360 LIVE: Miter Saw Stand project

[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 um on my the keyboard is my friend angelo juris will be answering any of your questions um we're going to go through another series uh you guys i've seen some of the feedback on facebook and in the comments that you really like these series that i go through where we assemble like a pencil sharpener or the laser projector and so this time we're going to do this table saw stand and you can kind of see we're going to learn a couple new things we're going to use commands such as you know sheet metal to create you know this sheet metal part it's got some interesting folds and stuff to it and some tabs we're going to be doing mcmaster car components 3d splines we're going to learn about you know different types of joints so you can kind of see how this whole thing works together uh we'll learn how you know to create the tread on this tire etc etc so um i'm also going to be showing some new functionality in fact i i included the outline and the drawing set um in the description of this video but i actually updated it today because of new functionality that we just released yesterday that we're going to incorporate in in this design so you'll see that as we go through so with that let's dive right in um like i mentioned before the the outline and the drawing set are in the description of this video so you can download those at a later time if you want to um okay so the first thing we're going to do um actually i'm going to point out some of the new functionality that i was talking about this is the drawing set and this is what we're going to be working on today is this kind of this exploded view assembly that you see i'm going to jump over to the tube and here is one of our new enhancements you'll notice that we just added in broken views into the drawing so even though this pipe is much longer i was able to create a broken view you'll notice that the dimension is correct and even shows a little broken view icon in the dimension which i think is really kind of slick so we're going to start out by creating these parts that you see on the screen here i'm going to show some some cool tips and tricks on modifying multiple parts at the same time so we're going to learn that also we're also going to learn about thin wall extruding we just added that and we're going to use that in this example here so here's just the drawings we're going to be using and then on this piece here it actually goes between the two pipes and you'll see it actually like conforms to the pipes on this drawing you'll see that it says length defined by the spacing between the tubes so we're gonna learn how to do that also okay so the first thing i want to do is in this design we're gonna be using metric so i'm going to change my unit type to millimeters i'll say okay and hopefully that makes a bunch of you happy i know we try and switch between inch and metric to appease everybody um so i'm going to start by creating that tube and like i've mentioned before we always want to start with a component so i'm going to right click at my top level and say new component and we'll give this a name i'm just going to call it tube and i'll say okay and you'll notice i now have a new component called tube the other thing i'm going to do i'm going to go ahead and save my design right now you'll notice it says untitled um i'm going to go ahead and save this i'll call it live stream stand that way like my auto save starts to kick in automatically so it's always a good idea to save your design right after you start okay so let's check out one of these new commands so i'm going to create a sketch on the side plane because the the pipes are going to kind of be going left to right so i'm just going to create a sketch on the side plane here and i'm going to draw a circle and in this case i want it to be 45 millimeters in diameter so i'm going to type in 45 and hit enter okay in previous releases if i wanted to make this a pipe i would come in here and say extrude and then i'd have to shell it out and i'd have to select the front face and the back face to do the shell and then i'd type in the thickness and so it added a bunch of extra steps into my timeline but you'll notice in the extrude command we now have this new option called thin extrude i'm going to go ahead and select that and you can instantly see what it does it allows us to add in a wall thickness so let's do something like you know three or six or something like that and you can see it's going to take the profile and basically add a wall to it so really cool command called thin extrude we're going to use that a couple times today so i want my wall thickness to be 1.5 and my total length according to the drawing was 1200 millimeters i'll go ahead and say okay and you'll notice i have the just one feature in my timeline the extrude feature but we have a hollow thin walled pipe okay um i want to i'm going to jump back to the drawing here real quick let's jump back here i'm going to create you can see that we're basically going to be creating the pipe and there's a little nut that's actually welded to the top of this pipe and we're going to when we create the drawing set we're going to learn how we can add you know welding symbols and all that kind of stuff to our drawings because we now have welding symbols but to do that i'm going to put a hole through the part and then we're going to insert in one of these metric 8 hex nuts so i like to use the whole command so let's kind of zoom up here i'm going to say the whole command i'm just going to click somewhere kind of near the top and what's kind of cool in fact i'll kind of go to a little bit of an angle over here and by default fusion is going to put that on the very top of the part okay if i had clicked more toward the side over here it would actually put it on the side every 90 degrees which is kind of cool okay and i'm going to make this a little bit larger so we can kind of see what's going on here real quick so you can see that there is the hole i want it to be a certain distance from this edge here so i'm going to just click on that face and you can see it allows me to enter in a distance in this case it's going to be 30 millimeters from that face and you can see when i type in 30 it goes ahead and positions that hole the center of that hole to be 30 millimeters from that edge okay the other thing is let's say by default it came in looking kind of like this where it's going all the way through the part and when i say by default it usually remembers the last screw type that you did and the last length and the the diameter etc so sometimes it goes all the way through well i only want it to go through the top of this pipe so i'm going to change this distance and i'm going to say 2 and i'm just going to click on the inside of this pipe and now you can see that it's only going to cut into through the top of the pipe i can tell it i want a simple hole i want it to have a flat drill point in fact it really doesn't matter in this case but i'm going to leave it flat and then finally i'll come in and specify the diameter