Fusion 360 Modeling - Modeling from a Print. Modeling Introduction.

hello and welcome my name is Mike matira and I'm going to walk you through a on modeling in fusion 360 in most cases demonstrations of modeling will show you from a designer's point of view the kinds of things that you can do its freeform design and it's all from within your own imagination in this lesson we're gonna talk about creating a part from a blueprint people may go to a manufacturing facility with a blueprint or possibly even a sketch on a napkin and ask someone to make that part so you're not designing something that's your imagination it's theirs so this lesson is about reading a simple print and creating a simple model at the time this video is produced Fusion is going through a change in the interface they're switching to a tabbed toolbar as you see here the current release will allow you to view that by going to your profile over in the upper right corner selecting preferences and under preview you can select UI preview that'll make sure that your interface matches mine as you go through this lesson now we're gonna do this as one continuous video but remember you can stop this at any time and I encourage you to stop and work through the process now there are a couple of different ways to model apart you can create a solid model or you can create a surface model the main difference between solid and surface modeling I like to think of as the difference between a stick of butter and a balloon now a balloon is hollow surfaces and surface modeling is kind of like a balloon you have a skin stretched across the outside of the part but the inside of the part is hollow whereas with solid modeling the stick of butter example if you cut into a stick of butter there's still butter on the inside we're gonna be creating a solid model of this part now if we have a look at this it's a simple prismatic part it's a rectangular part with fileted corners there's a pocket that will be cutting in through the top and through the front and back face there's an oval-shaped slot there are some holes in that slot that go all the way through the part now the modeling process requires us to create a sketch of the basic profile so let's start with our sketch right here we have create a sketch when you select that it shows you three planes it wants you to select the face that we will be creating the sketch on now you can select any of these but I always like to view it as though it's going to be sitting on my table so I'm gonna select this plane now yours may have flipped up into that top view automatically I have that turned off in mine but if you want to switch your view you can come up to the upper right corner on the view cube and double click where it says top that'll switch us to a top view we can also move around the graphics area by using our mouse we can use the wheel on the mouse to zoom out or to zoom in you could also hold down the wheel on the mouse and pan left or right now I'm going to move it over a little bit so I've got roughly a six inch view by a 4 inch view because that's what it shows on our print for the overall size of the part I'm going to start by creating the basic outline which is a rectangle and I'll create a two-point rectangle my first point is going to start from the origin give that a click slide over and you'll see as I slide over there are dimensions that are showing me how big this rectangles going to be now I could just click the second point and come back and dimension the rectangle later on or I could just say for the X dimension I want six and then I can tab over to the other box tell it I want this to be 4 and when I enter that it gives me a dimension rectangle you'll also notice that the outside profile of the rectangle is in black that means the rectangle is fully constrained very simply that means there's no guessing about what the Sai is the system knows exactly what the size is and it's locked down and fixed and that's all we need for the first part of this so we're going to stop our sketch at this point you can rotate over to a tilted view or you can grab your corner of the viewcube and slide that up and over now to create the basic profile of our part we need to extrude this rectangle down for the thickness and according to our print the thickness for this part is an inch and a quarter to extrude this will come up here and select the extrude command it wants us to pick the profile that will be extruding which is this boundary we created I'm going to drag this down in the negative direction and it shows me here I move that to a negative inches I'm gonna make that minus 1.25 and we could tell it to create a new body or you could also create a new component we'll talk about that more another time for now we'll just leave it on new body and we'll okay this now we have the basics of our rectangle the next thing we want to do is round off the corners and according to our print it shows that the corner is actually dimensioned as a diameter it shows a value of the radius from the outside to the inside of the pocket and it's one inch so that means this outer radius is going to be a half inch for this we can select the fill it command off of our toolbar and we can pick these vertical corners now you'll see when I mouse over that corner it highlights I can select each one of these corners now remember to rotate around you can hold down your Shift key hold down the wheel on your mouse and rotate there are other ways to pick that but for now I just wanted to show you how to rotate the part now I can grab the arrow and move it in until I get to a half inch but if it's not going right to a half inch for you simply key in 0.5 and enter the value now we have the basic outside profile of our part next I want to create the profile for the inside pocket we're gonna be drawing that pocket on this top face we'll create a new sketch for that so select create sketch and it asks you which plane you want to create this in now I could pick this plane right here because it's the same plane as the top of the part but it's important that you pick things that keep a relationship I don't want this sketch to be in relationship to this plane I want it to be