360 LIVE: Design a 3d Printed Flag Pole Mount

hello everyone and welcome to another episode of a fusion 360 tech Tuesday today we're gonna do how would you make this so this is actually a flag post holder and there's some kind of some cool stuff going on with this thing and so we're gonna learn a couple of cool new commands that I haven't talked about yet such as the RHIB command the web command I'm gonna show you some cool tips and tricks with with blends and the Phillips and hang tight at the end I have a pretty cool announcement that I think all of you are gonna be really happy about so let's go ahead and dive right in okay this is what we're going to be making and I actually uploaded the drawing into the description of this livestream so you have access to this now this is not like a fully dimension but it's dimension enough that hopefully you'll be able to follow along with this livestream and maybe go back and watch the video and learn how to make this so I'm going to be toggling back and forth to this drawing as we're going through now you can see we're gonna learn a couple cool commands such as this variable fill it I'm going to show you how you can go about doing that I'm going to show how did I make this curved text follow oops this shape here so we're going to learn about that also and we're gonna learn about the web and rib command so I'm gonna start a new design and let me do this really quick making sure I'm in millimeters because the drawing is in millimeters and I'm gonna start by creating a new component now I've mentioned if you're doing a single part you don't really have to do components you could do it as a body but I just personally like to get used to the fact that I'm gonna create everything as components in case I need to use this in an assembly or if I want to create a drawing of it or whatever so let's just call this flag pole oops folder okay so I have a new component called flagpole holder and I spelled it wrong so let me go ahead and rename that sorry okay and I'm gonna start by creating a sketch on this front view now I'm gonna show some tips and tricks there there's many different ways we could go about making this and I'm not saying the way that I do it is the right way or the way you have to do it in fact I'd love to see what you all come up with so please definitely post in the comments of this video if you attempt creating this so your results I love getting emails from you and seeing the comments and everything so definitely if you attempt this put it out into the comments so I'm going to just start by creating a line here I'm gonna kind of do the the basic shape okay so I didn't worry about dimensions or anything now I can come back and say for example this I want to be 60 according to the drawing and then I want the the bottom to be 27 and again just grabbing these off of the drawing now obviously you'll notice some some weird things going on but I want this to be equal now here's a cool little trick I'm gonna just create a line and if I get near the center you'll notice it kind of snaps to the centre automatically for me so I'm gonna go ahead and click there and I'm gonna do the same thing down here and you'll see I sort of snap to the center right there okay then I can come in and use a horizontal vertical constraint and when I click on this line you'll see that it forces it to be vertical okay and so that kind of makes everything equal now now this line I don't want it to be an actual object line so I'm going to select it and in my sketch palette I have the option to turn it to a construct in line and I personally recommend turning these into construction lines so notice what happens now it doesn't recognize it as an object line and so this is all one profile if I had left this as an object line you'll notice that it actually kind of splits the part in half and it thinks it's two separate profiles so I like to change it to a construction line maybe I'm going to come in here and dimension that line which according to the drawing is 95 so we can kind of see how that sort of changed the shape a little bit and then finally I might just throw a circle on here so I'm gonna get near this line and I'm just gonna say this is twenty seven point five again grabbing this off the drawing and all switch to the drawing here in just a moment to show you where I got all of this information I know that this circle is a certain distance so I'm using the D for dimension shortcut so I just hit the D key on my keyboard and it allows me to place a dimension I know this one is supposed to be 45 I think 46 I can't really see I'll have to confirm so let's just jump over to the drawing a 48 my eyes are bad okay so here's the information that I was using so this circle right here is the twenty seven point five and then I'm dimensioning the overall height of that circle being forty-eight so let's go ahead and fix that really quick that should be 48 and then the overall shape of the triangle we can kind of see is 60 wide at the top 27 wide at the bottom and then 95 for the height so that basically gives me my my basic shape right here okay now I'm not gonna add any Phillips or whatever I like to keep my sketches fairly simple so I'm just gonna say finish sketch I'm gonna go ahead and select both of these profiles because I like to start with kind of the major part of the design and this the back is kind of the major part so I'll come in here and say extrude again IB I love the fact that I can come in here and basically you know select what I want and pre-selecting I just right mouse click and it shows me the commands that make sense and I find this a huge help instead of trying to find the commands in the menu I know that ok I've selected a profile the only thing I can really do with it is extrude it or maybe edit the sketch okay so I'm going to say extrude and start to drag and I think the total thickness is 8 in this case I'm going to type in 8 and say okay so we just basically created the this shape of the back of this part here now I want to come in and maybe add in some of this detail and we can see that there's actually like a five millimeter wall there are some