which is eight millimeters in this case and i'll say okay and we just created a hole now why did i use the whole command to do this well one you can see it creates a feature in my timeline but think about how would i have to have done this with a sketch i might have had to come in here and say we want to create a tangent plane on that face you can kind of see it does that then i'd have to create a sketch on that plane etc etc draw the circle dimension it from the edge which would totally work there's nothing wrong with that but i find this just to be much quicker and it's really easy to come back and edit that feature i could come in and change the the size of the hole i can add it to have a countersink or whatever to it for example so i really like the whole command okay now let's go ahead and put that nut on top of there so i'm going to insert a mcmaster car component i'm going to make the window a little bit bigger so you kind of see what's going on here in the outline i not only describe in fact i'll show you it'll ruin my thing here but um on the very first page you'll see i even call out what it is and then you'll also notice a part number this is the mcmaster car part number so you can search for them or you can actually search for it using this information here so i'll do a little bit of both so you can see how that works so i'm going to do the mcmaster car again make this a little bit larger so for example i can click on the nut icon and then over here i obviously want a metric nut so i'm going to click on metric and it kind of filters some things out i also know that i want a metric eight so i'm going to go ahead and click on the m8 and then um you can kind of see it gives me different options of all the different types of nuts well i want to do a hex nut like so and then it displays all of the different kinds whether it's medium strength you know is it fine thread regular thread etc and in this case i'm going to go ahead and just do this first one here and so this is that part number that i was telling you about so i'm just going to click on that and if you see this little cad symbol that means that there is a 3d model associated with that so i'm going to click on product detail and you'll notice right here where it says cad i can come in and say i want you know a solidworks file and i just file a step file i can even say step with no threads which is kind of cool they just added this functionality and then even 2d drawings if i wanted a 2d drawing i like to use the step format and i'm going to say download now what this is going to do is you can see it very quickly brought it in but it's kind of in the wrong spot so i'm going to drag it sort of close to where it needs to be okay not exactly where but pretty close something like this and then you'll notice in our move we have this capture position this is a free position so typically when you say capture position it captures it in your timeline and so that could make your timeline get fairly complicated pretty quickly but with this inside here when i say okay you'll notice it didn't add that feature into the timeline so it's almost like a free pre-capture okay now i want to put it where it needs to go and to do that we're going to use the joint command so i'm going to say joint command and like i've mentioned in previous live streams i always usually get questions like well which one does it matter which order you click and the answer is yes and so you can see here it says component one and component two and i came up with a little phrase that helps remember which one do you wanna move and where do you wanna move it to well this is the one that i wanna move and i wanna move it to the pipe over here so i know that component one is the one i want to select first and you'll notice when i hover over this face in fact let me kind of move a little bit i get all these little tick marks where i could select well i want to grab the center point okay now as i'm moving around you'll see it kind of flashes quite a bit and it's kind of hard to catch that point because it's looking at other edges and faces and a lot kind of stuff so i want to control my selection so on a pc i'm going to hold down my control key and now notice as i'm moving around it's not selecting any other edges or any other faces i'm actually controlling my selection as soon as i let go of my control key it starts flashing again and locking the stuff so a neat little tip hold down your control key and that allows me to basically say i only want to capture the tick marks that are on the face that's kind of selected right now so i'm going to grab that middle point right there okay where do i want to move it to well this is interesting this is a curved surface and you'll notice if i hover over this edge the joint origin isn't really giving me anything that's really helpful and the nut will be positioned in the wrong position but watch what happens when i hover over the whole face so you can see this is the face that kind of defines the hole and you'll notice it has a top a middle and a bottom so i'm going to click on that top mark and you'll see that sure enough it moves the nut and it lines up those two points just like you were to set that nut on top of a curved pipe now if i could show my let me i can't really move my camera or whatever like that but you'll actually see there's the there's the stand in the background that's what i've been modeling it off of and all that kind of stuff um there's a weld they just basically put the nut there and they kind of weld it around that and we're gonna do that when we get to the drawing set but so i'm gonna go ahead and say okay and we've now positioned that nut on the end of that pipe and if i were to move the pipe you can see that the nut moves with it okay moving forward here there's also basically what this nut is for is there's a knob that goes into here and it helps um hold the extension arm in place so let's go ahead and insert in another component mcmaster car component and instead of you know clicking through and looking for it this way you'll notice that there's a find search window right there so i'm going to do a search for the part number which in this case was 290 7t27 and when i hit enter you're going to see that it's actually going to find the seven arm grip you know black nylon plastic or whatever you can kind of see here it found let me move this over a little bit you found that part number okay so i didn't have to go searching for it but you can see sure enough it's a metric eight all that kind of stuff so i'm going to say product detail that's what it looks like i want the step file i'll say download and just like before it's going to insert it into our design and you'll notice it kind of came in at if i turn on my origin you can kind of see those light orange planes it basically comes in at zero zero zero but we're working at the other end of the pipe so i'm just going to drag this over kind of drag it up a little bit get that free capture position and then again i'll use the joint command which is the one that i wanna move this guy and i'm just gonna catch the center bottom