360 Live: How would you make that?

[Music] [Music] [Music] [Music] [Music] [Music] [Music] [Music] [Music] [Music] hello everyone and welcome to another fusion 360 live my name is brad talas from autodesk uh today's topic is going to be uh how would you make that and this actually came from a customer um there are some sample drawings i'll show you this is one of those and he was like i don't even know where to start so i thought this would be kind of a cool example of you know how would i approach this and i actually have a couple other examples also that i'm going to bring up if we have time permitting let me start out by saying i hope everybody had a wonderful christmas break and new year's i have angelo helping me out on the q a today so let's dive right in um i'm actually going to start out um with something that so back a couple live streams ago we were working on this pencil sharpener and we were doing these gears and i was kind of complaining about how it was kind of difficult to figure out how many degrees when you come in here and you do a a motion link let me uh capture my position here um and i click my two the two joints or whatever um like this guy in this guy it's asking for um an angle and i was talking about how you kind of have to figure out and kind of tweak with it and play with it and i'm going to give a shout out to our friend um blaze barrett he shot me an email and he's like you know you can just type in the number of teeth and it'll figure it out automatically and i was like no that's not true and guess what it actually is so check this out um here's just a quick example so you can see i have a 24 tooth gear and i have a six tooth gear and right now i don't have any motion link between the two so i'm going to come in here say motion link it's going to ask for the two revolute joints i'm gonna click that guy and that guy and you can see it kind of gives a quick little animated preview so for this larger one which was this rev one i'm gonna put in six teeth and for the smaller one i'm going to put in the 24 teeth let's reverse it and instantly you'll see the animation updates accordingly and i i think i was blown away i didn't know you could do this so so blaze and actually a couple other people mentioned this too in some of the comments i can't remember all the names um you know so high five to all of you out there that knew this trick that i didn't know i wanted to make sure i shared that with all of you so all you have to do is type in the uh the number of teeth so i figured we'd start out with that cool tip um you know give a give a thumbs up if you like that so if you didn't know that let us know in the comments because i'll be honest i didn't know it so okay what we're going to do is we're going to create this part here and the drawing like i mentioned um there's a web page out there where a guy has a bunch of sample drawings they're they're in a different language and stuff like that and this was the drawing that the customer sent me and unfortunately i wouldn't say this is the best drawing out there there's a lot of missing dimensions or some assumptions that we're gonna have to make so for example this line right here it doesn't say how you know where it's located so we're going to assume it's tangent with the circle here you can see there's no vertical dimension over here no vertical dimension over here so as i was looking at this drawing i'm like man how how would you start this and and uh you know how would you figure this out well if you kind of look at it it's almost two separate that are kind of connected together and that's how i would approach this so we're actually going to start by drawing this vertical section first and then we're going to come back and we're going to create this horizontal section second okay i've linked this drawing i've linked my outline in the description of the video so you'll have access to these so i'm going to be referencing this drawing as we're going through okay so let's go ahead and get started here so i'm going to first of all make sure that my units are in millimeters for this one so i just click on that little edit or change active units we'll set it to millimeters i like to create a new component even though it's a single part i just like to get into the muscle memory of creating everything as components so we'll call this uh part um 214. i'll say okay and now i have a component like so we'll create a sketch and i'm going to create it on the front plane i kind of like to define everything on the front plane and then we'll use the drawing so let me jump back to the drawing here so we're going to be creating this front view or this this vertical section here i like to kind of pick something that's kind of my zero zero point and so i'm going to pick this um 30 millimeter diameter circle right here as my zero zero so i'll just go ahead and click there we'll type in 30 for the circle and there we go i'll do another circle now this one's a radius and so i'm just going to click somewhere like so d for dimension and you'll notice by default it's trying to do a diameter dimension but if i right mouse click i can do my radius dimension i've shown this in in other live streams so let's go ahead and make that 27 like so and then looking at the drawing real quick there's another circle down here again it doesn't show like how far over from this circle it is so we're gonna have to make some assumptions there probably have to wait until we get some other geometry built we do know that it's 50 millimeters down so i'm just going to draw another circle kind of down here somewhere and that is supposed to be a 24 millimeter diameter and i know that it is 50 millimeters down so that was pretty close 53. so i'm going to type in 50 and now that circle is down in the correct location okay so we