360 LIVE: How would you model that

to [Music] [Music] [Music] [Music] [Music] [Music] [Music] [Music] [Music] [Music] [Music] hello everyone and welcome to another fusion 360 live my name is brad talas as you can tell by my background i'm still traveling right now working remotely so i'm in coeur d'alene idaho right now on my way to montana so again hopefully this live stream goes smoothly with the internet so today i'm going to be talking about how would you model something like this now it doesn't look overly complex but if we look at it from the front we can see that you know it's got a curved surface on the top and the bottom it's got you know some pockets in here etc so how would you go about approaching this to model something like this with this curved surface and i've noticed even i posted this out onto the facebook forums and people have already responded how they would go about modeling it um so so whoops my method is not the correct method it's not the only way of doing it it's just one way of modeling this so it'd be really interesting to see how everybody else approaches something like this we're also thinking about having angelo take this model and then show how would you machine this so how would you do these pockets and the curved surfaces and the chamfered edges and all that kind of stuff so keep an eye out for an upcoming live stream on that okay um angelo is helping me out on this live stream he's answering the chat questions so if you have any questions please feel free to post them out there and he'll try and get those to me i'm on limited monitors so i can't really see the chat very well so i might have to wait near the end to answer some of these questions but so this is the drawing that i created that i'm going to go off of so i'm going to be referencing this drawing quite a bit i've also included the outline and the drawing in the description of this youtube video so please feel free to download those and follow along to the video later on or try it yourself once this this youtube video is over so i'm going to go ahead and dive right in and again this is kind of how i approached it i'm not saying this is the exact correct way first thing i'm going to do is change my units into millimeters because we are doing metric for this and because the part is pretty symmetric i'm actually only going to draw part of the part in fact i'm going to draw basically a quarter of the part and half of the part and you'll see that as we go along so i'm going to create my sketch on my top plane because most of the information to me is kind of being displayed in this you know this top representation okay so the very first thing in the drawing is it asks for a 30 millimeter radius dimension and you'll notice by default we do diameter dimensions so how do i get a radius dimension well all i have to do is click to create the circle i didn't type in anything and then i'm going to do a dimension and i can also use the d key d for dimension is my shortcut key so i'll go ahead and select this and again you'll notice it's showing me a diameter but if i right mouse click now you can see i can change it from a diameter to a radius and now it's asking for a radius number we'll type in 30 and we'll hit ok and i now have a 30 millimeter radius circle the next thing i want to do is to create a centered rectangle but it's actually not centered to the origin um in fact it's kind of hard to see but you'll see here so this rectangle is 100 millimeters tall but you'll notice that it's you know offset by you know 55 millimeters here so it's actually sitting a little bit higher you'll notice there's more room up here than there is down here so how do i go about doing that well i'll go ahead and go into my rectangle center rectangle and i'm just going to kind of draw it out here in space somewhere i'm not getting near the origin but i can type in it's 200 millimeters wide by 100 millimeters tall okay then i can kind of move this around you'll notice it's not fully constrained what i want to do now is line it up with this origin right here so i'm going to do a horizontal vertical constraint and i showed this tip last time you'll notice it's not catching to the midpoint here it's it's looking for a point and there is no point along here but i want to catch to the midpoint so i'm going to hold down my shift key and now you can see it's catching to that midpoint of this line so i'm going to click there click there and it's now lined up or made the center or the midpoint of this line vertical with my origin okay now i can throw that dimension on here so i'll say from there to there we'll make that to 55 and sure enough you can see it put it in the correct location the lines turn from blue to black that means they're fully constrained and we're going to be kind of focusing on that quite a bit to make sure that we have a fully constrained sketch as we're going through okay what i'm going to start doing now is start to kind of build these arms and these are kind of interesting um you'll notice they're like 60 degrees like this but like this is more sloped than this one is over here this is 50 degrees here a radius of 15. so i'm going to kind of start building these arms right here so let's start out with that 15 millimeter radius so again i'm just going to kind of start to draw off to the side and it's asking for a radius so i'm just going to click somewhere create my radius dimension and type in 15. then i will make sure that that's lined up using constraints like so okay now let me i'm going to back up half a second here you might ask well couldn't you just hover over this point right here and you'll see this cyan line kind of appear and now i know