Fusion 360 Tutorial - How to model a Diresta Toolbox - Season 3

if you follow this channel regularly you know that i am not a great woodworker see that uh that gap right there i am not one of these people who find great fulfillment in doing everything myself i don't find any joy in hanging a lamp or fixing a broken faucet or change the oil on my car it's not that i can't i've hung more blinds that i can count and have changed plenty of brake pads remember when brake drums was around and you used to have to put that spring back on when you assembled everything again what i do love is learning new things and i hope that's why some of you guys also come to this channel from time to time i follow many makers and have learned many tips and tricks but one guy stands out and again if you follow this channel you probably know jimmy the rasta if you don't follow jimmy do so please he has so many tricks up his sleeve and i follow him on youtube and on instagram so go ahead and go and follow jimmy show him some love give him some thumbs up last week jimmy did this toolbox on instagram and he did it one-handed because he had to hold his phone in the other hand that's just how good he is but like i said what i love the most is these small tips and tricks that he shares as he's going through and i want to share those with you but of course first we're going to have to model this thing up in fusion 360. now there's many different ways we could model this thing up in fusion 360. depending on what we want to get out of it we use parameters we could do all different kinds of techniques but i'm going to show you how i would model it up if i had to make it well actually i did make it i'm also going to show you how to make a 2d drawing so it's easier later on to prove to yourself that you made a mistake by cutting something too short and maybe if i get some cutters next week's video could be how we would lay it out and we will program it in cam in fusion 360. if you're one of those people who upgraded you a level from an old band so it's one of these fancy cnc routers let's go all right so we're gonna start out with a sketch always a sketch right and we're gonna select a plane so i'm gonna select the top plane here so i always start out with a 2d sketch on a plane that's how we normally start out here and i'm going to go up and select my center rectangle so already when i do that i'm probably going to use some symmetry in my sketch here and i'll show you that just in a second so send a rectangle and i'm going to just drag it out here and you will see that i can put in the numbers so i'm going to make this one 200 millimeters hit the tab key and i'm going to make it by 500 millimeters just like that and hit enter so we end up with uh with a box here now this is going to be my top view and this is kind of going to be the bottom of of this toolbox so i'm using sketches to drive all my modeling downstreams what i call skeleton modeling or layout modeling it just it just makes it a lot easier when you come back and you gotta edit things later on so this sketch is fully defined it's black 500 by 200 i'm gonna finish that sketch now i'm gonna go up here i'm just gonna expand out this sketch here and we can see that we have a little lock on it is locked down it's sketch number three i'm gonna slow left click on it and i'm gonna change this to top sketch and i'm gonna show you just in a second why i will do that because i'm gonna use sketches to drive everything all my modeling like i said going downstream so naming these from the beginning makes it a lot easier you can also use this view cube kind of like as your guidance here so the right view is going to be the next one so i'm going to create a new sketch and i'm gonna do that on that right view plane you can see when i click on that that we're now in the right view meaning that sketch4 i'm gonna rename that right view now i am going to sketch and one of the things that can make it easier for you i think in the beginning is not to worry too much about placing things in the right location let me show you what i'm talking about if i go up here and click the line command and out here in space i'm just going to create a line and you'll see that it's going to try to snap vertically but it's fine um so i'm just going to go ahead here and place a line and then i'm going to do one at an angle i'm going to go over horizontally and down in another and i don't know you're gonna worry about where i'm placing this actually the last one here i'm gonna place in an angle and hit the little check mark so this sketch um let me just hit escape to get out of the line command this sketch here is you know completely kind of loose sitting out in space now what i can do is this one is sitting on that right plane right there what we can do is we can associate this sketch with this sketch so if we ever decide to go in and change the width of this box that then this second sketch sketch the right scheduler sketchfall will update with it so let me go over here and just place myself to the right view here one of the ways we can do that is we can hit p on our keyboard p for project and i'm just going to select this line what is the line from our top sketch and hit okay and when i do that you'll see i get kind of like a couple of purple dots here and that means i now have that as a reference line and that reference line will update as we're changing the width of the first sketch so now what i'm going to use is a combination between constraints what you'll find up here and dimensions and yeah the dimensions tool sitting right over here so what i can do is i can go over and say all right i'm going to make a incident constraint and and one of my rules of thumb is trying to use constraints first and then dimensions at the end so i click coincident and i'm going to place a coincidence between the moving point and the the stationary point you see that that slams in there i could go ahead and do the same thing with the second one so i can go ahead and say this one to this one and you will see how it kind of adjusts like that now i'm going to hit escape and you will see that the sketch is still blue what means i can grab any of these corners and i can kind of start seeing what is still locked down see i can't move this because this is now black and locked out all right so then we can move over and we can say all right so we could we saw that we have this vertical here and we could go over and use that same vertical for this one we could also go over and use something like a parallel right let's say this one here or this one here should be parallel to this one and you will see that now they became parallel that will do it we could also start looking at see this is going in an angle here but they're not this thing and this link is not the same same length we could go ahead and say that we could use an equal between this one and this one and now those two lines will stay equal length no matter what i kind of like do like this so these constraints up here um kind of be can kind of be your your