three millimeter webs there's some holes that go through here so I'm gonna go ahead and do these holes now here's a neat little trick that I'm gonna show you'll notice that these holes aren't dimensioned but they have Center lines so they're actually based off the center line of this blend or fill it right here so if I create this fill it first it'll automatically position these holes for me let me show you what I mean by that okay I'm gonna come in here I'm just gonna click on this edge to pre-select it all right mouse-click and again it shows me the commands that make sense in this case I want to do a fill it those are supposed to be 8 so I'm going to type in 8 and I'll go ahead and select the other edge so I picked one edge I told it to do the Phillip command and then it allowed me to select this other edge and you'll notice that it's a radius of 8 now the edges down here are radius of 5 but we have this cool functionality where I can come in here and just hit this add a new selection so I'm going to go ahead and do that and then I'll select these bottom edges and notice how this says eight my new selection says zero but let's go ahead and change that to five so I think this is really cool because typically when you want to blend something you know or fill it something I want to do like all the edges at the same time in one command and so this allows you to do that so instead of having a whole bunch of filip features in your timeline we now have one filip feature that basically has two separate sizes to it in fact I can even come in here and rename my feature so instead of calling it just fill it I could say base plate blends or something like that for example and now when I hover over this it says extrude when I hover over this it actually says base plate blends so you can rename any of these features including your sketch I could come in here and say this is base plate right and so now you know once I have a whole bunch of sketches I could just hover over this and know that this has to do with the base plate sketch pretty cool I think okay so let's go ahead and now I want to do the whole so I'm going to click on this face right mouse click and it shows me the commands that make sense now I've shown the whole command before which I could use but in this case I'm gonna actually create a sketch I'm gonna say sketch will do the circle command and this is what I was talking about notice I'm not snapping to any grid or anything like that but when I get kind of near the center of this Filat right here it automatically snaps to that location I'm just going to go ahead and click right there and type in the the whole dimension which is 5.25 okay I'll do that again I just come over here and it automatically caches to the location I don't have to do any dimensions or anything now I'm just going to draw a circle I don't care what size and I'm going to do the same thing over here I'm just going to draw a circle and I don't care what size they're either okay what I'm going to do now is I want all of these circles to be the same so we'll use a constraint and there's one here called equal what this allows me to do is I want this circle to be equal to that circle there and same thing here I'll just go ahead and click those and now you can see all three are the same size so again it's still having to type in five point two five over and over again three times I just did it once and then we used the equal constraint and what's nice about this is if we were to come in and say that's supposed to be eight all of those would update all so I don't have to edit each individual dimension so that equal constraint is very very useful okay now I obviously want to make this more correct okay actually you know what I just realized something I'm gonna back up because you'll notice where my origin is right here I want to actually make this a little bit more centered and I realized I want this to be centered so I'm going to go ahead and finish the sketch right now and this happens a lot you'll you'll go ahead and do something you're like well how come that didn't quite work and I'm gonna come back to my sketch right here and sure enough we can see that I'm not lined up so I'm going back in time to this very first sketch and I can now say for example I want this point to be coincident with that zero zero and notice how it moved over in fact let me undo so you can kind of see what's going on here nothing is really constrained I can tell that by my blue lines but once I come in here and say this circle the center of the circle to be at 0-0 it's now fully constrained which is cool I'm gonna finish my sketch it did my extrude it did my fill it so I'll go ahead and edit this sketch now and let's just move this guy over just a little bit okay so now we can see how we're centered so again I accidentally made that mistake but I'm glad I did because I wanted to show you you can always go back in time make that change and all your downstream processes will update okay so now I'm going to dimension this guy so I'm just going to throw a dimension from here to here of six according to the drawing and I want it to be lined up so again I'll use this horizontal vertical I'll say that point there and that point there and you'll notice it lined it up to be vertical with each other and it turned from blue to black which means that it's now a valid sketch it's fully constrained so I'm going to finish my sketch and I'm about to show you another cool little trick here I want to extrude these now you'll notice as I'm moving my mouse around it kind of flashes and it's sometimes hard to pick the profile it's you know right there okay sometimes you have to zoom in to grab this profile zoom in to grab that profile zoom out and then zoom back in again right we've probably all experienced that well here's a neat little trick I'm just gonna come in here and say for example press pull and I'm just gonna draw a box now you'll notice I want to make sure I select everything so I'm going to kind of come up a little bit higher I'm just going to draw a selection box around these three circles and you'll notice how it's selected all three of those