i'm perfectly lined up with that center point and i could create my circle well here's the deal that was just a snap guide so it is not constrained at all to that point that's only a guide okay so that's why i tend to draw things off to the side then i come in and i say i want that to be [Music] vertical with that that center point that origin point and now you'll notice the only thing it can do is move up and down it can't move to the left or to the right but i can control this using a dimension so i'll go ahead and place my 60 millimeter dimension so i'll type in 60 and we can see that sure enough it turned black and that is constrained now to draw these little i call them arms or fingers whatever you want to do i'm going to just kind of rough them out and then control them with dimensions so i obviously want to do a tangent line because it's going to kind of come off this circle in this direction so i'm just going to click and hold and you'll notice by holding down my left mouse button it's doing this automatic tangent for me so i'm just going to click there and maybe something like that and then i'll do the same thing on this side i'm going to click and hold you can see i got the tangent and i'll just come over here somewhere so i quickly kind of mocked up what that's going to look like then we're going to control it with the dimensions from the drawing and again i'm not going to flip back and forth too many times on the drawing but just know that i'm referencing the drawing to to get these measurements and stuff so let's do a dimension i'm going to go ahead and control these we know those need to be 60 so i'm going to type in 60 i'll do the same thing over here now i could type in 60 or i can click on an existing dimension and it's going to reference that dimension and the reason this is handy is because if i came back and said make that 65 that's going to turn to be 65 also and i don't have to type it in twice or make a mistake you know typing in 61 instead of 60 or something like that okay so now we know those triangles are 60 degrees then i'm going to go ahead and control we know that it's 50 degrees between these two guys so i'll go ahead and place that one and say 50. but you'll notice like this one's leaning a little bit more than this one is over here this one's a little bit higher than this one is over here but this is kind of i think this is the fun part where you kind of see your sketch start to get built and controlled correctly so what i'm going to do is this is 50 degrees between these two angled lines well i need to basically create half of this so if if we knew that this was 25 because 25 is half of 50 it would then line these guys up well i need a line to do that so i'm going to create a line i'm going to change it to a construction line just by clicking on this little construction icon and i'm just going to draw that straight down like so i now have a construction line and because i started at the origin you can see it automatically created those coincident constraints for me so this line is tied i'm trying to drag it right now and i physically can't so it's tied to that origin so check this out this is actually kind of cool i'm going to now come in and say let's put a dimension from this line to this line here and i'm going to go ahead and place that well i could type in 25 but what if we end up changing this angle i then have to go in and change that angle so instead i'm going to reference that 50. so i clicked on the 50 and you can see it put that that dimension value in there well i want it to be 50 divided by 2. and notice what happens let me kind of move this down a little bit it now says 25 and you can see that those two blue lines became constrained and we can see that they look nice and even now we obviously know this is 25 so that has to be 25 and again because we're referencing this if we were to change this to 60 that would have to be 30. so and try not to type in the numbers as much as referencing existing ones that way if you come in and change them they'll update accordingly hopefully you guys knew about that tip okay let's go ahead um now i i tell you all the time i like to fill it in 3d but this is kind of a i would say this is kind of a major part of my sketch so i'm going to go ahead and do the fillet in 2d so i'll come in and say fill it i'll click on this point it's supposed to be 10 millimeters so it remembered that and i'm going to go ahead before i hit enter i'm going to go ahead and click on this point also that way it'll do both at the same time and i'll hit enter now you'll notice i can move these around if i need to i'll leave that one kind of up there a little bit now i want to make these lined up so let's go ahead and control one of these again kind of using the the drawing here i can see that this circle which happens to be or the center point happens to be the radius there is 141 from the top edge so i'll just throw a dimension from here to here to that point and i'll say 141 and we're starting to see all of this is becoming fully constrained well now i want this other finger to be perfectly lined up with that so let's go ahead and do a horizontal constraint i want that point to be the same as this point right here so you can see by using the horizontal constraint it went ahead and did that i notice there's a lot of road noise around me hopefully that's not coming through on the microphone hopefully you guys are able to hear me okay and learn everything let me look at the questions really quick um okay it doesn't look like we got any questions so let me continue on here okay so looking at my sketch there's a lot of my drawing i should say there's a lot of stuff going on and