kind of got the the larger circle the radius 27 the diameter 30 the diameter 24. now what i want to start doing is creating the rest of this geometry here and like i said we're going to kind of make it into two separate parts that are kind of joined together again i'm making an assumption that this line here is in line with the center of the circle so i'm just going to kind of mock up this shape over here in fusion so using the line tool i'm just going to get sort of close to vertical i'm going to over exaggerate over here just so you can kind of see what i'm doing here i'm going to make sure i come straight down i'll come straight over i'll come up a little bit and i'm just going to go to the left i have no idea how far and i'm just going to go up a little bit i have no idea how far we're just kind of mocking up the the shape of the part okay now i want to obviously make sure that this thing is correct so what i want to do is make sure that this line is in line with the center of the circle so i'm going to click on that end point say horizontal vertical and i'll click on that end point there and you can see that it moved over it's changed color to say that that's fully constrained okay we know the uh the width of this little rectangular area is 56 millimeters and then we know that the circle is um 20 from the bottom okay so we can use that information so i'm going to put a dimension here that is supposed to be 56 according to the drawing okay and then i want this circle to be right in the middle of this rectangle so check this out i'm going to put a in fact i'm going to move this dimension down just a little bit like so i'm going to put a dimension from here to this edge and i'm going to place that dimension okay now what this allows me to do is i could type something in or i can click on this dimension and you can see that it references it so i just clicked on that 56 it referenced that dimension and i could say i want this to be half of whatever that dimension is so i'm going to say divided by 2 and you'll see that that circle moved over a little bit and what's neat about this is like if i say make that 40 that's always going to stay in the center because this formula is using whatever that number is divided by two so instead of me having to do the math or whatever we'll let fusion do the work for me so if this was you know 73.5 or something like that that's going to figure out the correct formula and that circle is always going to stay centered so pretty pretty cool trick that you can do math like that um i mentioned that this was 20 millimeters down so i'll just bring that over here we'll say 20 and now you can see we're starting to kind of define the location of this area now again another assumption i'm making here is that this line is in line with the bottom of this 27 radius circle here so let's do that so basically it's going to be in line with that so i could come in here and say i want this to be horizontal vertical with that point there and you can see it moves that up and so now that line is in line with that point there okay the only thing i have left is this little guy right here and again according to the drawing we don't really have any information about how far over that is or anything like that so what i'm going to do is i'm going to use this 145 millimeter radius and start building that and then having that line connect to that radius so let's go ahead and draw a circle again just kind of out here in space somewhere i don't really care what size then i'm going to come back and dimension it right mouse click and instead of diameter i want it to be a radius and it's going to be a pretty large radius 145 and we can see it created a pretty large circle now a tip that i like to do is i like to get the circle kind of where it's supposed to be not exactly like i'm not going to try and get it to touch that circle right there i'm just going to get it kind of like so maybe i'll uh you know grab this point kind of bring it a little bit closer to where it needs to be okay the reason for that is if i had left like this circle down here and i said i want this circle to be tangent with this circle up here it's actually going to snap it and make it tangent down in this area over here so it's going to go the closest that it can and so that's why it's better to kind of get it where it kind of sort of needs to be like that okay then we can come in and say i want this circle to be tangent with this circle and sure enough we can see that that did that okay and then i want this point in fact let me move this point down so we can kind of see what's going on i want this point to be coincident with this circle here so i'm going to say coincident that with that and we can see how it brought the circle down and that point is now coincident with that circle well the last thing is we can see that this height should be 16 so i'm going to throw that dimension on there so let's throw a dimension on this edge right here and type in 16. and we can see that that circle is tangent there and this is tangent there or coincident there and i want it to be let's just say in line with the the center of this circle so the last thing i'll do is a horizontal vertical i'll say i want um that point to be horizontal vertical with that point there and you can see that sure enough everything has now turned black which means that it's a constrained sketch in fact if i expand this guy open we can see that little lock icon on my sketch means that everything's locked down so we're good to go so it took me a little bit of effort to figure out like you know making assumptions but you can kind of see as we came through we line things up we use dimensions to define where things were located you know some of this stuff here we just said make it in line with that point there but we