so instead of having to zoom in and hope to catch my profile whatever I just your a box around everything now I can start to drag and again how far do we need to go well the answer is far enough but you have a couple options I can actually hover over and you'll notice my cursor says snap to negative eight so it's actually kind of like probing through and grabbing that back face and it'll actually snap to that back face or I could come in here and say instead of going to distance just go through all and it's going to extrude all the way through the part and I like to use that one quite often okay especially because if this thickness changed or whatever it'll still always extrude through all of it no matter what the thickness is so there we go we got the three holes in there okay what we're gonna do next is I want to create this wall thickness now it kind of looks sort of complicated there's a lot of arcs and circles etc well we're gonna use a really cool command called shell so I'm just gonna select this face right mouse click and again it shows me the commands and one of them is shell I get this little blue arrow I'm gonna start to drag and you can visually see what's gonna happen here and also notice what happens when we start to get larger than that circle there it kind of combines it all together which is pretty cool okay and you can see that we're gonna shell to the inside and in this case five millimeter wall thickness so I type in five we can kind of see how that updated and notice how quickly we were able to create that particular shape using the shell command and not using a complex profile okay the next thing is to create these little arms here let me kind of you can kind of see what's going on right here again this is a fairly complicated profile but we're gonna use a really neat command and that command is the web command now I don't know if you've played with this or not but I'll show you how this works it's very very powerful so what I'm gonna do is I want to create a sketch on the top face the top of my web basically and it's gonna extrude down so I'm gonna click on this top face and say let's create a sketch okay then again using the drawing we can see here that there at the angle of 45 degrees so based off of the center marks of these circles so that's what I'm gonna do I'm just gonna create a line at 45 so we'll come in here all I have to do is get near my circle you can see how it automatically catches to the center and I'll start to draw my line now I want to be very precise so I'm going to tab over to my angle and I'm gonna type in 135 because that's the you know the opposite of the 45 right because this is 45 up here I'm gonna do 135 and you'll notice as soon as I type in 135 it's locked into place and so no matter where I move my mouse it's stayin at that angle which is really cool and then all I need to do is get near this line I'm just gonna go ahead and get near that line and you'll see it snap right to it I don't really care what the length is all I care about is it starts here and it's the angle of 45 and it ends there and I'll do the same thing let's just go this way I'll tab over type in 45 in this case and get near that line and you'll see how it snaps to that line okay then finally I'm just gonna get near this point and go straight up and believe it or not I'm done I do not need to offset any lines or anything like that all the web command requires is a profile so I'm going to say finish sketch and we can see that those lines are sitting on top of our part right here I'll come in and say web so it's asking for a curve now I'm gonna go ahead and click this line right here and we're gonna see an issue happen but notice what it does it actually uses this line and it's gonna create this web based off of that line so I can come in here and tell it what thickness I want it to be three millimeters thick and this is what's really cool I'm gonna go ahead and select this other line and you'll see how it automatically selects it also but here's the issue you can kind of see it's going through our hole right here and that's because of this option right here extend curves now if I turn that off you'll see it goes exactly the length of the line but then it leaves these little notches so I need to come back and maybe edit my sketch a little bit so let's go ahead and do that I'll come in here and edit my sketch and maybe instead of the line going all the way to the center we can come in and trim it so I'm going to say trim and let's just trim it too right there I just click on the area I want to trim away and now I'm saying just go to that curve okay so now let's try the web command I'll select that edge there and sure enough I can have extend curves turned on so we it goes all the way to that part but you'll notice it doesn't go through our whole right there I tell it what size thickness I want whether I want it to be five whether I want it to be free or whatever I can tell it to be symmetric so it's gonna add the web on both sides or you can do it in just one direction but typically you'll do it symmetric I'm just gonna go ahead and add in that second one there now here's the another issue I'm gonna go ahead and add in this third line and you'll notice that it's extending to the next geometry which is way down here and I actually don't want this in here now I could come back and delete these faces but what I'm actually gonna do is do this almost in two areas here so I'm gonna do just the X and I'll say okay and we've just created those little webs let's go ahead and expand open our sketch and turn it back on and we'll use the web command again so I'll say web what's the curve I'm gonna click on this curve and now you'll notice that because this area was created it didn't have to extend all the way down so we're actually doing this in two steps I'll go ahead and say ok and there is the back of our part and if we take a look at the actual model you can kind of see you know the crisscross and that little vertical line okay now I'm going to show you something really cool I think this is neat I don't know how many people know about this I want to put a small fill it on