketch entity first the construction line as my mirror line confirm this and then i also run the filler command between these two edges with a radius of six millimeters again let's make sure that the center point of the radius is coincident with the sketch line and this turns the construction into a fully defined sketch and then we can already leave the sketch mode now before i run the loft command i want to point out that i have deliberately placed the bottom sketch a little bit inside the cylinder of the chamber and this is to make sure that the loft object merges into this cylinder so this makes sense in a second when i run the loft command i pick the top profile first the bottom profile second and as you can already see so the operation is currently set to cut i'm gonna switch it to join the bottom part merges into the cylinder of the collecting chamber nicely so i'm gonna confirm this it already looks very good i'm not so happy with the slide pinching at the bottom so i double click on the love command in the timeline again and change the tangent edges from merge to keep so this creates a slightly more consistent form and then i can confirm this now because we have created such a nice edge we can easily apply a fillet to it so i'm gonna select it run the filler command and this time instead of using a regular fillet i use a variable fillet so i change the radius type from constant to variable and this one allows me to change the radii on different locations so we have a starting point and an endpoint and i can click this little plus icon and move the cursor over to the edge to place a second point or third point in this case so i do not have to be precise here i can simply choose a location on the edge because i can still change its position by changing this value so the starting point is at zero the end point is at one and for the point in between i'm going to type in 0.5 to place it at the bottom of the peak for the start point let's add a radius of 1.5 centimeters the same goes for the end point 1.5 centimeters and the one at the bottom should be a little bit smaller so i go 4.4 centimeters everything looking good and then i keep it as it is all that's left to do now is to run the shell command one more time to make the collecting chamber hollow inside so i select the top face first click on the shell command at a wall thickness of three millimeters fusion gives me a preview everything's looking good and then i can keep it like this next let's continue with the nozzle in the inside so i select this surface run the extrude command by hitting the e key and if i want to make this extrusion as high as the chamber i can simply shift click on the top surface of the chamber and fusion makes sure that both surfaces align i set the operation from join to new body because i want to keep this inside part as a new body and i also change the taper angle to -4 before i click on ok and when i hide everything except the nozzle i can then run the shell command pick the bottom surface give it a wall thickness of two millimeters and confirm this for the opening of the nozzle i create a new construction plane again i offset this top surface by minus eight millimeters then i right click on it and create a new sketch and here instead of using the project function i go to create down to project and choose the intersect feature instead so this creates a sketch entity where surfaces are intersecting the sketch plane as you can see in the preview here so i select our nozzle confirm this make sure that i look perpendicular to the sketch plane then i create a straight line starting from the center to the circle turn this into a construction line draw another straight line at the top make sure that this is horizontal add a dimension in between of 0.13 millimeters and then i use the mirror command to mirror this line and i hit the s key to bring up the sketch shortcut menu i pick the circle here draw one right on the center and add a radius or a diameter of seven millimeters and then i use the trim tool so the trim tool is available in the modified drop down menu the shortcut key t is already assigned to it and i use this one to trim away some lines so i simply hover over the lines and when they are highlighted in red i can see what part of the line gets trimmed away and when i'm done i simply finish the sketch and run the extrude command use these two outside profiles and extrude them this time not in a distance but to an object and i select the top plane of the nozzle make sure that the operation is set to cut and then i click on ok the last thing we need to do to complete the nozzle is to also perforate the bottom of the collecting chamber so i'm gonna hide the basket and the boiler and also the bottom ring then i show the cross section start a new sketch on this little plane inside the bottom camber i hit the p key to run the project command then i select this inside circle click on ok and use this to perforate the bottom and for the extent i switch it to to object select the bottom face confirm this and now we have created an opening where the cafe can flow up through the nozzle and leave it on the opening at the top before i combine these bodies into one body let's create the hinge of the top lid which is also the starting point of the handle so i create a new sketch on the front plane first and before i draw any lines i go to create project intersect i select the outside surface of the collecting chamber confirm this and we have a projected line at the back and one at the front that i don't need so i select and delete it then i look perpendicular at the sketch plane run the line command by hitting l on the keyboard and then i draw a couple of lines again i have already taken some measurements on the mocha pot so i'm not too concerned about adding dimensions while i'm drawing these lines i can add the dimensions later on so before we do this i want to add a few additional constraints so let's make this line and the projected line over here parallel so i select both select the parallel constraint and i do the same for this line and let's make this one at the top horizontal and now i'm ready to add a few dimensions so i start