don't know what this length is we knew what this length is and we wanted to be in line with the center of that circle okay so now i have the basic shape now i could come in and trim this circle in my sketch but honestly i don't really ever do that i just like to come in select my profiles and we'll say extrude now this is a pretty symmetric part so i'm going to change my direction to be symmetric and what that means is it's going to extrude in both directions the same distance it's going to keep my sketch kind of in the middle when i do symmetric you'll notice i get this measurement option half length or four or whole length i'm going to say whole length and the overall distance is supposed to be 22 i'll say okay and i now have that part created it's got some filleted edges so i'm going to select one of those edges and say fill it six millimeters again according to the drawing i'm just going to go through and select the other ones and you'll notice because i'm in the fill it command it's only letting me you know it's allowed me to probe through and click this edge without even having to rotate so kind of a cool little trick okay i'll go ahead and say okay and if we look at our drawing real quick we kind of have that part all created we'll come back and we'll do the chamfers near the end or whatever okay so the next thing is to kind of work on these little wings whatever you want to call them so i mean we can kind of see this is more of a top view we can see a 90 degree angle there's a radius in here these look like slots that are 44 millimeters wide tenon radius so let's just go ahead and do that now i'm going to create my sketch on this face right here and the reason for that is we're going to extrude up to this point and this it's going to kind of join everything together i don't really have a flat face right here i could create a plane at a point in a certain direction or whatever but because i already have the plane right there i'm just going to use this guy and say create sketch and now we put a piece of paper on that face and we'll go ahead and create a slot because that's kind of what the shape looks like so i'm just going to click a couple points i don't care what size right now and let's go ahead and just do something like that okay now i can come in and dimension this guy and you'll notice when you originally create the slot it's asking for a diameter but by doing this dimension i can do a radius or i can do a diameter so i have the option here and according to the drawing it's a radius so i'm going to do a radius of 10 like that um i'm gonna offset this guy oops not d offset let me uh hit o for offset chain selection is turned on so i'll go ahead and click that you'll see it's going to select all of the edges and i can offset the six millimeters according to the drawings let me kind of move this you can see it a little bit better so if i come in here we can see um there's the radius of 10 and then we can kind of see that this is a radius of 16 so obviously an offset of 6 in that case then what i'm going to do is define where this slot is located um so let's go ahead and you'll notice i haven't done the width or though i should say the length yet we'll come back to that here in just a little bit i'm going to create a circle let's look at the drawing real quick i'm going to create a circle that kind of defines you can see this radius 32 and it looks like it's going to be tangent with the the slot there so circle i'm just going to draw it out here in space i don't care what size i know it's a radius so when i dimension i'm going to change it to a radius and that is supposed to be a radius of 32. like so and i'll kind of move it sort of where it needs to be pretty close like that okay now i want it to be touching this object so i'll say tangent i'll say there and then you can see i can click on this line right here and you'll see that it makes it tangent right there and then i'll say i want it tangent from there to there and now you can see if i were to move this circle it's staying tangent along this edge here and it's staying tangent to the edge of the slot and because we haven't defined the size of the slot yet the slots actually growing and shrinking in size okay um i do know i need the arc to be a certain location so we can see in this drawing right here that it's 89 millimeters from the front of the part and 32 millimeters up from the right side of the part so let's go ahead and dimension this so i'm going to throw a dimension from here now you'll notice it's not letting me pick this edge right here and that is because we haven't projected any geometry and this is a curved edge if we were to rotate it you can kind of see sure enough that's a curved edge so there really isn't an edge there for us to pick so before i can throw the dimension on there i'm going to do p for project and instead of doing just specified entities i'm going to do the whole body because really i kind of want like a silhouette of this whole thing and you'll notice the different results notice when i do the specified entities it doesn't really highlight this edge but when i click on bodies and i hover over you can kind of see that edge appear so it's almost like a silhouette projection so you will get different results depending on what you click and sure enough i can now see that edge there which should let me dimension this direction we want that to be 89 and uh i think that's all i need to do um and yeah radius 32 which we did yeah i'm just checking my notes making sure i do everything okay we did the tangencies okay so the next thing i want to do is we're gonna end up mirroring this thing um so let me let me throw a dimension on the uh the width of the slot um actually you know what let's do that later let's just go ahead and do the mirror here so what i want