right there so i'll click there where do i want to move it to well i want to move it to this and i'm going to look inside the pipe and again i'm hovering over the hole and you can see that it has a top a middle and a bottom so this time i'm going to click on that bottom point and you can see how it brought the the whole knob and the bottom of the thread is basically right right there at the bottom of that hole kind of a cool little trick in this case i'm leaving these as rigid i mean i could make it revolute and all that kind of stuff but in reality there's no need to i'm just i want these to move together so i'm going to make it a um a rigid joint type and i'll just say okay and if we move the pipe sure enough the nut and the knob move together just for fun um i want to change the color of the knob um because on the real one it's yellow so i can come under here and go to modify appearance or the a key for the shortcut so i'm going to hit a and you can tell i was already in there here's all the different default materials i'm going to go to plastic you can see we have different plastics i'm going to go to translucent and there's a a glossy yellow so i'm just going to drag and drop that onto the the knob okay now unfortunately because this is a mcmaster car component you'll notice it's one part in fact let me expand open the tube here and you can see because this is our active component these parts came in underneath that component here's the body and you'll notice it's one solid body which isn't very realistic for rendering or anything like that so here's another little tip for you i'm going to switch back out of plastic let's go into metal let's just go into like steel now you'll notice it says bodies okay well if i were to drag steel onto here it'd make the whole thing steel well i'm going to change this to faces and now i can i'm going to zoom up here i can drag this steel rough onto like that thread and you can see that it just colored that face so i'm just going to do that again i'll do that with this face here this face here and then finally the inside thread and so i just colored those threads the individual faces a different material so kind of a neat way to colorize certain things on your part so for example this whole thing could be yellow but maybe this top part i wanted it to be black or something like that i could just assign it to that face okay so i now have a tube and if we jump back to this assembly here you can kind of see we basically created this tube and it's the exact same thing over here so we're going to learn how to you know move and copy and a lot kind of stuff so what i want to do is start to kind of organize so here's my tube and i'm going to basically create an assembly so i'll right click up here and say new component now the reason i like to right click here and do it instead of from the menu is i'm basically telling it where i want that component to be so for example if i right clicked here and said new component it's going to put it underneath the tube okay let me undo that but if i were to say here and say new component it's going to put it underneath the stand so let's call this table assembly i'll say okay and now you can see i have this table assembly component well i want the tube to be part of that so i'm just going to grab the tube i'm clicking and dragging i'm going to drop it onto the table assembly and now you can see if i expand this open that the tube and everything that has to do with the tube such as the nut and the handle are underneath this table assembly now what i can do is right click on tube and i'm going to say copy now there's a couple different ways of doing this you'll notice it says move copy and this would give me the exact same result okay however i'm going to show you there's two different ways of doing this so i'm going to say copy okay then i'm going to right mouse click on table assembly and now you can see paste and paste new we're going to talk about paste new in an upcoming live stream in this case i'm going to just say paste okay notice my browser i now see a second tube i'm also in my move command and i basically want to kind of move this off to the side and i want to rotate it 180 degrees now how far do i need to move it i have no idea i'm just kind of moving it off to the side we're going to let the 3d model define the spacing of these tubes i'll just go ahead and say okay and now you see we've got this tube assembly here and this tube assembly there really quick way instead of having to recreate geometry okay let me zoom out a little bit here let's take a look so we created the tube we did the whole millimeters from the edge we put the uh steel hex nut on top of there we when we did the extrude we specified it to be 1.5 millimeter wall thickness so we're basically done with this guy so let's move on to this part here which is what we're calling the end cap pretty pretty simple part okay i'm going to be using these dimensions to help me define the shape so once again i want to create a component now why do i always create things as components well it's going to keep my timeline much easier to manage so i'm going to say new component we'll call it end cap i'll say okay notice my other parts kind of ghost out a little bit and my timeline has nothing in it so far and our end cap is our active component okay so i'm going to create a sketch and again i know it's going to kind of go across this way so i'm going to put it on this plane here but just to be different i'm going to draw it out in space i'm not going to put it right where it belongs i'm going to kind of do it out in space and then we're going to move it into place and the overall shape kind of looks like a slot so i'm going to use the center to center slot command and again i'm just going to randomly pick somewhere in space this the overall length is 185 so i'm going to type in 185 from center to center it's at 0 degrees so i'm going to hit enter there and now it's asking for a diameter and it's a 48 millimeter diameter i'll hit enter and we can see what it did it created this slot feature so instead of having to do two circles some tangent lines trim them dimension them etc i just used basically two mouse clicks with the slot command okay like i've shown before i'm still in my sketch but i can click on my profile right mouse click and say extrude and it's going to finish my sketch for me and it's going to put me into my extrude command automatically the overall depth is 19. so i'm going to say 19 and we'll say okay and now you can see in my timeline there's the sketch there's the extrude the body for it the sketch for it's all organized inside that component okay let's shell this part out now i'm going to use the shell command so i'm going to select this face and say shell and it is a wall thickness of 1.5 according to the drawing and there we go we basically have this cap now you might say well how come you didn't do the thin wall extrude well the thin wall extrude is kind of like for a pipe right it didn't seal one end and leave the other end open shell allows me to say i want this face open and everything else stays closed