with this one here and add something like 1.2 centimeters let's move this in a little bit and down and the bottom line up quite a bit then let's make this one two centimeters long add a distance between this line and this point or let's let's also remove this horizontal constraint at the top here and add a perpendicular constraint between these two lines so again this one is already parallel uh to the projected line so i'm gonna select this one here and this one at the top and pick the perpendicular constraint and now i can add an additional dimension between this line and this point down here and this one should be 2.4 centimeters long let's move this dimension down a little bit then i also add a distance we'll define the length of this line this one should be six millimeters high and this one down here is two millimeters long and last but not least i'm gonna create an additional line turn this one into a construction line add a distance between these two points of six millimeters then i bring up the shortcut menu draw a circle with a diameter of 0.3 and then i make this circle tangent with this point by selecting the tangent constraint first then i select this circle and this point and let's also make sure that this point here is connected to this line so i simply drag and drop it to the end point and i make this line also horizontal the last thing i need to do before i exit the sketch mode is to add a vertical constraint to the center point of the circle and the end point of this construction line then the sketch is fully defined i can finish it and run the extrude command and this time i set the direction to two sides and extruded by five millimeters on each side then i make sure that the operation is set to new body click on okay and as you can see there is a little gap between the cylinder and the newly created object and we can simply close this by selecting this face so i'm gonna zoom in close select this one and now i go to modify use the press and pull command to shift this face a little bit to the front so it intersects with the cylinder like so and last but not least i'm gonna run the combine command and now i can select all four bodies make sure that the operation is set to join click on ok and then everything is combined into one solid body to literally round this part off let's add a couple of fillets so i set the radius type to constant first and then i select some edges type in something low like 0.05 and then i control click to add more edges to the selection maybe also this one on the inside and a few on the nozzle and also these at the bottom then i can confirm this and show the other parts of the mock-up hud so by now you are maybe already aware that there exists many different approaches to build parts in fusion 360. we have only used solid so far but after a short break i show you how to use t-splines and surface modeling tools to build the handle and the lid now for the handle i have decided to try a slightly different approach we are going to use t-splines but before i build the handle i create a new component so go to assembly new component i also make sure that the top level assembly is selected before i do this if you working on one of these components inside this top-level assembly it's going to create the new component inside the selected or the currently active component so i'm going to call this handle and then i go to insert and insert an image that we can use to trace the handle i have prepared this one and i'm required to select a plane so i'm gonna hide the border and the basket first then i choose the front plane so that the image gets inserted on the front plane we have to flip it horizontally and then i use these little handles here to scale it up and i do not have to mess around with the scaling here i can simply confirm this then open up the handle component the canvas folder right click on the canvas and select calibrate then i pick two points on the image this one here and this one up here and tell fusion that the distance between these points is approximately two centimeters then it scales it accordingly i right click on the image again select edit canvas make sure that i'm in the front view and then i move it in place and to do this right make sure that the camera is set to autographic instead of perspective and i can use the gizmo here to position the canvas like so and when i'm done i simply click ok when you take a look at the toolbar you have probably already noticed this purple create form icon so when i click it i enter the form mode or the t-spline mode and before i can place any of these 3d primitives so i select the box first i have to choose a plane so i'm not going for any of these coordinate planes but i zoom in and try to select the plane of the hinge so it's this one here then i set the rectangle type from center to two point and then i draw the box on top of this face make it a little bit bigger like so i also gonna limit the amount of edges for the length to 1 and also for the height to 1 i'm gonna keep the second edge for the width because i will use the symmetry tool later on and then i confirm this free form objects are special because they behave a little bit like subdivision models and one of their characteristics is that the transition between single faces remains always smooth so you can open up the utility tab and select display mode and the first mode shows the freeform object as a box or in box mode the second mode it displays the freeform object in box mode together with a smooth preview and the third one is the smooth display so you will see me switching between these modes when i adjust the mesh but for now i keep it in smooth mode i select symmetry select the face on the left and the one on the right then i confirm this and as soon as this green line appears it means that the symmetry mode is now enabled then i go to the modify tab again search for decrease function and select the edges at the front so that they align a little bit better with the surface of the hinge then let's make the top and the bottom curve a little bit less round so i'm gonna switch to the box mode modify babble i select the top edge and the bottom edge decrease the