you hear me all the time where i talk about keep your sketches simple um and i highly recommend doing that because the more complex your sketch gets the more confusing it kind of gets so i'm actually going to reuse this sketch a couple times but then you're going to see we're going to say okay we're at a good stopping point let's create a new sketch and then finally let's create a third sketch for example so i'm going to keep this sketch pretty simple i'm not going to do any of these pockets or holes or anything like that i'm really all i'm concerned about right now is kind of the main shape okay so we can see that the overall thickness of this object is 24. we can also see that it's pretty symmetric so i'm actually going to do half of the model we're only going to create the top half of this model and then we'll mirror it near the end to move everything to the bottom side so i'm going to go half of 24 so 12. so i'll finish my sketch i'll go ahead and select my profiles that i want extrude and i'm going to go ahead and say 12 instead of the 24. also notice i'm extruding up so my sketch is kind of on this bottom plane and there's kind of our basic shape now i'm going to continue on here let's fill it these edges here so again using information from the drawing i'm just going to fill it these vertical edges might rotate so i can see that one a little bit better 10 millimeters we're good to go there and now i want to start working on some of these pockets and stuff like that here's my original sketch i'm going to kind of keep that as my original almost like my skeleton sketch and then my next sketch i'm going to do just for example the pockets so i'm going to click on this top face create a sketch and then i want to grab the information so we're going to project so create project project or as you see me always do i always use the p key p for project but i want to project the whole body in fact i mean it wouldn't matter in this case because there's not much going on i could do the specified entities but i'm going to do bodies pretty much the whole time so i'm going to switch to bodies right now and it's going to project that whole body onto our sketch including for example the center points of these fillets and now you kind of know why i did the fill it before i did this sketch if i had kept these square i wouldn't have something to reference right there for example okay so let's do some again referencing this drawing here here i'm going to create this radius 40 circle that goes all the way around like so and we're going to start creating these pockets again going to keep it simple so we're not going to do these rounded edges until later but i can see they're 15. here's a construction line that goes to the corner there so i'm probably going to do that and then an eight millimeter gap there okay so let's let's kind of build that so circle construction circle because i'm just going to kind of reference the circle again it's a radius so i'm just going to go ahead and click dimension this guy and say radius of 40 and it'll update and then i'll do my line i'm still in my construction so i can go ahead and draw a line to that point there i'm going to go ahead and do a vertical line because i'm probably going to end up mirroring some of these pockets so once i create this i'm probably going to mirror it over there in fact let's go ahead and do another construction line like so okay let's offset these this angled line right here so remember it was a spacing of eight so i'm going to type in four and it's going to offset four i'll repeat that command i'll go ahead and offset that guy i'm going to start to drag in that direction and i can see it's a minus so i'm going to say -4 and now we have those lines there i'm going to offset this line here but notice it's trying to do the whole thing all i care about is the line so i'm going to turn off chain start to drag and say minus 15. okay then i'll go ahead and do the um come on sorry let me do that again offset minus 15 enter i must not hit enter i'll do the offset here this is 71.5 again according to the drawing right here 71.5 to kind of define the edge of this pocket so we just created some construction lines that will help us out we have this curved surface here we have this 15 and now you can kind of see we're getting a particular shape here so i'm going to trace over this so i'm going to click on the line command and make sure my construction is now turned off so i'll go from here to here and from there to here however i can't use the line command to do this so i'm going to show you a neat little trick here in just a second i'm going to continue doing that exact same thing so i'm going to trace from there to there and from there to there okay so what about this little segment because i don't have a valid profile well notice this is one solid circle goes all the way around under the modify command there is a command in here called break and watch what happens when i hover over this segment it's kind of hard to see but there's little red x's that are appearing right here in the corner here and up there so by clicking on this segment i just broke that segment out of the full size circle so let me do that again i'll come in here and say break i'm going to click on this segment it goes to the next boundary so that's why you see that x there and the x down there so i'm going to go ahead and break that then i can come in and see that that's its own little segment well i don't want it to be construction i want it to be an object line same thing with this guy i can click on it and say change it from a construction to an object line and we now have a valid profile right there we don't have one