and so you can kind of see sure enough that that back face stayed closed if i had said do a thin wall extrusion of 1.5 and i say okay this is the result i would have got right and i wanted to keep that back face so that's why i didn't use it in this case okay oops um let me change it back to this guy say okay there we go okay now according to the drawing there's um some holes there's a rectangle that goes through and all that kind of stuff we're actually going to come back to that later i'm going to show you how we're going to use some cool tricks to modify multiple parts at the same time so i'm actually pretty much done with this part i'm going to start working on this part which is the end cap cover it's a plastic cover this guy is made out of metal this one's made out of like plastic and it helps kind of protect it so we're gonna um again use information from this drawing and we're gonna use information from the other model so let's jump back into here so under the table assembly i'm going to create a new component i'm going to call it end cap cover you'll see that kind of ghosts out a little bit now what i want to do is i want to create a cover that's basically just going to slip over the top of this and i could go back to my drawing and you know or take measurements and all kind of stuff but here's a neat little trick to do what i would call kind of like an over mold i'm going to switch to the surface tab now we're in thin wall surfacing so we're no longer in the solid tab we're in this surface tab and i'm going to create an offset so it allows me to create a new surface at a specific distance from the selected face so i'm going to say offset what are the faces so i'm going to click on that guy there and you'll notice by default it chains all the way around and i'm going to over exaggerate just so you can kind of see what's happening here so it's taking those surfaces and it's going to offset them and create a thin wall surface now i also want to grab this face here so i'm going to control select that face there and you can see what it's doing it's creating taking those faces and just basically creating a thin wall offset well i don't want it to be five millimeters i want it to be point five millimeters i wanted to just barely clear this other part so you can kind of see the distance there also watch what happens under my bodies folder when i say ok you'll notice that the icon looks different than a solid body this is a solid body here this is a surface body in fact if i turn off the end cap we can now see it's just this little thin no thickness part however under the create menu you'll notice there's a command here called thicken so i'm going to click on thicken it's asking for the faces and you can see by default what it's doing again i'll over exaggerate now it only grabbed that loop so i want to make sure i add in this face here also and it's now almost like we're taking that surface and giving it some thickness and in this case it's supposed to be three millimeters i'll say okay and you'll notice i now have a body i still have this thin wall body it got turned off it's still there i can reference it i could use it or whatever but i now have a solid body that fits perfectly over this other part with 0.5 millimeters of clearance now that's a different kind of a method right i could have recreated i could have created the slot the correct dimensions i could have extruded it shelved it out made sure you know had three millimeters of wall thickness totally would have worked but this is kind of a neat trick to kind of do like an over mold like i want something to go over an existing shape that i have at a certain thickness and have it follow those surfaces so that's why i showed this particular method hopefully that makes sense for all of you okay so now what we're going to do is if i look at the assembly here you'll notice there's some screws and some bolts or some nuts attached to those and they go through both of these parts and this is what i was going to show you that's why i created both these parts first and now we're going to position the holes for those screws so i'm going to still make sure i'm on my end cap cover that's my active component i'm going to go ahead and create a sketch on here and i want these screws to be located at very specific points so i'm going to under the create menu say point i'm just going to go ahead and drop these points somewhere i'll put one there maybe one over here and one down here somewhere okay so i just created three points in space on that face now i can use fusion to kind of define exactly where i want these to be so for example i could say i want this point to be horizontal with the center of this arc here so you'll see it dropped that down and i want this point to be a very specific distance from the center of that arc in this case 30 millimeters 30 millimeters and you'll see it kind of jump to the left a little bit okay same thing with these guys i'm going to constrain those i want those two points to be vertical with each other i also want them to be a specific distance apart i want those to be 25 millimeters okay now if i move one the other one has to move with it or whatever i can also specify that i want that to be a certain distance from the arc the center of the arc so i'll say 30. now if i grab on these guys you can see i can still move them up or down okay so neat little trick here i'm going to create a line and here is something new that we just added yesterday you'll notice in my sketch palette we've always had construction geometry we also now have center line geometry and this is actually really cool if i draw a center line and then i click on revolve it automatically knows that it's going to revolve around that center line so you'll see some some new functionality with this in upcoming live streams but i'm going to go ahead and do just a construction line between these two okay and then i'm going to do a line from here and then i'm just going to hover over this line and let's zoom up a little bit and keep moving down until you'll see it's going to snap to the center point so it kind of sees that little triangle up here so i'm going to go ahead and click there now i have this line that i can say i want that line to be horizontal and watch what happens to those points it has to move those down to keep that point at the center of that so now i know that these two points are centered where they need to be and we can see that it's fully constrained and that's it i'm not going to draw any circles or anything like that i'm just going to say finish sketch but i now have these points where i want them to be we're going to use the hole command so i want to make sure you'll notice i'm in this surface tab still i'm going to make sure i go back to my solid tab and then i can see the whole command in fact i don't even think there is a whole command in the surface tab so we're going to go to the solid tab i'll say hole and right here under placement it says at point for a single hole or from sketch multiple holes and we basically created a sketch so i'm going to click on that guy what's my sketch point