in relationship to the top of this part so if the top of the part moves for any reason I want my geometry to move with it so we'll select that as the surface that we're going to be drawing on now according to our print it shows that we have a wall thickness of three hundred thousandths so basically I need to shift this outer wall in 300 thousands to start with for that we can use the offset command so I'll select offset with offset I can pick an individual wall or I can pick a continuous chain we want to offset everything around the outer boundary in 300 thousands so we'll leave that set to chain I'll select this outer curve I'll grab the blue arrow slide that in and I could slide that until I get to 300 thousands or I can just key in 0.3 and okay that next we need to create the circle that matches this inside for the holes so I'm going to go to center diameter circle we're gonna pick this point which represents the center of our circle and instead of keying in a dimension I'm just gonna slide out until it connects to the endpoint of the line and the fill it when it does that it should be at exactly one inch and I'll do this here pick my center point and pick this outer edge of the line again they're all black because they're locked down this edge is locked down in relationship to the outer edge these circles are locked down from this center point and also connected to the outer edge so everything is constrained to some other existing geometry now in some systems you might have to go and trim this together and cut away the sections of geometry that you don't need with fusion all we really need is this inside boundary here we'll leave it just the way it is we're going to stop our sketch we're going to do another extrude I'm going to pick the area that I want to extrude and I'm going to move my arrow down and because it knows we're going down into an existing block it knows that the operation type is going to be a cut boundary we're cutting away the inside of this pocket and I could slide that down till I get to one inch which is what my print calls for for the total depth of the pocket and then I can okay that next we need to put some fill it's in these corners and according to our print it says that is a two hundred thousands radius fill it in each one of those corners so again we're gonna go to the fill it command and I'll pick each one of those vertical edges now again you can't always see what it is you're picking sometimes when you mouse over it you'll be able to grab it you can also hold down your left mouse button and then it shows you all the choices that are available so when I see the edge that I want I can grab that but in some cases you may have to rotate it a little bit to get exactly what you want with all of those verticals selected I can key in a value of 0.2 and enter that and we've created a fill it on all the sharp edges inside the pocket so we need to create a counterbored hole and each one of these corners now for that we're gonna need some geometry again I'm going to create another sketch sketch is gonna be on this top edge the geometry I'm going to create is going to be a point and when I mouse over this area it should find the center point you'll see a circle show up that's showing us it's actually grabbing a center of a circle if you're not getting that you may need to zoom in a little bit so with those four geometry points selected will stop this sketch I also want to show you that all of your sketches are listed here in the tree under sketch and each time you use a sketch it gets turned off right now the sketch for our points are still visible let's create those holes so we're going to go to create and I'll slide up to the hold command and we can tell it what kind of hole we're going to be creating and where those holes will be located so I'm going to grab each one of these points as the location for the hole and for my hole type I'm going to set this to a counterbored hole now according to our print the top diameter for the counterbore is 0.5 62 the diameter for the drilled hole is 0.3 91 the depth for our counter bore is shown as 0.4 and here it shows an overall depth of an inch and a half but to make things easier we're gonna tell it the extent for this hole is going to be through all that'll make sure it goes all the way to the bottom of the part and again because of the associativity of the model if later on I make this part thicker this hole will still pass through the bottom of the model it's better than putting in a specific depth let's okay that and now we have our counterbored holes next we're going to work on the slot that's shown on the front side of the part so we'll be working on a completely different plane than we have been now according to our print it says the slot is two inches wide and end a half-inch wide in the y-axis and it's located three inches from the edge of the block and the center is a half inch down from the top of the block now these are the important things you have to remember when you're creating someone else's drawing is to draw it the way it's shown on the print the print is your rule book and you have to do it the way it's shown on the print now we might change this later on to make it a little more flexible and associative but for now we're gonna do it exactly like the print so I'm going to create a new sketch when it asks for the face that we're creating the sketch on I'll pick this front face of the part and now I want to move so that I'm perpendicular to that face so I'll click on front on my view cube and I'll roll my wheel to zoom up a little bit so to start with we're just going to create the slot itself and then we'll worry about positioning it so I'm gonna go to slot and there's several different types of slot we have one here that's an overall slot and that's the way our part is dimensioned it's the overall length from end to end so I'm basically going to pick a point here slide over I can make that two inches now if I wanted to and then click my second point and then slide out and if it's not clicking to a half inch dimension I can just hit point five and hit enter now this time you'll notice the slot is blue that's because it's not constrained it's