to do is i want to mirror it halfway across and so i need a line a mirror line that i can use so i'm just going to click on my line command now i want it to be a construction line so i'm just going to come over here and click construction and then you'll notice as i get near the center of that line it kind of snaps automatically and we can see that that's a construction line i'm going to come over here and it's going to snap to the midpoint there and we can see that we just created a construction line so you can toggle this on or off if you don't want it to be object line so i'm going to go ahead and toggle that off and now it'd be just a regular line if i toggle that on you can see it's going to be construction geometry cool little tip okay so i now have this line that goes across we can come in here and say we want to create a mirror and i want to mirror all of this information including this circle here so here's a little bit of a trick if i if i try and draw a box like this you'll notice for example it grabbed this object line right here and not a big deal probably won't matter in this case but sometimes you don't want it to select that okay but if i drew it down here and went like so you'll notice it didn't select that circle which i do want however if i come from instead of left to right i go from right to left you'll notice it's doing a different window this is called a crossing window so it's going to select anything inside the window and anything that was being crossed by the window and you'll notice that it gets all that geometry including this circle but it did not grab that extra little line right there so again quick review if i do from left to right it's going to grab extra geometry that i really don't want in this case but if i go right to left it's going to do a crossing window and it's going to select everything inside of it and anything that that window was crossing now i can specify this construction line as my mirror line so i'll click on that and we can sure enough see that that's going to mirror across to the other side and let's take a look at the drawing real quick um so this was 44 so i'm going to come in and dimension that so let me just throw a dimension on this line right here we'll say make that 44 and you'll notice because it's mirrored this updated also that's kind of why i waited until after we mirrored just so you can kind of see whatever you change on one side changes on the mirrored side also okay moving on here we're kind of getting the overall shape the last thing i want to do is to create this shape here and i can see that it's 90 degree lines they look like they're tangent to the slots and then there's a radius 16 right there so let's um jump back in here i'm going to use this cool little trick where if i just get near the edge and i click and hold you'll see it's going to create a tangent constraint for me automatically so i'm just going to get sort of close to where i need to go right there and then all i have to do is get near this edge and move along it until i see that tangent icon appear you can see right there i'll go ahead and click and it created the the tangent constraint for me automatically now i want this to be perpendicular with each other so i'll come in here and do a perpendicular constraint that line and that line and you'll see it kind of changed a little bit and then i want this point to be in line with the center of the part so i'll say horizontal vertical that guy there with that guy there and you can see that it brought it down now how come these are still blue well if i grab this line you can see i can move these um slots tangently up and down along that circle okay so the last thing we need to do here is take a look at the drawing and we can see that these slots are 120 millimeters apart so i'm just using that dimension so i'll throw a dimension from that edge there to that edge there i'll go ahead and place it and tell it i want it to be um 120 millimeters and you'll notice that these turn black which means they're constrained now you'll notice these stayed blue this is actually an issue i turned into the development team even though it's fully constrained and you can't change it so if you end up getting these blue lines we think it has something to do with the the tangent we're not 100 sure but it is fully constrained you can't change these or anything like that so just just fyi if you're going through this don't stress over those lines not fully constraining okay so i pretty much have everything i need i'm going to finish my sketch again i don't really need to trim anything i'm just going to grab the regions that i want which are these regions right here rotate it so we're kind of looking at it from the top a little bit i'll right click and say extrude and i'll start to extrude you can kind of see what this is going to do now how far do i need to go well i'm going to change the distance i'm going to say to object and all i have to do is get near this corner right here i'm just going to go ahead and click and you're going to see it's going to extrude up to that point to that object i'll say okay and it joined when i did that extrude in fact let me edit it again you'll notice it says join and so it's going to extrude and because it's touching this vertical part it's going to join them together if i just said new body it would have created a totally separate body for example so now they're joined together you might also notice that in the drawing there's a radius back here and i could have drawn that in the sketch but i'd much rather keep my sketch simple come in here and say okay let's add the 16 millimeter fillet as an actual fill it feature like so that way i can come back and change it if i need to so we've got the the basics of the part done the only last thing is to do these