i'm going to click here and let's just zoom up so we can kind of see what's going on i'm going to go ahead and drag like so so we're extending past now here's the magic notice right here it says objects to cut and it's folded up if i click on that and i expand it you can see that it's going to cut through the end cap cover and the end cap at the same time and i can visually see that if i kind of look in there you can see there's the end cap and this is the end cap cover i could say i don't want it to go through the end cap even though it physically is so you have the ability to turn those on or off but what's cool about this is we're basically putting the holes through two parts at the same time okay so instead of distance i'm gonna say go through all it's going to figure out how far it needs to do that also i want to have a chamfered edge so i'm going to say countersink and it actually remembered my last entry so it's 11.2 let's pretend that wasn't the case let's just do like six or something okay so i can come in and say i want it to be 11.2 and you'll see that it will create that chamfer for me and then what's cool is i need to make sure my diameter is correct so in this case i want it to be [Music] um i don't even see it um i apologize guys let me look at the drawing um okay diameter six and then this little symbol you see right here this is that um countersink symbol so there's that 11.2 that i was talking about so we're gonna do a six millimeter hole so i apologize i didn't have that in my outline okay so this needs to be six and then i can just click on other points i'm just going to click and click and it's going to use all that information and position those at those very specific points and we can see that it's going through both parts and this is exactly why i said um on this drawing here even though there's dimensions and holes we're going to leave that alone we're going to have this model define where the holes are you know it has the countersinks and everything like that okay so continuing on with this design there is this little plastic extrusion we can see it comes out 25 millimeters it's 35 millimeters square with a two millimeter wall thickness so i'm on this end cap cover i'll go ahead and edit this sketch again instead of having to create another sketch i'm just going to go ahead and edit this sketch again rectangle center rectangle it's at this point right here and it was 35 by 35. i'll click on that profile and say extrude okay now i'm going to start to drag so we can kind of see what that looks like and we know we need to go 25 millimeters for the total extrusion but once again here is where this thin extrude really is going to come in handy because it's only going to affect this part right here if i said okay and had to do a shell it you know the shell is gonna incorporate all these other faces so i'm gonna say thin extrude and let's change that wall thickness to two according to the drawing i'll say okay now you're gonna see a little bit of an issue it doesn't go all the way through the part well that's okay so what we're going to do now is make sure my end cap is turned on i'm going to turn off my sketch so it kind of keeps things clear i'm going to click on this face and say extrude now watch what happens if i go this way it's going to add material if i go this way it's going to start to cut material and just like before notice it says objects to cut if i were to change my distance to all notice what it's going to do it's going to take this shape and it's going to cut through both our parts i'll say okay we can now see through and it's cutting through our end cap now why does this matter well check this out i'm going to go back to this extrude here let's change the wall thickness let's make it something like six i'll say okay and our hole updates accordingly so no matter what this wall thickness is it's going to stay the correct size going through let me go ahead and undo so you can see that sure enough that updates also kind of a cool little trick there with that cut command you know objects to cut we're doing one thing and it's affecting multiple models and they're kind of linked together right if i change something on one the other thing has to update accordingly and this is where i really kind of geek out check this out i'm going to activate my end cap and notice there's the extrude right there it automatically added it to my um end of my timeline of that component automatically the last thing we did and notice that they even did the holes the last thing we did we basically did a sketch we did an extrude and we did a shell and that's where we stopped with this part but because we cut into them with the whole command and because we cut into it with the extrude command it added those into the timeline pretty pretty powerful i think okay let's finish this guy up according to the drawing there's a one millimeter radius that goes all the way around and we want to change it to be a different material so i'm going to select that edge say fill it one millimeter so i'll say okay so i see um somebody asked a question um is there a way to change the name of the instance um i'm guess i need a little bit more clarification are you talking about like for example this is called end cap cover and then there's just a body i can rename this body i could call it you know my cover or something like that it really doesn't matter in this case okay so you can change the names there if in here i could also change the names of this extrude so if i right click you can see it says rename so i could call this you know whole through you know both parts or whatever you can give those things names so notice this says fill it one but if i hover over this it now says hole through both parts so okay so let's continue on here i want to change the appearance i'm going to hit a for appearance let's uh we're going to make this out of plastic so i'm going to go to plastic you can see some default plastics here i want to do a textured plastic and you can see here um plastic texture random polka dot regular skin we have a couple different ones i'm going to just do this random just going to drag and drop it onto my part and if i zoom up here you can kind of see what that looks like i can edit that i could change the color to be you know more of a red or whatever or a lighter gray you can kind of come in and change that all you want so i'm just going to go ahead and leave it like so and it's a little bit of a lighter gray in this case okay um okay so um looks like angelo clarified the question so where here it says like tube colon one and tube colon two um that the instance number so in this case i can't change you know i can't rename you know to be zero zero one or zero zero two or anything like that so those those get created automatically so a great question uh whoever asked that okay so we now have the end cap we have the end cap cover what we want to do now is kind of assemble these together so i want to make sure um that the table assembly is my active component because i'm going to start adding some more stuff into it so i'm going to go to table assembly