here because it's not closed but i'm going to go ahead and show you a cool trick here we're going to mirror this because this is basically the same down here so let's just use the mirror command i'm just going to draw a box around what i want to mirror what's my mirror line this line right here i'll go ahead and say okay and we can now see that we have a valid profile there there and there so i kept my sketch pretty simple and you can kind of see i started with this and then i mirrored this but look at all of these icons here could i have done this a little bit differently and the answer is yes i'm going to undo and instead of doing a mirror i'm just going to in fact i could break it let's go ahead and break this segment right there let's go ahead and convert that to that and now i'm done i am not going to mirror or anything like that in my sketch and notice how much cleaner this looks i'll go ahead and extrude these guys i'm going to start to push down so you can kind of see what's going to happen instead of typing a distance i'm going to say go through all that way i don't have to remember was it 12 was it 24 was it 13 i don't i don't care i just want it to go all the way through the object like so okay then i'm going to come in and fill up these guys so i'll say fill it these are five millimeters so i'm going to fill it just those two edges there and then watch what happens when i add in these other edges they start to create that curved pocket there so i didn't create the fillets in my sketch whoops sorry in my sketch um i kept them sharp and then i used the philip command to do it in 3d now why would i do that well if i want to come back and change the size of these from from 5 to 2 it's very fast and easy to do that i don't have to edit the sketch it's just right here as a feature okay now instead of mirroring the sketch could i mirror these pockets so let's go ahead and create mirror i do not want to mirror faces because then i'd have to come in and select every single face that would take a long time i don't want to mirror the body because this is all one body so i want to mirror features and it's asking which features do you want to mirror well i want to mirror the extrude and i want to mirror the fillets so i'm going to mirror both of those features what's my mirror plane we'll say that guy i'll say okay and i now have those pockets there so basically i created a quarter of it and then we mirrored it that way now i think you guys are probably clueing in what we're going to do next we're going to now mirror this to the other side so create mirror features okay well what features do i need to select well if i only selected this mirror feature notice my preview so this mirror feature is referencing that extrude and fill it so i need to actually come in here and say i want to do all three of these i want to do the extrude the fillet and the mirror we'll mirror that that direction we get a nice preview what that's going to look like i'll say okay and we now have those pockets on both sides now if i go back to my drawing some of you eagle-eyed people might be like well you forgot a pocket there are actually two pockets right here now i did this on purpose because this is this is exactly how i modeled the part i got along and i looked at my draw i'm like oh man i totally forgot to do those other little pockets down near the fingers what do i do and so i'm trying to recreate what would happen you know in the real world with all of you designers and and hobbyists and engineers and all that kind of stuff you're going to run into situations like this um i forgot to do something or i should have done it you know 20 steps ago etc so let's take a look at what we're going to do to resolve this so here is my sketch in my timeline this right here so i'm going to go ahead and edit that sketch but now you'll notice we don't see a lot of the 3d stuff going on because that's happened after we created this sketch that's okay so i want to start creating these pockets again i'm going to use information from the drawing so i'm going to offset this line here oops that line minus 16. i'll do the same thing for this line here minus 16 and then i'm just going to draw a line that kind of touches this line here it goes horizontal and touches that line there now why do i care about where it's touching well you can see it's actually creating coincident constraints so no matter what i do with this line you can see that it's always going to be touching the edge of those of those two lines there it's kind of cool so coincident constraint coincident constraint horizontal constraint but you'll notice that the line is blue it doesn't know where this line needs to be so according to the drawing it is five millimeters down from this edge so you can see that right here five millimeters down from that edge and it turned black now is this a valid sketch it is and i could leave it this way now some people are like well that looks dumb i want to trim my lines but watch what happens when i trim these lines you'll notice i get constraints and or dimensions were removed during this operation so sometimes when you go ahead and trim we lose some information so this is no longer constrained so how would i fix that well i could just throw a dimension back on here you'll notice it remembers it was 16 and i could do the same thing here i could even reference that guy if i wanted to and now again it's fully constrained so you have a couple options don't trim it or trim it and maybe you might have to rebuild a constraint or dimension okay so let's go ahead and finish our sketch here now you'll notice we kind of went away so i'm going to go ahead and turn that sketch back