little grooves that you kind of see here um and again i'm just kind of looking at the drawing i can see that they're five millimeters deep and they're spaced you know 68 millimeters apart from each other okay so i'm going to create a sketch on this top face right here i'm just going to draw a rectangle again i don't really care about what size i'm just kind of doing something like so we're going to use this to machine a little bit away however i need the spacing to be correct so i'm going to do a dimension from this edge to the let's just do the origin because that's right in the center i'll place it over here and again i'm going to use that math well it's 68 total and i want to go half of that so i'm going to say divided by 2 and you'll see that it will actually yeah that was pretty darn close let me undo let's do this i'm gonna bring this way down like so so you can really kind of see what's happening here so let me do that dimension one more time real quick so i'm gonna say 68 divided by two and you'll see that that rectangle kind of moves up and now this line is exactly half of 68 from the origin i don't really care about the the size of this rectangle i don't care that it's not fully constrained or anything like that i could you know dimension it if i want to but in this case i'm just using it as a reference i also could just select this as my profile but in reality i like to select the whole thing okay and the reason for that is you know what if there's a slight draft to these edges or this slot or whatever and if i only do this it could create little sliver faces or whatever so i like to select all of the profile almost like a cutter is going to be going back and forth you know removing this material i almost think about how is this going to be machined for example so we're going to extrude down in the negative direction so we'll say -5 we want it to cut sure enough we can see what that looks like okay and there we go because we created this symmetrically our origin is right in the middle of the part you can kind of see that right here as i rotate around you can see that right there so i have a mirror plane that i can use so i could come in here and say let's mirror [Music] what do i want to mirror i want to mirror the extrude feature what's my mirror plane i'll go ahead and click on this this front plane you see right there i'll say okay we just mirrored that extrude feature again i kept my sketch simple it's just one little rectangle i could have done it over here and added more dimensions or whatever but i was able to use the mirror command and mirror it okay so the the last thing i want to do here is um according to the drawings look at some of the chamfers so we can see that we've got you know one millimeter chamfers and then we also have i think it's in the notes one and a half by 45 so i'm going to go ahead and click on this edge and say chamfer and you'll notice that it selects a bunch of lines because of this tangent chain so i'm going to go ahead and select some other lines here and you can see that i'm only having to click like one edge and it's selecting a bunch of edges all at the same time so that tangent chain is really useful so i'll go ahead and do that i'll grab this edge and this edge but there's a couple edges that aren't chamfered like this one here and this one here so we'll leave that alone and let's just type in one and you'll see that it's going to chamfer all of those edges for me at the same time going all the way around pretty cool i could also come in and add a new selection set i'll go ahead and click on that edge there that edge there that edge there and then i want to chamfer this edge and the one behind it so i'm going to just grab the face and it's going to grab all of the edges that have to do with that face and let's just do 1.5 and you can see that it's going to chamfer those 1.5 and it's going to leave the other ones one and it's doing all of my chamfers in one feature in the timeline so that's fairly new we just recently added this where it's very similar to the philip command where you can add selections into here and have them to be different sizes you could even have them be different types whether it's an equal distance or if it's a you know two distance distance angle etc pretty cool so that's it that's how i went about creating this model so hopefully that gives you some tips and tricks on how you would approach something that's like man where would you start break it down into its simplest forms um sometimes it's as simple as rectangles and circles and then you start you know cutting machining away etc so another one that came through the facebook group was how would you create this part now this looks really simple i mean it's just it's a rectangle with an angled slot and this one actually caused a lot of commotion on the facebook group they're like oh you could create surface lofts and do you know this and that and all this kind of stuff and i'm like man it can't be that complicated and in reality it wasn't as simple as i expected it to be so i'm going to show you how i came about creating this model and i'd be curious if if any of you have other methods you know throw them in the chat window or try it out maybe share it on the facebook group or something like that so basically the important thing is this one dimension right here this 1-5 16. that is where this hole is located on this edge in fact i actually grabbed this um bring my book up here this actually came out of my old drafting book you can see there's the the part right there with the dimensions and everything like that so you can kind of see that 1 5 16. so we're going to make it exact i also picked this one because it has um you know dimensions like 5 16 and 1 16 and 5 8 and stuff so we're gonna do a cool trick with this let me bring