that's my active component and then i'm going to insert a mcmaster car component so we'll come here make that a little bit larger and in this case i want to do a metric six phillips flat head screw so i'm going to go to screws and bolts metric i'll filter for metric six only and then if i kind of scroll down here you can see all the different types well i want to do a flat head screw and um 14 millimeters long so that's this guy here and so you can kind of see it's basically filtering everything out to show the different types of 14 millimeter long metric screws well now the only thing that's left are the different head types so you can see this is a hex drive then we've got phillips etc and you can see right here i'm going to switch to philips and now it's only showing me the phillips heads and this is the one that i want or i could have just searched for that number up here but i like to kind of show the power of this filtering over on the left so i'm going to grab that guy we'll download this um and again notice where it kind of came in so i'm going to get it sort of close to where it needs to be it doesn't have to be exact or anything like that i'm just going to put it like there capture the position i'll say okay we'll zoom up and i'm going to create a joint so what's the one well i'm going to line up the top edge since this is kind of like a tapered edge or whatever i'm just going to grab that edge there and this edge here now you'll notice it put it in the right spot but obviously facing the wrong direction well i can say flip and it's going to flip that around and we can see that sure enough that's going through the part i'll say okay we've just positioned that and again i'm doing these as rigid instead of revolute or anything like that now i want to create a nut on there to kind of hold this whole thing together so just like before we'll do a metric six in this case so metric six hex nut you can see we can do lock nuts etc so i'm gonna say hex nut and i think in this case it's this o16 3d step i mean a lot of this is repetitive so i'm kind of going a little bit faster bring that up bring it over capture the position say okay now you'll notice because my table assembly is active here's the that rigid joint right there so it's showing up at the table assembly level not at the very top level it's these joints are basically have to do with this table assembly so that's why i made that active and these are the joints that are going to be underneath that assembly in fact watch what happens to rigid1 when i create another one you'll see another rigid appear so i'm going to say this face here to this center point there and it puts the nut in the correct location i'll say okay and now we can see that second rigid joint right there okay so what happens if i move this black part now this is i'm trying to highlight things that happen to me all the time i'm going to go ahead and move this black part and you'll notice that the screw moved but the nut did not okay why is that and this part didn't move well i didn't build a joint between this metal part and this plastic part okay so that's why they didn't move together and when i positioned this nut i actually captured the whole location on this part not on the screw so the nut is associated with this part here i know this can get a little bit confusing and so here's some tips that i use that kind of help me out these are basically assembled the way that i want them to be so under the assemble menu there is a command called rigid group i'm going to say rigid group what are the components well i want i'm just going to say yes i'm going to select that guy also and i'm basically saying make all of these rigid with each other so i'm going to say ok and now when i grab that black part they all move together it doesn't matter which part i grab they're rigid they're glued together welded together whatever term you want to use it's a rigid group okay so remember when we created this black part we basically just grabbed the surfaces of the gray part and we thickened it and stuff like that but we never ever said you know create a joint between the two and that's why they were separate hopefully hopefully this is making sense i'm trying to show you my struggles that i run into sometimes as i'm going through these designs okay i want to have these guys be over here also oops um so i'm going to select both of these right mouse click and say copy now i want them to be underneath my table assembly so i'm going to right mouse click on my table assembly and say paste now why am i emphasizing this well i could right click on my i can make this active i can right click here and say paste right and then it would put the screws up underneath the whole stand i want them to be underneath this table assembly so i'm going to right click here and say paste and by default it puts them in the exact same location so i'm going to just drag these to the left out here in space somewhere and i'm going to say ok now here's where things can get a little bit interesting i copied the screw and the nut but watch what happens when i grab the screw the nut does not move with it why is that well it did not copy the joints because i said copy this guy and this guy notice the joints are up here right the joints aren't underneath this assembly here in fact these aren't even assemblies these are just plain old components so sometimes you'll like copy something and you'll go to you know change it you're like why didn't that move together that's because the joints are actually right here now there's a simple fix i'm just going to come in here and say i want those to be together so i'm going to say rigid group that guy and that guy now they move together i'll go ahead and create a joint i'll say that edge there that edge there now don't freak out you'll notice the nut didn't move but as soon as i say okay it has to update that rigid joint so sure enough that worked let's do that again i'll copy and this time instead of copy and paste i'm going to use this move copy just to show you it's the exact same thing so i'm going to say move copy however you have to be very aware the very very first thing you need to do is cre hit this create copy because if you start to drag you'll notice it's not doing that okay so um let me go ahead and suck these again real quick i'll say move copy i want to create a copy of the nut and the bolt and i'm going to drag that to the left and you can see now it's creating a copy it's allowing me to move those but just like before there's no it didn't copy that joint so i'm going to do this rigid group one more time here say okay add the joint from here to here say okay and we now have this what i would call an assembly okay and if i move any of them they all move together okay now you'll notice my um structure is getting a little bit um crowded so i want to kind of clean things up and basically what i mean by that is all of these little nuts and bolts that you know because we've made copies of those they're kind of being listed here so i'm going to create a new component at my table assembly i'm just going to call it hardware i'll