a whole bunch of edges okay and that would take me a long time to select all of those edges so I'm just going to come in here and say fill it and instead of selecting edges I'm actually going to select a feature so I'm going to grab this web feature and check this out I'll type in let's just say 0.5 mm and instantly it selects all of the edges that had to do with that feature okay so imagine how long that would have taken me to select all of those edges now you'll notice a little thing going on here it didn't blend like this edge here so I'm going to go ahead and select this other rib and you'll notice how it goes ahead and does that also okay now there's a couple in here like you know might want to add in so I could always come in and and grab more edges to add those in if I want to but the fact that it's selected all of the ribs now I'm going to go ahead and cancel out and do that one more time because I think it's so useful I'm gonna say fill it will select that feature and that feature and tell it that we want it to be 0.5 okay and it grabs all of the edges that have to do with those web features now I show that it didn't do these edges right here I'm like well I could select those individually or I could come in and select the shell feature and notice what it did it grabbed all the edges that had to do with the shell so we're actually grabbing multiple features and it's selecting all of those edges I'll say okay now I hope you think that's as cool as I do imagine how long it would take for us to select those where now we can just grab a couple features in the timeline and it doesn't automatically so thumbs up fusion team for that loved it okay let's move on here we basically finished the back of the part here in just a couple moments now we want to start working on the the front of this so maybe one of these tubes right here so taking a look at the drawing let's just kind of zoom out a little bit we can see the diameter of the tube is a 34 and a half with a wall thickness of 3.5 but how are we gonna create this tube and this is where it kind of gets how would you do this right and that's kind of why we call this how would you make this part well what I've done here in this drawing is I have this centerline and we can see that it's 40 millimeters up from the bottom and it's about 95 millimeters long so we're going to actually create a plane in this particular direction that's 95 millimeters away from that point and we're just going to extrude to our part so that's I'm kind of giving you the the movie trailer part what are we going to be doing here so okay so let's go ahead and create another sketch and because I created it at the zero zero we're symmetric right so I'm gonna grab this face of the origin and I'm just gonna draw a line I don't care what length what size what angle I'm just gonna draw a line like so now I can come back and dimension this so I want to go from that edge there to this edge here and I want that to be 45 degrees and you can see how the line updated I also want the length of the line to be 95 millimeters again according to the drawing so we kind of see how that updated and then we know that the point right there needs to be 40 millimeters from the bottom of the part so I'm going to type in 40 and again we can see that that line is now fully constrained it turned black we know the angle we know the length and we know the location now once again I don't want this to be an actual object line so I'm going to select it and turn it to a construction line like so and we're done and if we kind of rotate around we can kind of see how that line is that 45 degrees to this face it's right in the middle and it's at a particular so what I want to do now is be able to draw a circle at the end of this line okay so to do that I need to have a sketch plane on that line and I've shown this command before but playing along a path is extremely useful so I'm going to say plane along a path well click on that path and that's going to create a plane that I can put anywhere I want on this path I'm going to drag it all the way to the very end you kind of see in fact if you don't know this that the plane along a path is basically a ratio so you can see there's 0.5 if I go all the way to the end that's 0 if I go all the way to this end that's one so it's not really a distance as much as it is a percentage or a ratio right so if I typed in you know 0.75 it's going to be right at you know 3/4 of the way up the line okay so obviously I want it to be at the very end I'll say ok and I now have that plane at the end of that line which I can create a sketch on so I'm going to say create sketch we'll use the circle command and according to this it's 34 point five and that's all I need to do okay I'm not going to draw the inner circle you'll see why here in just a moment but that's the overall diameter of that post so we'll select it right mouse click and it shows me the commands that make sense I'm gonna say extrude now here's another neat little trick how far do I need to extrude well I could drag but as soon as it intersects its gonna cut through right so obviously we want it to we'll say join but to get it to go all the way along that face it would stick out the back line so which is kind of weird right so we're gonna use a cool command instead of distance we're gonna say extrude to an object what's the object I'm just gonna click on that face and fusion figures out automatically for me what does it need to do to extrude to that face so that is the to object and its really useful we're actually gonna use this I think a couple times today and now here's something we're gonna run into I'm gonna use the shell command to hollow out this tube okay now why did I not just draw two circles well I could have very well could have but I like to use the shell command because then I can come back and say make it four millimeters make it one millimeter you meter you know instead of having to go back to a sketch or whatever I can just look for the shell feature and change that in my timeline however I've already shelled out this part and I don't want it to be calculated in my shell so what do we do