on so you can kind of see it there now here's the deal this also has to be over here so what i'm going to do i'm actually going to back up one step in my timeline so i'm going to go back one step so i'm before i did the mirror to the other side okay kind of went back in time a little bit i'll go ahead and do this extrude how far we'll say all so it goes all the way through that looks good i'm going to turn off the sketch so it's a little bit easier to see let's fill it these edges so i'm basically kind of working on this part of the design back in time before we did the mirror so hopefully you kind of see what we're going to what's going to happen here so i'm going to do radius of 4 for that edge a radius of 4 for that edge but it's a radius of 6 for this edge right here well they're all kind of related so i'm going to come in and add a selection set so i'm going to click on this little plus and i'll just go ahead and click on that vertical line and make it six and now you can see we're going to have one fillet feature in the timeline but it's going to do two different sized fillets in fact if i say okay there's my fill it feature i really like these selection sets because you know we're kind of working on the same area right here so instead of having three or four different fillet features i could have one with as many selections and sizes as i want okay so i've now created that little pocket and let's just take a look at the drawing and i'm like you know what there's a rectangular pocket in here also that's on the other side man i should have totally done this before i mirrored those pockets the you know these through pockets well that's okay let's come in here and create the pocket so let's go ahead and in this case i'm going to create a new sketch just to kind of simplify things i could go back and edit this sketch here but i've got a lot of stuff going on over here i don't really see the 3d representation of it so this is what i was talking about earlier where sometimes i'll have maybe two or three sketches now you saw that we went back and edited this sketch we added some extra stuff to it but here i'm just going to create another sketch and now i have a nice clean representation i'll go ahead and project the body because i want to grab information from the body and i'm just going to draw or mock up basically a quick little rectangle like that i don't care about the size or anything yet we're going to come in and dimension these so again according to the drawing it's four millimeters from the top it's 24 millimeters from the edge four millimeters etc so now i do care about the size so let's go ahead and do that i'll say we know that this is going to be 24 this is going to be 4 here and you can see how as we start to do this it's starting to constrain um the sketch for us oops make sure i'm in my dimension from there to there i want that to be ah sorry guys a vertical dimension four okay and then the last dimension here is four right here so basically it's four all the way around so i will throw a dimension from this edge to this edge and i should have and could have you know clicked on an existing dimension like so to reference that in fact let's go ahead and do that down here i'll throw a dimension from here to here and let's just reference that one and that way if we decide to you know change the size of this and make it six everything's gonna update around again a little tip there instead of having to type in you know six six and six to change that i only have to change one of them okay finish now this this is a little bit confusing hopefully i can explain this this is a section view that's cutting through the model and we can see that there's basically a web and it's this face you see right here and it is four millimeters thick so while the rest of this model is pretty thick right here it's only four millimeters thick now i drew my sketch on the top face and you'll notice i don't have a dimension that tells you from you know from this outside edge to here what that is we have no idea what it is and the drawing doesn't tell us so how would we solve this i like to throw these little curve balls in here so let me check the questions really quick before i dive into here um okay so all asked is there a way to print a sketch there is so if if you come into here you can right mouse click and you can see you could save this as a dxf so you could bring that up into a pdf drawing or whatever there's lots of viewers out there for dxf or if i just come in here and say file um share nope i guess there is not no i thought there was there's 3d print but usually under share like i could do capture image so for example let's just do this file capture image it'll let you capture this image and then you could print that so yeah that's oops that's a good question okay let me turn my body back on okay um another question for y'all are some constraints more expensive to compute like would using horizontal b um you know take more performance than using like symmetry so i that's this is a really good question so thank you for asking that ale i don't know if one is heavier than the other but i personally do not use symmetry that much one because it really complicates and clutters my sketch yes i know you can turn off your you know what's being displayed and all this kind of stuff but i like to keep my sketches simple and i would use a 3d mirror versus using like a symmetry in my sketch um so i don't know how to really answer that question like if if i referenced this four with a bunch of different dimensions i don't think that's any heavier than just saying this is four this is four this is four etc i just think this is faster and smoother