say okay and now you can see i have a component called hardware i'm going to go ahead and grab those guys drag it inside there and now notice how simple that looks okay i'll come back to my table assembly i'm going to go ahead and move and watch what happens okay again i'm not the best person to explain why did this happen my understanding is because of how i reorganized this it's actually tied to the timeline when things happened in time and by reorganizing by by moving those into the hardware it forgot or it hasn't even happened in time yet that those were supposed to stay stuck to the screws okay and like i said i'm showing you my mistakes i'm showing you what i struggled through because i hear this a lot where you know you'll mirror something and there's a part out in space somewhere or whatever so i'm just showing you some tips and tricks on what i do to get through some of this um i do know that you know the people in charge of fusion are trying to come up with you know better methods that might make this easier in the future make more sense like why is things happening the way they are but if you really dug deep into this it's it makes sense what it's doing is it has all has to do with the timeline now i don't want to get too deep into that so how would i fix this well just like i did before i could come in here and say you know what fusion i want this to be a rigid group so i'm going to say rigid group and i can select yes i'm going to say yes on those guys hardware and notice actually in the timeline you can really see what's kind of going on it's selecting all of those components so i'm saying i want these guys to stay together i'll say okay and there we go so yes it's creating another rigid joint in this case but it's not really affecting anything like um i mean it's adding an extra thing into my timeline but this is my method now if you guys have other methods that you have found that works really really well for you put them in the comments in the youtube video so we can share that with other people like i said i'm not a pro when it comes to assemblies and copying and pasting and all kinds of stuff you're going to learn about paste new you'll hear my struggle with um you know wanting to copy and paste and something happens so i learned about why we would use paste new so you'll see that in an upcoming live stream so okay um at the top of the hour so we are pretty close to uh to being done here um so i want to position this into place so let's create a joint and which component do i want to move well it's basically this gray part and i want the center there to be at the center of this tube so i'm just going to hover over the edge of that tube kind of move so you can kind of see what's going on here and you're going to see it's going to move that component over and as soon as i say okay everything else moves over also okay i know that freaks a lot of people out when they they say joint they click on that and they click on that and they only see one thing move the answer to it is right here which component are you moving the end cap and where are you moving that component to the tube it's not asking you which components and listing all of them it's basically two components and as soon as you say okay all of the other you know rigid joints revolute joints etc are updating accordingly okay so now we have that in place now i know where to put this tube so again i'm going to say joint now i want to move this guy to here so which component which one do you want to move i'm going to just grab the edge there where do i want to move it to well check this out i'm going to move zoom up here and even though there's a hole that's kind of going through it i can still select that center point and it's going to bring that tube over you can see how good that looks that's floating out in space but as soon as i say okay obviously that has to update accordingly okay so we now have the tubes located where they need to be so the next thing i want to do is basically create a copy of the uh this whole end cap going on okay so it's a cap it's a cover it's got some hardware i could probably organize that even a little bit better so let's right click on table assembly new component and i'm going to call this end cap assembly there it is i'm going to select these three and just drag and drop it onto end cap assembly i expand that open now i can see all the parts that are in there but instead of having to select multiple things each time i can now say for example i want to move copy the end cap assembly and it's going to grab everything inside of it i'm going to say create a copy oh okay and here's something good i run into this a lot too the selection cannot be copied because it contains the active component so to copy this selected components first activate the component you wish it to be copied into so basically what it's saying is you can't copy the active component so i'm going to make my table assembly active now i'm going to come in here and say move copy create copy now it's happy i'll drag this guy i'll rotate it 180 degrees making sure it's 180 and i'll say okay and notice i now have two end cap assembly is that one there and that one there and i should only have to do one joint for this guy so i'll say that point there that point there it moves the the one part we can see where it's supposed to be i'll say okay and it did not move all of the rest with it why is that well it didn't copy any of the rigid joints or anything like that with it so again really quick simple solution rigid group i want the end cap assembly all to be rigid with each other i'll say okay we'll create that joint again real quick from there to there i'll say okay and everything moves together all the screws the nuts everything so that that rigid group command is actually really really powerful i use it quite a bit okay i know we're going through at a pretty good pace um running a little bit long but that's okay the last thing i want to show is this little center tube um it's only 25.4 millimeters in diameter so it's a little bit smaller than the other tubes and i want it to be exactly centered now if i turn on my origin you'll notice it's off to the side somewhere i didn't create things symmetrically or anything like that so i've kind of dug myself a little bit of a hole but in reality this happens all the time i didn't realize i should have made it symmetric or anything like that so how can i get something that's exactly centered well we're going to use construction planes i'm going to show two different methods one is a little bit longer and i think will make more sense and then the other one's faster and you'll be like oh yeah i'll probably use that one from now on so what we need to do is we want to create a mid plane now it allows you to create a plane between two faces or work planes well unfortunately if i come in here and say mid plane between this pipe you'll notice it does not let me select that pipe because it's not a planar face okay so what we need to do is to create some planes i'm going to turn off the two end cap assemblies and there is a cool command in here called plane