value a little bit and then i go to the modify tab again slide edge select the top edge and the bottom edge and slide these guys a little bit more to the center and when i switch back to the smooth mode again you can see that the top part of the handle is slightly less round and that's exactly what i'm looking for so i go to the modify tab again this time i select edit form i make sure that the selection filter is set to all or two faces i select both front faces so even if symmetry is active here i select both of them switch to the front view and then i extrude these faces by holding down the alt key and then i simply drag the front face to the right i can also rotate it a little bit and i do this a couple of times and loosely tried to match the shape of the handle let's create one more around here and we can probably move this up a little bit and then create a long extrusion and an additional short one at the bottom i'm always keeping the alt key pressed while i extrude these faces and then i switch to the vertex tool zoom in a little bit select these vertices and then try to follow the curvature of the handle so it doesn't have to be perfect for this demonstration but you could literally spend hours creating nice looking forms so controlling them is pretty easy so don't forget that you can rotate the entire structure in case you have to and then let's also take a look at the handle from the side view i'm gonna select the guys at the bottom move them in a little bit and when i'm done i simply click on ok in the edit form dialog box take one last look at the geometry and then i exit the form mode by clicking on finish form as you can see we have a form icon in the timeline so in case you have to change something you can simply double click this icon to enter on the form mode again make your adjustments here and when you are done you can exit the full mode by clicking on this button let me also enable perspective again so that i get a slightly better idea of what the handle looks like in 3d and i also show the basket and the boiler again and i turn off the component color cycling toggle and i think it looks pretty good so after a short break we can continue with the lid of our mocha pot prima fascia the lid seems to be pretty simple but when you take a close look you can see some slide form changes it's a little bit thicker at the back where the hinge is and it's a little bit thinner at the front and when you take a look at it from above you can see that the front is also slightly overlapping the opening of the beak and i will try to consider these slide form changes and we will also take a look at the tools that you can find in the surface tab before i create the first sketch i make sure that i'm in the top level assembly then i go to assembly and create a new component let's call this one lit make sure that it is active i then also show the component colors hide everything except the top part and then i start a new sketch on the top plane by clicking on it then i click l on the keyboard for the line tool to enter the draw mode and here let's bring up the shortcut menu by hitting the s key then i draw a circle and i make this circle equal to the outside diameter of the collecting chamber and then let's draw a straight line starting at the origin over to the beak turn this one into a construction line by hitting the x key on the keyboard then i bring up the shortcut menu again by hitting the s key type in arc and here i choose the three point and create a small one here and a slightly bigger one at the front to create nice forms it is important that these arcs are tangent and as i'm going to mirror both sketch entities using the horizontal construction line i'm also gonna draw a vertical one turn this line into a construction line two then select this line and the arc and click on the tangent command again so that we have also a tangent consistency when i mirror both arcs in the next step so i double click on one to select all of these sketch entities run the mirror command choose this horizontal construction line as my mirror line when i now click on ok zoom in a little bit select both arcs right click on them and show the curvature combs then you can see that we have a perfectly smooth transition from the top arc to the bottom arc so when i hide the curvature comps again and let's get rid of this um tension constraint here just to give you an idea what it looks like when it's not tensioned then i move this line in a little bit so you can already see that a crease appears here and when i now show the curvature comps again by right clicking on them and toggle on the curvature display you can see that the combs are slightly overlapping in the center and that's of course not what i want so i undo this until the tangent constraint appears again and then i hit the t key on the keyboard to run the trim command and trim away these parts of the circle then i can already select the sketch profile hit the q key to exit the draw mode and run the extrusion command at a thickness of 6 millimeters and let's also change the component color to something else so that we can see things a little bit better i'm gonna keep the orange one and then i start a new sketch on the front plane so this is gonna be the sketch that i will use to cut away the top part of this extrusion and before i draw any lines i go to create and run the intersect command select the surface at the front and the big one here to get a projected line at the back and one at the front and then let's draw a straight line add some dimensions so that i can place it right in the center of the extrusion so the extrusion was six millimeters and the position of this straight line should be at three millimeters and let's draw also another straight line at the front and add a dimension of one millimeter with a radius in between or fill it in between these straight lines of 2.5 centimeters and i also add a length to this line something like 6.2 let's move this guy a little bit closer to the front and add another three point arc at the back make sure that this one is tangent and then i can already finish the sketch next we can use the sketch to split the bottom part of