here well instead of joining it let's actually create this as a new body in fact I'll expand open the bodies you can see we only have one right now I'm gonna go ahead and say okay and now you'll notice that we actually have two separate bodies in fact I could turn this guy off and we're left with this as a separate body it's still extruded to the other part okay but it's separate now I can come in in and say you know what let's shell this out how far 3.5 according to the drawing and if we look at it it's kind of selling it out only one way but if I add this other face it's gonna turn it into a tube we're selling it out the top and the bottom so kind of a cool cool prick there I'll say okay let's turn this other body back on now and you can see that we were able to sell that out now I do want this to be all one body so let's go ahead and combine these together so I'm going to say combined I'll say that part there and that part there we want to join them together and when I say okay we'll see that we're back to one body now we're gonna see an issue here we hollowed this guy out but because we joined it to a solid piece there's no hole going all the way through so how do we fix that well we could have created the sketch and extrude through but instead let's just select that face and say delete and notice what it does it actually deletes that face through our part and now that post is going all the way through very useful command there okay hopefully this is all making sense I can see Aaron's pretty busy in the chat window there if you have any questions or comments definitely throw them out into the chat window so the next thing I want to do is to create this area right here okay and if we look at the drawing I kept it pretty simple we can kind of see a section view of this area so we can see it's about ten and a half wide and five millimeters wide it's curved etc I don't have any dimensions like where it goes to on this post and then you'll see why here in just a moment I left some of this up to your discretion so I'm going to go ahead and create these two curves right here and we're gonna learn another cool command okay so I want to create those curves so I'm going to say let's create a sketch on this side profile here and I'm gonna use the arc command so three-point arc let's just start at the top now you'll notice it captured that point right there but as I hover over here it's not capturing the edge of this cylinder there's no edge that's projected that it can catch too because a cylinder really has no edges and I want to be precise okay so how do we go about doing this we're going to use a command hopefully you're familiar with the project command project allows you to project geometry so for example I can project this face you can kind of see how it's highlighting it red right here so it's gonna project that face onto our sketch plane here but you'll notice if I hover over this it doesn't project an edge it's only projecting the end right here so that's really not helping me in this case so you might say well what do we do well there's another cool command under the project menu called intersect and what this does is it allows you to pick geometry and it's going to project the intersection of this geometry so our piece of paper is slicing through the middle of this tube you can kind of see that here so when I click on intersect and I just grab that guy let's take a look at what it did it basically projected what's intersecting with this plane okay I'll turn the body back on you can kind of see now we have an actual edge that we can catch - so intersect is very very useful especially with like spherical cylindrical organic type shapes okay okay so now I'll do the same thing just so you can kind of see what's going on here let's do intersect and I can grab you know like for example this face right here or this face here it really doesn't matter I'll get I'll grab both of them and it basically projected the intersection on to that work plane or the sketch plane I should say okay so now I'm gonna go ahead and do my arc command so let's say arc three points I'm gonna go from here and then when I come over here you'll see that it'll automatically snap to the center and that's kind of what I did in my example that's why I didn't really dimension it I'm just gonna get what I think looks good so let's just snap to the center there and then I'm just gonna go ahead and place my arc now if i zoom out a little bit we can actually see a center point for that arc and let's go ahead and dimension this because according to the drawing and you see you can see the radius there according to the drawing the radius is 40 so I'm going to type in 40 we'll say okay and there we are then I'm gonna go ahead and just offset this curve the 2.5 thickness again from the drawing I'm gonna do 2.5 and believe it or not we're actually done with our sketch I'm just through basically two curves so here is a new command that I haven't shown it's not new infusion it's just new that I haven't shown it yes so it's the rid the command this is actually quite useful so I'm gonna click on rib and it's asking for a curve now go ahead and select that curve and by default it's usually set to next let me go ahead and try that one more time we do rib make sure my default is usually set to next so I'm going to click on this curve here and you can see it instantly figures out how to fill in that air yeah okay so it's basically taking this profile and extending it to the nearest geometry so we know that the width here is five so I'm going to go ahead and type in five and you can even see that it's curving around because of this curved surface I'll say okay and there is our rib now think about how long that might take not using the rib command I would have had to have intersected it with this because of the curvature of the face I mean it might have taken a little bit of time I could do it but the rib command is so useful in fact let's go ahead and use it again for the top t part I'm gonna come in here and say rib now if I were to select this guy it's going to basically just add on to it and if I were to change the thickness it's