at an angle and this is going to allow me to create a plane through an edge or an axis notice the pop-up next to it or a line at a specific angle so i need to because these are round i need to create an axis first so i'm going to go to construct axis through cylinder what's the face i could do the inside face or the outside face it really doesn't matter and you'll notice that it's putting an axis right through the center of that cylinder i'll do that again i'll repeat my last command i'll put an axis through this guy so now i have an axis i can say plane at an angle what's the line and now notice it's letting me click on that line where before it wasn't letting me do the face i can click on this line and you can see that it's going to put a plane on that line well i want it to be vertical so i'm going to just rotate this guy and that plane is now rotating around that axis to be 90 degrees right there i can shrink these down i don't know if you guys know this or not if you get near the corner you'll see the little dot appear i can do that on any corner of a plane so there it's a little bit nicer so i'm going to do that again plain at an angle on this edge rotate it 90 degrees making sure it says 90 sure enough it does i'll shrink that guy down and that like so now i have two planes that slice right through the center of my pipes of my tubes if i come in here and say mid plane i can go here and here and now it's creating a plane right through the center okay now i'm going to back up to show you a couple other options that would have worked here i could also have done tangent plane on this face and you'll notice it creates a face tangent or a plane tangent to that i'll do that again tangent to that and i have two planes that i could now do a mid plane right so from there to there and i now have a mid plane obviously that's much faster but i wanted to kind of show the whole axis through the center and be able to rotate those planes very specifically okay and then the last way which i think is the cheater way is if i turn these guys back on i know these are symmetric so i could come in here and say mid plane and i could say for example between that face there and that face there and it's going to create a plane right through the middle that you know works but i would be a little leery about that you know if this ever changed or something like that but i mean that's the fastest way of doing it but i i like the uh axis through the center where we created those guys and then we created the planes at an angle and then we were able to do the mid plane in fact if i come in here i could turn off the planes that i really don't need i just want the one in the middle now i could even turn off the axis and let's create a sketch create a sketch i want to you'll notice the origin is in the correct spot i'm going to pretend that that didn't happen maybe it's not exactly in the center we don't want to assume that so i'm going to project p for project i'm going to project one of these tubes now i want to do the whole tube so i'm going to say body i'm going to click on that tube and say okay and we just projected the geometry onto this plane now let's say it wasn't perfectly centered how could i get the exact center well i could come in here and draw just a couple construction lines from one corner to the other and from one corner to the other and then where they cross and in this case it's perfect but where they cross that is my center point okay so that's one method of doing that so i'll go ahead and create my circle at the center and according to the drawing the pipe is how big is it um 25.4 i should remember that 25.4 i'll say okay and finish my sketch let's turn these tubes back on so we now have a plane that's perfectly centered between the two pipes our circle is centered perfectly the length of the pipe okay i'll go ahead and do my extrude command again and i'll just start to drag to kind of give it a direction so here's a neat thing i i don't know exactly how far i need it to go but i want it to go to this pipe so i'm going to say to object and i'll click on that pipe and you can see sure enough it's extruding to that pipe and it's creating that special little curve for me well i also want it to go this direction so instead of one side i'm gonna say two sides i'll start to drag this direction i can see that that's right here and again instead of a distance i'm gonna say two object click on that guy and it's going to extrude that distance to that object and then lastly i want it to be hollow so we'll use the new thin extrude notice my extrude menu is getting much longer here but i can now specify what the wall thickness is um in this case i think it is 1.5 1.5 and it's going to hollow that out for me all in one command so if i turn off one of these tubes we can see that sure enough that's hollow and it's the correct length we didn't have to say it's 70 millimeters or anything like that it's exactly where it needs to be and this will be welded in place when we get to the drawings let's turn on our end cap assembly okay so we are pretty much done now let's take this to the next level this is where it gets kind of fun i'm going to activate this end cap that was that little metal piece that we worked on originally okay let's go all the way back in time let's edit this sketch let's throw a dimension on here and instead of 185 let's make that 300. so you'll notice that that got larger i'm going to say finish sketch and look what happened everything updated accordingly and this is really the power of parametric modeling so the the plastic cover updated the screws move to their correct location the center pipe is the correct length this pipe is the correct distance where it needs to be this is kind of honestly the power of parametric modeling if you kind of think how is this going to work everything updates and that's kind of why i did the you know where we created that one part and then we did the cover and then we punched the holes through both and then we punched the square hole through it because that's where the um the arm extension is going to slide in and out through that pipe and stuff like that but it's so cool that you can you know down the road make a change and everything updates accordingly so with that i want to thank everybody for attending i'm going to check my questions real quick i don't see any other questions that came in so hopefully everything made sense um tune in next week i think angelo is going to continue on with his cam series the intro to cam series and then we'll continue on with this table in fact i'll show you where we're headed next we're going to work on the the sheet metal part here you'll notice like the legs you know rotate into place and all kind of stuff we'll we'll do the handle we'll do the extension arm so this will be a multi-part series but hopefully you're learning some new tips and tricks so with that have a wonderful day and keep fusioning thank you you

Channel: Autodesk Fusion 360

Views: 11,055

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: OQzhOzoDCd0

Length: 78min 47sec (4727 seconds)

Published: Thu Jan 21 2021