to to make changes down the road so yeah that's a good question i i do not know the answer to that so i do know the more complex your sketch gets the longer it takes to calculate and that's one of the reasons i like to keep my sketches as simple as possible so okay so let's do this we're going to extrude this guy now what we're going to do is change the start to not be this profile so i'm going to change this basically what it's saying right now is when we do an extrude it's going to start at that profile plane where we where we drew this profile well i can come here and say offset or i can say from an object so i'm going to say from an object let's click this bottom face now watch what happens when i start to drag it is starting it's using this profile but it's starting from the bottom of the part and it's starting to extrude up well i don't want to start from the bottom we know that there's a four millimeter thickness there but now notice i have this offset so i'm going to type in minus two and we can visually see what's happening now it's starting and again you're probably asking why the minus two so it's starting here this is the positive direction so i told it to go in the negative direction two millimeters now how far do we need it to cut well we want it to go all the way through so it's using the profile from the top face starting at the bottom face offsetting two millimeters and then extruding all the way through the object kind of different but really powerful i didn't have to move my sketch to the other face or create another sketch or undo or anything like that i just used this start option [Music] and you might ask what's offset well remember my profiles here i could have said offset you know three millimeters down and then start to extrude so that's what that is object allowed me to pick a totally different object or a different face so cool little tip there hopefully you guys learned something there let's go ahead and fill it this pocket so i think these are radius six according to the drawing so there's that guy now if i were to come in and add a selection set i could but notice that these fillets go away so i have to manually select all four of these edges and i even have to rotate potentially or whatever but then i could come in and say okay that is a radius of two and it'll do all of them [Music] in one fill it feature okay or i could come in here and say this is a radius of six let's just do those four edges i'll say okay there's my fill up feature then i could come in and fill it and because of this tangent chain it's going to select all of those edges for me i can say 2 and i get the exact same result except for the fact that i now have two fillet features again totally up to you is one better than the other i don't know i mean i think the the simpler your timeline is the faster it'll calculate kind of going back to aeol's question so i would probably do a selection set but knowing that i'm going to have to probably manually select some edges so if this was a very complex model i'd probably do two or three fill it features and let the chain command really help me out but on something as simple as a rectangle i'm probably going to do it with just one fillet feature so i'd come back into here add in that and i just have to select those four edges now do i have to select those four edges check this out okay so there's my result i'm going to go ahead and get rid of that instead of the four edges i'm going to do a selection set i'm going to click this face and i'm going to say 2 millimeters and notice the result that i got by clicking the face it selected those four edges of that face automatically and not a lot of people know that you can do this so let me back up selection set i was manually clicking all four of these edges okay but instead i can just click on that face tell it i want that to be a two millimeter and it's going to select all those edges so if you liked that if you didn't know about that tip make sure you give us a thumbs up or thumbs down if you didn't like that tip we take all feedback okay so we're still back in time remember i already mirrored all this stuff over here but we're still working on this i'm going to look at my drawing really quick i can see that there's some holes that go through this pocket i'm going to go ahead and do those it looks like they are five diameter through holes so i'm going to click on this face and use the whole command i really like the whole command instead of using like a sketch and a profile or whatever it gives me a nice preview obviously way too big so the first thing i'm going to do is change my diameter to five okay that's looking a little bit better now where does it need to go well you'll notice there are no dimensions to these circles however there are center lines so we know that they're centered or concentric with the arcs or the other fillets so i'm going to start to drag this little blue dot and you can see two white dots that kind of appeared and that is the center of all of these edges these fillets here so i'm just going to get near that dot boom and it drops right onto it and it's perfectly where it needs to be i don't need it to be that long so i'm going to just say go through all it figures out what it needs to do diameter 5 looks good i'll say ok i'll repeat my last command hopefully maybe not oh yeah because i pre-selected so i'll just do the whole command i'll click there it remembers my five i'm just going to start to drag drop it right there it snaps right to it and we'll say go through all and there we go those two holes are exactly where they need to be and i didn't have to create a sketch or anything and there are features in the