the lid so i go to modify split body the extrusion is my body to split the splitting tool is the sketch that i've just created and fusion shows us a preview and the red plane here indicates where the splitting takes place i'm going to confirm this and when i open up the component and the bodies folder you can see that i now have two bodies in it a top part and a bottom part i'm gonna keep the bottom part right click on the top body and select remove and a new remove icon appears in the timeline now i can already continue to build up the cone like shape that makes up the lid and for this reason i'm gonna delete these top faces and this is only possible when you switch from the solid to the surface tab now i select all of these top faces and simply hit the delete key on the keyboard as soon as i do this the solid body turns into a surface body so when you take a look at the browser tree here while i move the history marker over to the left you can see that i was starting with a solid body so this is also obvious when i show the section analysis the cross hatching marks the solid material and when i move the history marker behind the delete face command you can see that the solid body turns into a surface body the cross hatching is gone and we are now looking at the rear side of our paper thin surfaces and they are usually tinted in this brown gold color for the surface loft extrusion we need an additional sketch so i'm gonna create one and i create one that sits a little bit above the bottom part of the lid so go to construct offset plane choose the top plane to offset and offset it by 20 centimeters then i right click on this plane create a new sketch and draw a circle right on the origin with a diameter of one centimeter then i finish the sketch let's also hide the chamber and then i go to create loft and now i start to control click on all of these bottom open edges let's make sure that we do not miss any of them so this is my first profile and my second profile is the circle fusion already provides me with a preview it is looking very good so i'm gonna keep everything as it is and click on ok in the loft dialog box as you can see the circle at the top is still open we can change this by running the patch command then i select the opening here and confirm this so it looks like nothing has changed because we still see this brown color and this is simply because the normals of this newly created face are flipped so it's this one here i can simply go to modify reverse the normals select the top part and click on okay so this is not necessary for the next step but it makes things a little bit more clear and before i knit everything together let's turn on the section analysis one more time as you can see the surface body that currently consists of three parts is still hollow inside so i'm gonna hide the section analysis again and then i go to modify and here i run the stitch command it's also available up here i select all three faces the green lines indicate where the stitching takes place and then i can confirm this and as soon as i do this the surface body or the three surface bodies have turned into one solid body so when i move the history marker over to the left again you can see that the bodies folder contains three surface bodies and as soon as the knitting is done fusion turns all of these surfaces into one solid body again and i can also prove this by running the section analysis and now the cross hatching marks the solid material in the inside of this solid body then let's add a wall thickness this time i do not use the shell command so let me hide the collecting chamber first i start a new sketch at the bottom face here i draw a circle with a diameter of 8 centimeters i exit the sketch mode by hitting the q key and then i extrude this by minus 1.8 centimeters with a pretty huge taper angle of minus something like 64. this is looking good probably a little bit too high so i'm gonna lower it and then we can keep it like this all that's left to do now is to add a sphere on top so i switch to the solid tab go to create choose a sphere primitive for the plane i select the top plane and then let's draw one with a diameter of 1.6 centimeters and instead of a cut i set the operation to join or probably have to reposition it a little bit so i set it to new body first confirm this select the sphere and run the move and copy command and here i set the pivot to the center of the sphere first and then i move it in place by simply using this gizmo so let's move it up a little bit and last but not least i combine both bodies into one solid body again let's also unhide the connecting chamber again to see if everything fits perfectly on top to complete the mockerbot let's create a second part of the hinge that is connected to the lid so i start a new sketch on the front plane zoom in a little bit and the first thing i'm going to do here is i project this line by hitting the p key and then let's start drawing a couple of straight lines and when you click and hold the left mouse button clicked the straight line turns into the arc tool when i release it i can continue with a straight line again and when i click and keep it clicked i have access to the arc tool again and let's close this off with another straight line and another line here so let's add a vertical constraint to this one a horizontal constraint to this one and let's also add a few dimensions so this line should be 0.55 the one over here let's make it vertical first and then i also make sure that this line and this arc are tensioned by selecting both and then click on the tangent icon at the top and let's add a length of 0.45 to this one a radius of 0.25 to the arc at the top and another radius here at the bottom of 0.45 and then i'm going to move everything a little bit closer to the center and last but not least i also project the circle and the inside and as you can see quite a few lines are still blue so the sketch is not fully defined yet but this is totally fine it doesn't always have to be a fully defined sketch as long as it is a closed profile and we use this closed profile in the next step to make an extrusion and i also want to point out that i have