just a two inch by half inch slot sitting somewhere on that face it's not anchored to any reference point to anchor it we're going to create some dimensions so you can hit D on your keyboard or you can select sketch dimension off of your toolbar first you want to pick the thing you're going to dimension so I'm going to grab this centerline of the slot and then I'm going to grab this top edge of the part and I'm going to slide over here click that in position and tell it that that needs to be at 0.5 next I want to grab the middle of the slot and there's nothing to grab in the middle so I'm going to hit escape to break out of my dimensioning command and I'm gonna go to create a point and this time I want to put a point at the center of this line now when I get to the midpoint it shows me a triangle so I'm on the line and I move to the middle and when I see that midpoint they give it a click now I have a point that is constrained to the middle of that line I'll hit escape to break out of the point command I'll go back to my sketch dimensions and I wanted to mention that point in reference to this edge and tell us that that needs to be at a dimension of three inches now you can see everything is black because everything is constrained let's stop the sketch I'm going to tilt my view a little bit so I can see it better as I do an extrude of that profile moving my arrow in so it does a cut operation and I want to move that in a distance of minus 0.2 as it's shown on the print next we're going to put those holes in now our print says that those are quarter inch holes and they're basically at the center of each one of these arcs so we're gonna create a new sketch those holes are going to be on this face which is the bottom of the pocket I'm gonna create a circle that goes from that diameter out and I'm not going to worry about the dimension I'm just gonna click it anywhere for right now I'm going to do another one over here and again you can zoom up if you need to see this better or you may need to rotate around to see the center so we'll grab my center point I'll slide out and click my second point again they're blue because they don't have an actual size it's just wherever I click them into position I'll hit escape to break out of the circle command I'm going to do a sketch dimension could have dimension that circle and I'm going to make that a quarter inch diameter now I could do the same thing over here I can grab this circle and slide out and it shows me the current value of that circle and I could key in a quarter inch or I could click on this mention and create a reference so now this dimension will be the same as this one and when I hit enter you'll see they're both a quarter-inch that way if I come back here double click on this and change it they both change that's all we need we're going to say stop sketch I'm going to go to the extrude command I'm gonna grab the center of each of these circles I'm gonna zoom out a little bit so I could see a little bit better you can move my arrow in the other direction so it knows I'm doing a cut operation and for my distance I'm gonna tell it all that means it will cut all the way through the part again so no matter what size the part may change to later on those holes will always go all the way through the part and will okay that now we can see we have the holes on both sides you well the next thing we need to do is to create the slot on this back face so again we're going to create a new sketch it's going to be reference to this back face I'm going to go to create go to my slot options this time I'm gonna do a slot that goes Center to Center I want to grab the center of that circle and move out to the center of that circle and I'm gonna slide out and key in a dimension of a half-inch that's all we need and again it's all black because it's fully constrained these center points are locked down to the existing holes and I keyed in the width of the slot as a half-inch so let's stop this sketch will create a new extrude for this area dragging into that direction a distance of minus 0.2 and that completes the part so that's everything that was on the print fully modeled according to the customer's specification so what did we learn well we learned how to create a sketch we learn how to create sketches on different planes and on different faces we've used those sketches to extrude to create a new body and to extrude to cut away from a body we've created lines points arcs and circles as our base sketch geometry we've learned a little bit about creating constraints and we've created a fully constrained solid model so what are the advantages of having a parametric solid model like this well let me show you what we can do if we expand our sketches I'm gonna go to my initial base sketch which was my first rectangle I'm gonna right click on that sketch and I'm going to tell it that I want to edit that sketch so it goes back to its simplest form when we first started on this part and I'm gonna tell it I want this to be eight inches and I want this to be six inches stop the sketch and you'll see the whole part updates now the slot stayed in the same position because this slot was referenced to this edge if this slot had been referenced to the center of this wall it would have moved proportionately so it stayed in the center so how you design things can be very important when you're creating a solid model I can change that back I'll right-click on the sketch edit the sketch make that six make that four stop my sketch you can also reference those through the timeline if I wanted to change that inside fill it I can mouse over until I see the inside fill at highlight I can right click on that and tell it to edit that feature and instead of two hundred thousandths I'll make that three hundred thousands so if for some reason the customer comes back and gives you a change in a dimension this makes it real easy to modify your part without having to start over and that concludes this lesson thanks for watching

Channel: Mike Mattera

Views: 57,616

Keywords: F360, Fusion 360, Fusion CAM, Autodesk, Autodesk CAM, Autodesk HSM

Id: 6wMzp8fZj18

Length: 25min 30sec (1530 seconds)

Published: Thu Nov 01 2018