up my drawing here so okay so like i said that location of that hole is very important to me and that's the key thing so we're gonna start a new design i'm gonna create a new component we'll call it angle block angle block okay i'll expand this open i'm just going to create a sketch on the front plane doing a rectangle now i like to again keep things symmetric so i'm going to do a center rectangle and that way everything kind of comes from the middle it needs to be one inch tall and it needs to be 4 and 1 16 wide but you'll notice i'm in decimal right now 5.63 well check this out i can type in 4 space 116. and it's going to figure that out for me automatically so you can do you know formulas you can do fractions you could even come in here and say you know 4 and 1 16. plus um you know let's just say 25 millimeters or something like that and it's going to figure that out and if i edit that dimension it actually remembers those values in there it's pretty cool didn't even have to change my units so okay so we set it back to four and one sixteenth say okay another tip i've shown before i could say finish sketch or i can just click on my profile right mouse click and i can extrude right from here and i don't even have to hit the finish sketch i'm going to keep it symmetric like i said i like to kind of keep things symmetric now this is 2 and 9 16. so i'm going to say 2 9 16. for the whole length and there we go okay now i need to locate where that hole is going to be so i'm going to put a sketch on this front face we'll create a sketch i'm just going to draw a construction line from top to the bottom making sure it's vertical like so okay then i'm going to dimension it and this is the important dimension i keep talking about so this needs to be 1 and 5 16 over from the edge and you're going to see it's going to push that line over so this point is 1 and 5 16 from the edge of the part now i created this construction line to be able to define another plane in a certain direction and to do that we're going to say construct plane at an angle and you'll notice it says line so for example i could click this edge here and it's going to let me put a plane along that edge at any specific angle or i could come in here playing at an angle what's my line well this construction line excuse me is my line so i can go ahead and rotate and you can see how it's going to rotate around that construction line well we need it to be at 30 degrees according to the drawing i'll go ahead and say ok and i now have a construction plane at a very specific angle at a very specific point so now i can come in here and create a sketch on that plane notice my view cube i'm not looking straight at the front or at the left or whatever we're looking straight at that piece of paper like so i can create my circle now you'll notice it doesn't seem to be snapping to that point be very aware so if i were to click right here am i at the correct location the answer is no i want to make sure i'm actually snapping right to that point so i might have to do p for project we'll go ahead and project the body now you can see that point is kind of highlighting right there so if i do a circle so that didn't do it okay so let me go p for project let's project that edge instead of the body now if i do my circle sure enough we can see that it's snapping to that edge so again make sure that you're getting the result that you want okay so i'm going to create a circle at this point um it needs to be 5 8 in diameter so five slash eight we can see that that worked correctly and then i need to do another circle this one's a radius so i don't know what size i'm going to do a dimension a radius and you'll notice that my dimension let me go ahead and say 0.75 you'll notice that my dimension is vertical in this example here and this kind of threw me for a loop and i learned something new i want to share with you it's really hard to see but you'll notice there's a green line right here and there's a red line right here and and angelo's shown this in the cam workspace you'll notice that there's a green line on the view cube a red line so that basically tells you uh which direction is the x direction which is this way and this is the y direction and so the text by default always tries to go along the x direction so that's why it's going in this direction here so again don't let that worry you it's just doing what it knows to do is to go in the x direction okay so i got those where i want i'm going to say finish sketch i can now see the the part i'm going to click on my profile here and again i'm going to i'm going to grab everything here so i'm going to say profile let's grab that profile and let's go ahead and grab this profile just in case um there's multiple profiles because we were slice you know we were cutting it in half with this projection line right there okay now here's where it's gonna get kind of weird this is kind of what threw me for a loop i'm gonna go ahead and say extrude and we'll start extruding in that direction and i can already see i missed something i don't want it to cut i want it to join okay cool it's taking that profile and you can kind of see it's extruding it well i want it to go flush with this face so instead of a distance i'm going to say to object and i'll click on that face and i get the result that i want you can see it's taking that profile and it's extruding it at the correct angle to that face but notice what's happening here at the front okay i don't want all this extra stuff hanging off the front and unfortunately two object only goes in one direction now if i came in here and said two sides that lets me extrude like so and if i say to object you'll notice it doesn't let me click this front face which is really weird it lets me click points so i'm going to click on that point