timeline so i could go back and edit those very easily okay now i pretty much have everything i oops i need except for these holes here we're going to come back to those later but i have this pocket i've got this pocket okay so let's advance forward in time and just these pockets mirrored over nothing else did well why not well because when we created this mirror we only told it to select certain things out of our timeline so i'm going to edit this mirror feature and you can see right here features three selected we only mirrored the extrude the fillet and the mirror well i can come in and say well now i want to grab the um this extrude here that fill it there so now it's going to mirror that pocket you can see the preview but i also want to do maybe that pocket the fillet and the two holes and notice the preview i'll go ahead and say okay and just like that we didn't have to create multiple mirror features we were able to kind of go back in time and put all of these where we wanted them and then add them to the existing mirror feature i think that's pretty cool you can do that okay let me look at questions really quick see if there's any new ones okay it doesn't look like it so um okay so now obviously i want to create these whoops counter board holes we can see it's a diameter 10 diameter of 14 and i think i left out i did the depth of the counterbore i apologize guys we'll make it up so i'm going to use the whole command and just like before if i drag on this face we can see there is a point at the center of this curve so i'm just going to snap right there we will build this the right way so i'm going to say counter bore i like to do the the larger diameter first now i'm probably going to get an error um yeah well maybe not okay it's smart enough um the counterbore diameter is going to be 14 and then the counterboard depth is going to be six okay now i want it to go all the way through so there is a depth there so i want to basically go all the way through and you can see we get that result there say okay and there's our counter board hole and i'll do the exact same thing over here it's going to remember all of my last settings so all i have to do is drag it into place now i could have done this before the mirror feature etc etc i could have but i didn't want to beat a dead horse doing things over and over again so it's totally again up to you if you wanted to do that before the mirror and then mirror that whole feature it would have appeared there i feel more comfortable knowing that that's going exactly at the center of that curve okay so pretty quickly we've created this whole part now all that's left is to create this curved surface and you'll notice i just did a flat extrude i didn't do anything to make this a curved surface i'm going to basically create a curve according to these dimensions here and use that to split the body and that's how i came about doing this so i'm going to go ahead and create a new sketch and let's just do it on this front plane we'll project the whole body we'll say okay you can see it projected that whole body and then i want to create a line construction line and i'm just going to click somewhere like up here for example and maybe over here making sure that that's horizontal and the reason i'm doing that is because we can see here that the overall thickness of this curve is 12. so i'm going to dimension that to be six millimeters up because we're basically slicing this in half so half of 12 is six so let's go ahead and throw a dimension on here from here to there let's just make that six i could even have measured this line and said this distance has to be half of what that measurement is that way if we were to ever change the thickness of the part again think about all the functionality you can do here okay so now i'm going to do an arc and let's do a center point oh let's do a three-point arc so i'm going to start at this point here i'm going to catch to there then i'm going to catch to this point here and i usually move to kind of see what's going on i can see uh-oh i'm in construction so let's go ahead and turn that guy off and then you can see i can snap right there so i'm going to go ahead and click but this line is still blue well why is that well if i grab on it i can see that i can still move it so this is one of those examples where i like to over exaggerate or under exaggerate and physically see that my constraint is actually working so now you can see i drag this curve down a little bit maybe i'll drag it up a little bit like so okay so now i need to constrain this so let's do the midpoint of this arc is at the midpoint of this line and now we can see that that arc is no longer blue it's fully constrained so again i always kind of like test and try to make sure things are working the way i expect that looks good then we're going to use just this line i don't have to create a surface or anything like that i'll come in here and say split the body what's the body to split in fact i'm going to expand this open that's the body to split what's my splitting tool i'm just going to make sure i click on that line that arc and we can see that it's going to take that arc and basically create a surface and use that to split that's kind of what's happening in the background you'll notice i have extend turned on that just you know gives us a little bit extra border all the way around instead of just to the edge of the line i usually have that turned on watch what happens to my body's folder when i say okay we now have two separate bodies now we don't need body too so we're going to go ahead and just remove that not delete but remove we don't need it we're going to remove it from our design