gonna add to the thickness there so I don't want it to go all the way down so instead of saying to the next shape I want to go very specific depth and in this case I want to go to point five so it's taking this edge right here and creating the rib that's two-and-a-half millimeters thick and now I can specify the overall thickness of it which according to the drawing is ten and a half 10.5 and I'll say okay let's go ahead and turn off our sketch here so you can kind of see what this looks like now I see a little bit of an issue which we'll get to here in just a second but notice we've created a somewhat complicated geometry using two simple lines and an arc and another arc okay now what I see here is I see a line that kind of goes across you can see that it did wrap around now I don't like this line right here so I'm going to just grab those two faces and say delete fusion will have to heal that geometry so what it looked like is you know it came to a point and they went straight to the part well I want it to continue this nice curvature to go all the way to the part so I just deleted those phases out of there okay now just like I showed before check this out I can come in and say fill it and grab features so let's grab these two rib features and type in 0.5 and notice what it's gonna do it's gonna fill it all of those edges that have to do with that rib feature okay so I'm not gonna do it right now but I just wanted to show you that that actually works and it does it on both sides so again saving a huge amount of time on trying to you know create you know select all those edges for example okay now let's say we want to create this curved Filat here so you can kind of I'll highlight it in this one here so it starts out small gets fairly large and then ends small again and this is just to add some strength to this tube being attached to this base so how would we go about doing this well we're gonna use the Philip command so I'll say fill it but instead of a constant radius we're gonna do a variable radius okay it's asking for the edges I'll go ahead and select this edge here and you'll notice that it starts with a start point and an end point so I'm going to go ahead and say well we start at one and you can actually kind of see the preview already it's going from 1 to 0 around which is kind of cool but we want to start at 1 and we want to end at 1 okay now as I move my cursor kind of near this edge let me zoom up I don't know if you can see that little red ball very you can kind of see this red ball and this is actually gonna allow us to add in extra points and I'm just gonna kind of move along and what's kind of cool is if I get near the bottom here you'll see a turn green okay so I'm gonna go ahead and click right there and hopefully this makes sense now we can see again kind of a percentage or a ratio from zero to one so halfway along this edge we clicked a position and I want it instead of being one millimeter I want that to be 15 millimeters and now we can see what's going on here it's starting at one as it goes around it's going to go to 15 and then as it gets to the end it's gonna go back to 1 again okay now I don't really like how this looks it kind of tapers off way too fast so I'm gonna add in some more points I'm just gonna move my cursor until we see this red dot again I'm just gonna go ahead and click and notice right here a new point has been created at position point 2:05 well I want it to be a quarter of the way so I'm gonna say 0.25 and I want that to be a radius of 3 and notice what happened it's keeping it smaller then it's getting to a radius of 3 2 right here then it's going from 3 to 15 right here pretty cool right I'm gonna come back over here I'm going to move until I can see that red dot and let's just go ahead and click somewhere like there and I want that to be 3/4 of the way so I'm going to type in 0.75 and again I want that to be 3 and watch what happens okay we can kind of see how it keeps it nice and tight and then it opens up to the 15 so we can create some pretty cool fill it's using this variable radius now you're probably asking okay where'd you get all these numbers let me show you on the drawing over on the side over here I basically described it it's a variable blend one millimeter at the ends three millimeters at a quarter and three quarters and then 15 millimeters at a half okay so that's what that note means when you go to create that variable blend okay so the next thing we're going to do is now we've pretty much created a majority of this we need to create this horizontal flagpole holder because this allows you to hang it at like a 45 or to do it horizontal again just using the dimensions off of the drawing we can see it's thirty four point five our thickness but we notice that it's kind of at an angle and there's a notch cut out of it so we're gonna work on that okay so let's go ahead and I need to be very specific where I want to start creating this part from so I'm going to create an offset plane from this face so I'm gonna go ahead and click on that face start to drag and according to the drawing it's 80 millimeters away so I type in 80 we kind of see what that looks like I'll say okay and we just created a construction plane that's 80 millimeters from that face now I can sketch on this so let's go ahead and create a sketch and I'll draw my profile so I usually draw kind of off to the side and then I bring it into location so I can I know that this needs to be 34.5 okay I'm gonna throw a dimension on here I know it needs to be let's just go here and that needs to be I think it says 46 and again I want it to be in line with the center so I might come in here and throw a line from the center so I can go something like this straight up don't doesn't matter what size and I'm going to convert that to a construction line okay so you kind of see what this looks like then all I have to do is say I want I could say coincident let's just say that guy there and that guy there and you can see how it moved it over fact let's look at it from the front and there's our shape now to save time because I'm running out of time here I'm going to go ahead and