and you can see it's extruding to that point so unfortunately we can only do the two object in one direction so how do i fix this well what i ended up doing was saying instead of starting at the profile let's offset let's just offset maybe an inch so what's cool about this if you kind of think forward here where this is is exactly still in line with this point and that's the important thing here right so i'm just going to offset my plane 1 inch we're going to join that together i'll say ok then i can come in here and say extrude one side how far to object click on that face and we can see that sure enough it's still in the correct location we'll join that together we'll say okay let's turn our sketches back on so we can see that hole and you can kind of see what we did here so we kind of had to do it in two steps but we now have this angle exactly where it needs to be all we have left now is the uh um oops let me do that just sorry we select the profile here and that profile there we're going to extrude i like to start to extrude to kind of see what that looks like i'm going to say instead of distance i'm going to say extrude all and it's going to go all the way through the part in one direction okay just like we ran into previously it only goes in one direction and you'll notice that there's like this weird little sliver going on here so there's two different solutions you could do here i could change it from one side to two sides and then just bring this out a certain distance again i can't say all it throws an error it doesn't like that for whatever reason okay i can't say to object it doesn't let me pick that front face so i could do a distance like so or i could leave it one side and i could say okay then i could just come in here and click that face and hit the delete key on my keyboard and fusion is going to heal that geometry and you can see it did add a delete feature into my timeline and i kind of like this solution better because if i were to come and change like the width of this block no matter what that face always has to delete whereas if i had changed the extrude and did the two sides for example and i only came you know just far enough for whatever but then we made the part bigger this distance is gonna stay right here and that weird sliver is gonna show up again so that's kind of why i like the delete face okay i'm not going to finish the the whole drawing here it's pretty simple um you know create two little rectangles and machine those through um same thing with like the holes i'll go ahead and do the holes we can kind of see where those are located at so i'll just show some tips and tricks with that so i'm just going to click on a face and say hole and i can position it where i want well right here you'll notice it says reference and you can even see as i kind of hover over on these edges so i'm going to click on that edge and the hole needs to be um 9 16 so i'm going to type in 9 16. you can see it kind of jump over i'll go ahead and click on that one there and it needs to be um 1 in 9 30 seconds you can see it kind of jump down there then i can come in and specify you know what kind what size hole it is so it's a half inch hole i want it to go all the way through so you can kind of see just by changing it to all it goes all the way through i'll say okay and again because i did this symmetrically oops i could come in here and say mirror what feature the whole feature what's my mirror plane that mirror plane right there i'll say okay and again if i were to change the width of or say the length of this block that hole is always going to stay in the correct location and that one's always going to be mirrored symmetrically around it so that's one of the reasons i like to do things symmetrically um let's just since we we have a couple minutes i'll go ahead and create a sketch here i'll throw a rectangle on here and another rectangle over here i could do that or i could just throw a dimension on this guy and he's supposed to be three eighths so i'm going to say three slash eight this one is supposed to be five eights so i'll say 5 8 i can click on this and say extrude now here's another tip i'm going to say go through all and you'll notice nothing happened but notice the direction the arrow is pointing well right here it says flip so i'm going to hit flip and now it's going in the correct direction so if you change it to all and you see nothing happen just go ahead and hit this little flip icon we'll say okay i could mirror that guy so i could say mirror what's the feature the extrude feature what's my mirror plane that front plane i'll say okay and we get that result i could have drawn two rectangles and dimension them i mean there's many different ways that you could create this model i like to use the mirror because if i end up changing the size of the model down the road everything is going to kind of update accordingly which is kind of cool okay so that's that guy um we have a couple minutes let me bring up a couple more this one i saw on the facebook group and i thought it was a really valid question he had modeled a box that looked kind of like this um i'm assuming you know maybe it you know hooks onto a belt and holds a cell phone or a tool battery or something like that and after he printed it he wished that these um arms were kind of at an angle a little bit instead of being straight out now you know you could go back and edit the sketch potentially but let's pretend that it wasn't modeled very good or maybe it was imported from another cad system there was no sketch or timeline to edit okay in fact let's force that i'm going to do not capture design history we now have a model that has no information but what i can do is come in here and say move now i don't want to move bodies i want to move faces now let me show you