not connected this line to the lid so the hinge and the lid are not touching but this will also make sense in a second so i'm gonna finish the sketch and extrude the sketch this time again by two sides and let's enter one centimeter on both sides i also make sure that the operation is set to new body and then i click on ok to connect the hinge with the lid you can simply select the front face then run the extrude command and instead of distance i choose to object and then i select this round surface here and fusion connects the hinge perfectly with the lid so i'm gonna keep it as it is the operation is set to join and we have now turned two bodies into one body then let's start a new sketch on the top plane of the hinge i draw a construction line again and select the two point rectangle and instead of using the two point rectangle i switch to the center rectangle draw one here add some dimensions so let's make this one a little bit wider than the hinge that is attached to the collecting chamber and now i'm already good to go to exit the sketch mode by hitting the q key i select the sketch height the collecting chamber and then let's cut straight through the hinge and then i probably delete these holes here again because we don't need it to make the hinge work and the great thing about parametric modeling is that we can always go back to a previous state in the history and adjust the model so it was this extrusion here by double clicking on it i enter the feature and here let's not only select the outside profile of the sketch the build c extrusion but also the circle on the inside to get rid of the holes on both sides and when i click on ok the model updates the way it should then let's create a pin in between the two parts of the hinge so i zoom in select uh face on the inside enter sketch mode then let's hide the lid for a second run the project command select the circle and then use this profile exit the draw mode by hitting the q key and instead of a distance i pick two object and select the opposite face and then let's show the collecting chamber again and to be able to connect both using joints i have to ground one object first so in this case it's the collecting chamber i right click on it and select ground when you look at the timeline it seems like nothing has changed when i was selecting the ground command for the collecting chamber before but as soon as you switch to the top level assembly and go to the very end of the list you can see that we have a new ground command here so i switch back to the lit component go to assembly joint and i zoom in a little bit hover over the pin select the center point of the pin then the lid gets transparent so that we can see through it and select the point on the hinge that is mounted to the collecting chamber and here i also go for the one that sits in the center of the hole so it's this one here the motion is probably currently set to rigid so i do not get a preview but as soon as i switch it to revolute the lid starts to rotate around the joint that we have just defined so i'm gonna keep it as it is and confirm it and now we can move the lid or we can open and close the lid but unfortunately it still goes through the geometry so we can change this by right clicking on the join command and edit the joint limits so i set a minimum and the maximum the minimum remains at zero and the maximum value could be something like 88 so i'm gonna set the minimum back to zero the maximum to 88 click on okay and now we can open up the lit as you can see we have some slide intersections here between the hinge and the lid and this is something we would have to change by modifying the back part of the lid but i'm going to keep it as it is for the moment and show the other components of this design the last thing i want to show you in this tutorial is how to change the appearance so i go to modify appearance and currently this steel material is assigned to our parts i double click it make it lighter quite a bit and then let's search for a plastic mat material i choose the black one and let's assign it to the handle and then i switch the selection from body's components to faces and assign the same also to the sphere at the top of the lid by double clicking on it i can adjust the color let's make it lighter just a tad then i right click on the steel material and duplicate it double click on it choose a different color faces is still selected and then i apply this to the outside of the collecting chamber and of course also to the beak we leave the top face as this and complete the bottom faces and also the hinge then let's duplicate this one again double click change the color and apply this color to the boiler and then let's also add the bialetti logo to the collecting chamber so i go to insert this time not canvas but decal i look for an image on my local hard drive well it's this one here then i select the face rotate the image by 90 degrees so minus 90 degrees in this case scale it up a little bit move it in place and as you can see it perfectly follows the curvature of the surface maybe this is a little bit too big let's move it down just a tad perfect we are done that's it for this fusion 360 beginner tutorial thank you very much for your interest i really hope it was useful if you like the content subscribe to my youtube channel leave a comment in the comment section below if you have any question like the video you can even buy me a coffee the link is in the description so thanks for tuning in and see you in the next one cheers i love good coffee

Channel: 3D Gladiator

Views: 169,801

Rating: 4.9110012 out of 5

Keywords: kevin kennedy fusion 360, lars christensen fusion 360, fusion 360 beginners, learn fusion 360, fusion 360 beginner lesson, fusion 360 tutorial, 3d gladiator, fusion 360, cad design, inventor, solidworks, 3d modeling, Autodesk, autodesk fusion 360, industrial design, 3d printing, cnc milling, cnc, 3d design, 3d artist, Manufacturing, 3d printer, cam, 3dconnexion, Wacom, 3d scanning, 3d scanner, learn fusion 360 in 30 days, fusion360, car design, 3d car modeling, 3d tank model

Id: mK60ROb2RKI

Length: 90min 54sec (5454 seconds)

Published: Fri Jan 08 2021