basically if i were to say delete there's things that are referencing that and you could it could get kind of confusing so i always use remove and notice we now have one body if we look at it from the front it's nice and curved and we could go back and change that curve just by editing that arc if we wanted to and we basically created everything all i need to do now is mirror this whole body so instead of features this time i'm going to say let's mirror the body that guy what's my mirror plane i'll click on that face there kind of gives me a little bit of a preview and i want them to join and we now have the pockets on both sides however we also have the counter bore on both sides which i really don't want the counter bore on this side so i'm just going to come in and select these four faces and say delete and you can see that it's now a hole the counter bore still exists on the top but we basically just deleted that counter bore feature just by selecting those four faces okay there's a chamfer that goes all the way around so i'm going to click on this one edge and say chamfer it's a one millimeter chamfer and again because of tangent chain it went all the way around my model in fact i'm going to go ahead and select both of those edges and we're going to chamfer both of those edges all the way around okay one last thing here actually a couple things we might run a little bit over i apologize there is some screw holes here and we can see that they're 100 millimeters apart okay so i like to use the hole command but what i'm going to do is i'm going to create a sketch and i'm just going to throw a couple points on here so i'm going to use the point command i'll just do one there and one there for example okay let's go ahead and project the body we might need to use that then i'm going to horizontally constrain these guys so i'm going to say i want those two to be horizontal with each other i also want them to be horizontal with the origin and we know that they need to be 100 millimeters apart so i'll come in here and type in 100 but now how do i get them to center well just like i showed before i could throw a dimension here and it says it's 31 well i'm going to click on that guy and divide it by 2 and just like that we now have these points that are exactly where they need to be i can use the hole command and here is a neat option at a point a single hole or from sketch so i'm going to click on this from sketch i'll click on one of these points and it'll give me a quick preview what that's going to look like well obviously we don't want that so i'm going to change it to a countersunk hole we want it to be a simple hole and the depth is going to be 10 the diameter the countersink diameter is going to be 5.5 again according to the drawing i'm just grabbing this from and the whole diameter is going to be 5.2 so i've kind of it's created that little countersink we've got that drill point we got at the right depth and then i can just come over here and click that point right there by doing this from sketch i could just keep clicking as many points as i wanted to i could even do that center point if i wanted to we'll say okay okay and i could come in here and say obviously we want that to be tapped or whatever so now they're tapped holes the last thing i'm going to do here is this little groove that cuts through these fingers so i'm probably going to create a new sketch for this obviously and let's do it on like this side plane and i can kind of rotate a little bit project and again i'm going to project the whole body and you'll see that it just basically grabs the whole outside shape of it that i can reference instead of just a single face or whatever if i had done selected entities i'm going to create a slot and let's just do a center point slot because i want to control the height of my slot so i'm just going to get near this center point here move straight up and i'm just going to go ahead and click somewhere i don't care where the diameter is eight and i've created this slot but you'll notice that that arc and that arc are blue that's because it doesn't know how tall that slot is supposed to be so we'll come in here and throw a dimension from that edge to that point it needs to be i think 44 if i remember correctly from the drawing and you can see that that grew and it's fully constrained i'll finish my sketch and let's do a symmetric extrude so i'm going to say extrude start to drag we can kind of visually see what that's going to look like let's go symmetric and we're going to obviously go all the way through and we can see it slices all the way through and we are done with our design so i would go ahead and save that so not an overly complex timeline probably about 15 15 steps 15 features or whatever but the fact that it's got you know the curve the shape we used the mirror command we basically built a quarter of it mirrored that mirrored that and then we mirrored the whole body to get that other side so let me check the questions really quick i know we're over i don't see any more um so hopefully you all learned some new tips and tricks with that like i mentioned before the outline and the drawing are in the description of the video and want to thank everybody for attending and join us next week where i think angela is going to take this part and show how you would put tool paths on it to manufacture it with that have a wonderful rest of your day thank you you

Channel: Autodesk Fusion 360

Views: 20,257

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, computer aided design, free software, 3d modeling tutorial, manufacturing, laser projector

Id: 5nrjujHIvEg

Length: 66min 51sec (4011 seconds)

Published: Thu Jun 24 2021