what typically would happen here people are like okay i want to move these faces so they're going to draw a selection box around those faces but notice where the rotate is well i kind of want to rotate it more like over here like along this blend for example or that fill it so right here it says set pivot so i'm going to click on set pivot and then i might pick maybe like this top edge or this bottom edge right here it really doesn't matter in this case um and you'll notice it's kind of like snapping to the midpoint endpoints again that doesn't really matter i'm just clicking a point and you have to come back here and say done so i'm going to say done now watch what happens when i rotate the front of the box rotates also and this is not what you would expect this is not not what you're hoping for now we're able to rotate the arms but i don't want the front to rotate why is the front rotating well fusion's trying to keep everything tangent and i i selected this front fillet you know when i drew my selection box it grabbed that okay so let's try it a little bit differently let's right click and do the move command and i'm going to let's just try maybe doing something like this drawing a selection box oops make sure you're on faces i'm just going to draw a selection box like so you'll notice what it's selected let's set my pivot again i'll pick that exact same pivot point let's grab that arrow and notice the result i get now okay because i didn't select these front fillets it's moving those faces it's keeping those faces tangent all that kind of stuff but now i can come in here and say you know go minus 15 degrees up to 15 is too many let's just do uh 10 degrees or something like that seven degrees oops and say okay and we've now modified this model that can you know clip on be a little bit better so hopefully um that helps you out again if you get a weird result try selecting less faces okay instead of doing a selection box like that do a selection box more like this for example or i might even try i haven't tried this let's try doing faces let's do the right to left and just do something like this you can see all the faces that it's selected i'm curious if this is going to work let me uh this is live so we'll see yep so that worked also that might even be the best solution there is to just do a crossing and saying i only want really these faces here to move i don't want any of these vertical faces or phillip faces to move so that left i'm sorry right to left crossing selection is pretty cool trick okay the last one this was actually kind of a cool one um have a customer he designs speaker boxes and he was asking and he needs to create very realistic renderings so um you know i was showing you could just do a very simple shape and add a material a cut through material and it'll simulate what this looks like but he actually wants all the little shadows inside these holes and stuff like that so how would i go about creating something like this that actually rolls around you know is on a curved surface rolls around another surface and continues on that direction well the trick here is to use sheet metal so i'm going to back up here and i'm just going to step through so i created a sketch let me turn this guy on very simple sketch that kind of defined the top view of my speaker grill okay then i used sheet metal in here to create a flange using that profile so it's the correct thickness etcetera okay then i unfolded it so modify unfold i was able to pick one of those flat faces and it unfolds it flat created another sketch on that face drew a you know created a hole then i patterned that hole and you can see it goes all the way across then i created another kind of offset hole like so patterned that to kind of get the the triangular shape there you can kind of see where i'm going with this then i patterned those two patterns up in that direction and then finally refold the faces now again this is pretty complex geometry so you saw it took you know a few seconds for it to uh um to do that okay so anyways that is how you would go about doing something like this the sheet metal tool is a really kind of cool tool to do odd shapes like this so okay with that i hope you learned um some tips and tricks on how would you approach you know complex models something that you know missing dimensions or where do i start how do i create that angled hole but i know it has to be a certain distance and you just kind of have to think um a little bit outside the box kind of like what i did with that angled hole you know we had to extrude two different directions but i was able to to make sure that that hole was in the correct location using the sketch um tune in next week uh hopefully angela will be doing a uh cam series so uh oh i haven't asked him yet so i don't mean to put them on the spot but hopefully we'll do a cam series um i'm also coming up with a new um series kind of like what we did with the pencil sharpener it's going to be a multi-part series on how to model more of a sheet metal type design so you'll see that coming up soon give us a thumbs up if you like this if you have any other ideas or topics you'd like to see throw them in the the youtube comments after this has been published we always read those and and thank you for attending and have fun fusioning you

Channel: Autodesk Fusion 360

Views: 39,223

Keywords: fusion 360, autodesk, design, engineering, mechanical design, mechanical engineering, industrial design, product design, software, CAD, CAD software, Computer Aided Design, Modeling, Rendering, 3D software, Autodesk fusion 360, cloud based CAD, CAD in the cloud, cloud, Free CAD, Free CAD Software, Autodesk CAD, cloud manufacturing, free CAD program, 3D CAD solution

Id: Z6XPqjJRtaY

Length: 66min 23sec (3983 seconds)

Published: Thu Jan 07 2021