create the other circle I was going to show that I would use the shell command but unfortunately in this case we can't I'll show you why here in just a moment so I could come in here and say this is going to be thirty four point five minus three and a half right I could do that so I could say thirty four point five minus three point five and that'll create the circle for me or I could come in here and say offset and I can come in and just drag this down a little bit and we want to go minus three point five in this case okay so there is our shape there's our profile now let's go ahead and extrude this guy will say extrude start to drag and again we're gonna run into that weird issue and all kind of stuff so let's use instead of distance let's just say to object and click on that other pipe and you're gonna see that it's gonna figure out what it needs to do to actually extrude to that shape I am I'll go ahead and say okay now again we see this issue here so let's just select it and hit the Delete key and now we're looking through the part so we were able to make that go all the way through now unfortunately there's an issue here and if I expand open this guy you can see that there's actually a vertical wall so it's not a tube it's basically a tube with vertical walls so how am I going to do that well let's go back to our sketch and I'm going to just create a basic shape so I'm just gonna get near this circle here and this kind of extend up a little bit I don't care how far and I'm just gonna kind of get the basic shape like so now obviously I want to be more precise so I'm gonna say I want this line to be tangent to that circle I want that line to be tangent to that circle and I want those lines to be vertical so I'm gonna say that line to be vertical and that line to be vertical so I'm basically just adding a bigger profile section right there okay now I need to edit my extrude and instead of just saying this little region I need to expand it to that region there and kind of see what that looks like so it's going to extrude the cylinder and this region here to look something like this kind of weird okay the next thing we need to do is to add in this 45 degree angle now how do we do that again there's many different ways you could do this I could maybe drop from the side and machine in the way or whatever but instead let's use the draft command where this actually allows you to add Draft now you'll notice it's asking for a draft plane and I basically want to hinge it right down here at the very bottom but my origin plane is way up here I really don't see a draft plane that I could use so we need to create one and we're going to use the construction menu tangent plane I want to be tangent to a curve so I'm gonna say tangent plane what's the face I just get near this face and check it out it actually puts a plane right on that face and I can specify what angle I want that to be right now it's at zero or minus 360 but I could say I want that plane to be a you know 45 degrees or whatever right well we obviously want it to be at zero I'll say okay now I have a plane where if I came in and said Draft what's my plane it's basically gonna hinge right here so I'm gonna click on that plane what's the face I'll grab that face there and we'll start to rotate and let's just go minus 45 degrees now unfortunately it looks like it's cutting let me I might have to do this before I do the cut so this is interesting that this happened this way so let's go ahead and cancel that out and um I want to let me see what do I want to do here go ahead and I'm gonna suppress that feature for the deleting of the face let's try that first I want to try this let's go draft that what's my face that guy okay so that wasn't the issue unfortunately um so let's do before this extrude right here so I'm going to come back and unselect that guy and say okay and let's do let's just taper this feature right now so I'll come in and say draft here's my plane there's the face and we'll rotate minus 45 and I think I see what's going on here it's because of that little knots right there but we'll say okay then let's come back and edit the extrude here so let's how do I do this I'll come in let's add this guy maybe oh I let's try this maybe this profile is too high so let's just bring that down a little bit lower let's just see if that helps with it and when I do my extrude I'll add that guy back in say okay okay I said this multiple times I also make mistakes now you'll notice I went through and said okay why is this happening so I think what was going on was my profile was too high and as it was rotating through it was starting to cut way more material so I said maybe I need to blower that down a little bit so that's what we did I'll go ahead and unsuppressed this delete and I should be okay maybe I need to do that oops yeah I'll just do it again I'll say delete looks like it's saving it there we go okay I'm going to go ahead and turn off my construction plane really quick and now you can see we have this basic shape now I'm going to kind of cruise through here because we're getting toward the top of the hour and I like to keep these less than an hour if possible the next thing we want to do is to cut out this little notch and again not a lot of dimensions here I basically gave you one dimension and we're gonna use some geometry to help us out so let's come back here click on this face and I'm going to just create a quick sketch here now according to the drawing we're basically referencing some existing lines and again I want to catch to the edge of the cylinder so I'm going to project intersect so I'm gonna grab that guy there say okay and it projected the intersection of that body okay watch I'm on the wrong face there that's okay let's go ahead and do that again I apologize I'm going to put my sketch on my middle plane there so I meant to do okay then we can do our intersect because I really like to show that intersect command so we'll grab this guy and we can see it sure enough it projected those lines for us what this is going to allow me to do is I can come in and just go from point to point I get that guy there I can project this line here and let's offset that line the correct distance so in this case 21.5 so it's kind of hard to see what's going on here but I basically projected the edge and then I offset this line to get this corner right here and we got the right distance now I can use a three-point rectangle so I can for example grab that point there grab this point here and I'm just going to come out here in space a little bit so we used that geometry to help us create that shape now we can extrude how far I'm going to just say all now I want it to go in both directions so I'm going to say symmetric and we can see that it's going to cut that notch out of there I'll say okay and we've now cut that notch it's perfectly lined up with that tube and there you can kind of see what that looks like okay this next section I think a lot of people are going to be excited about I posted a picture on Facebook with some some text on this curve and people like ok how are you doing that are you using that sheet metal trick or whatever no I'm gonna show you what kind of a neat another new neat trick here that I use quite a bit to make the text actually match the curve of the pipe so that's what we're gonna do next so to create text I need to have a construction plain so I'm gonna do a tangent plane I'm going to click on this curved surface here and I want to put it at a particular angle so let's just go maybe like minus 35 degrees now you'll notice I'm getting a warning message down in the bottom corner and it says the object you're creating is not visible well that's because I've turned off my construction as soon as I turn it back on again we can now see where that plane is I can see that I'm at an angle of 35 okay I'm gonna go ahead and sketch on this plane I'll quickly create my text here so let's just say text and type in what I want so on this it says made in USA let's go ahead and rotate that so we're 90 degrees let's make it bold and I can now position this kind of where I want it on there and I'll say ok so that text is now sitting on a flat piece of paper right on that face ok now I learned this from you guys I used to convert or explode the text but if you come in here and say press pull I didn't know this you can actually you don't have to convert your text so thank you all for that so we're gonna extrude this text but you'll notice it's gonna be flat okay and that's not what we want so check this out before I extrude I'm actually going to grab this face using my surface commands I'm going to create an offset and this actually allows you to offset individual faces so we can see here we've got chain selection on or off so I'm going to just go ahead and click on this face and I want to offset that one millimeter and you can kind of see the preview there it's it's taking this blue face and offsetting it one millimeter and watch what happens when I say okay it actually captured that face and it's a it's a surface right now okay so I'm going to turn off for now I'll come back to that now I'll do my extrude or my press pull I should say so let's just press pull out a little bit how far let's just go to millimeters I also want to go the other direction because I want to make sure it's intersecting that curved surface and let's just go ahead and join these together so here we are we've extruded our text it's totally flat now I'm going to turn on this other surface and we're going to use a cool command called replace face well this allows you to do is to replace one face using the another face okay so I'm going to say replace face what's the source face let's click on this guy and what's the target face it's going to be this surface here and you can kind of see the preview I'll go ahead and say okay what it did it replaced that flat face with the curved face and now you can see how that M is actually matching the curve of this tube now I could do all the text but you get the idea it's the exact same thing I would just select all of these guys and and match them but what I love this check this out I can come back and change my offset so instead of one millimeter let's just say 0.2 millimeters I'll say okay and you'll see how it actually updates that thickness there so that's how I went about making this curved text on this part you can kind of see how it follows that shape so that is using the replace face command okay so that's pretty much it now all I would have left to do is to come in and fill it you know the edges that I want for example so we want those to be in a 1 1 millimeter etc etc but that is the basis of designing this part so we actually did quite a bit in just under an hour okay I mentioned that I had a cool announcement I want to we were too hopefully gonna have a video like a another camera but we're gonna have some more live streams from one of our cam specialists named Angelo he's recently joined my team awesome guy very very knowledgeable on cam he actually comes from Tesla and has done quite a few parts for that in fact I'm gonna just bring up his Instagram page really quick he's gonna start doing some live streams that are really focused on the cam side of things and let me make sure I'm sharing my screen here there we go we back up a little bit so basically a very very strong machinist so you can see like for example here's something he's creating infusion here's another part etc I'm not gonna say much more than this I want him to introduce himself so keep an eye out for him you're gonna see him on some upcoming live streams focused a lot mainly on cam everything from basics to more advanced type stuff I am you hopefully you can see my face uber excited that he's part of our team so keep an eye out for make sure you subscribe make sure you give thumbs up thumbs down whatever if you like this video other topics you'd like to see we are looking through all the ideas that you come up with and adding those to our list and we hope to see you on a future livestream so thank you

Channel: Autodesk Fusion 360

Views: 30,668

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, photogrammetry, mesh, mesh editing

Id: dt_kkO-ojcM

Length: 69min 35sec (4175 seconds)

Published: Tue Mar 26 2019