friends um another thing you can do that many times can become helpful is that you can use this symmetry constraint i find that one useful and the way that we could we could use that one would be to draw a line so i'm going to hit i'm going to go over here and say select line or hit alpha line i'm just going to create a line up here and if i want to get out of there i can just double click and we have a line right there we could use the symmetry and the symmetry works by saying this point and this point and then select the line and then the this is now symmetry with that what means that whenever drag things now like now we have this uh symmetry in here where we can we can move that so i'm really using all my my constraints up here to try to get as far as i can um before before i'm i'm going to put dimensions on it by the way if you want to make that one construction you can select it in its construction line and then becomes a dotted line here all right so now let's add some dimensions to lock this one down so i'm going to hit d on my keyboard or you could select up here same thing d on my keyboard and let's go ahead here and i'm going to make this one 85 like that and i also know that i'm going to make this one here here i'm going to make this one 200 tall and then this happens and you're thinking like oh my goodness what just happened well what happened was that the the angle the predefined angle i had here over constrained the sketch and it was just it's just really just a bad placement error the way out of it is like you can just do a control z and then an undo right to get back here and and then we could just go ahead here and just change um if i delete this dimension here we could just change this up here to a different angle and then when we hit the sketch dimension you will see that now it's gonna work so it's just because i had my um oops it escapes get out of this um i had my my line too far down and fusion kind of crossed these two lines because you could go two directions and it shows the wrong one so 50 50 select the wrong one now you look at this you think all right this is pretty good right but you can see that we still have um something that is that is blue and the easiest way to do is just grab a corner and start moving and you can see that we probably want to put some kind of a dimension on it here so i'm going to go ahead here and do a dimension and you do that by clicking a line and another line and then we get a dimension here and i'm going to place this dimension here and i'm thinking i want to make it 150 what looks pretty good now i want you to focus just take note of that that i use this dimension to make it 150 because when you actually go to make this in word then i'll show you another way when we get to the drawing on how i would dimension this because i don't know about you but doing something in 150 degrees could be probably problematic um or hard to calculate or something like that last thing we need here is i need a hole to put the handle in so i'm going to go up and select a um a center and you could you will see that it does going to snap into kind of the center line here um and if you do that then it's going to be vertical i'll kind of try to align it vertical and i'm going to go ahead here and i'm going to make that 25 millimeters in diameter and you will see that i can still kind of move it around though it hasn't been hasn't been locked down so we can see we got to move it we got to control it this way and we got to control it this way too so one way we could make it vertical is by going and hit the vertical horizontal relationship here and say this point to this point and now i cannot move it sideways but i can move it up and down and i'm going to use the last dimension i have here between the center point and here to place that and i'm going to make that 170. now this sketch is fully defined and i use constraints as much as possible so the only things that i have i have in here as dimensions are these here and the only reason for that is it makes it easier when you come back in six months to look at this again that you can remember what it was now another thing i just wanted to highlight was that we use that projected line down here what means that let me just rename this to right side sketch so i can see what sketches what but if i go in here i can right click on this top sketch here and i can say show dimension and if i double click on this 200 and i change that to 150 you see how this will will follow now you could be intelligent the way you do your sketches like right now i know that if i go probably 80 then i'm gonna get this here um you could be intelligent and put some try to find some ways to to make some calculations where things may be scaled down or something else um but the idea about this is that if we decided that we're going to make a smaller bigger box that that this kind of updates with that that was the idea about that projected line and this is what i need for my um for my um my right view now i need my my front view here so i'm going to create a new sketch and i'm going to do that on that front plane and i'm going to i'm going to go ahead and do what i did before i'm going to hit p for project and i'm going to capture that bottom line and kind of do the same thing as i did before so if it ever change size i'm going to do this showing you i'm going to show you a couple of things here just that you might run into so i'm going to this time select the two point rectangle i'm going to select this corner here i'm just going to draw out a rectangle now it won't snap to that point so i'm going to have to constrain that but i'm just going to go ahead and place it somewhere around here and then i could now go ahead and i could select coincident and i could find that point right there zoom in if you can't see it it's like one pixel there so there and then i got that now it's still blue on top because i haven't defined my height yet um but i wanted to show you something else before we do that we could go ahead here i want to create a scenario where i'm actually gonna run into to some issues so i'm gonna go ahead and select another two point rectangle and i'm gonna go ahead here and create a little lip there and now i might want to start doing some dimensions so i'm going to go ahead here and i'm going to create a dimension from here to here and i'm going to say i'm going to make that 53 and i'm actually going to do the same thing over here 53 and i'm going to break this just in a second and then i also know that i need this to be i want this to be 60 right there and just for the heck of it let me just throw that all the dimension on that too remember what that was that was supposed to be 85 from the first one now you do this and then i wanted a radius to go down here so i'm going to go over and i'm going to select an arc and i like the free point arc and the free point arc if you hold over it comes up with a little dialog saying place start point so i'm going to place a start point and then it says place an endpoint i'm going to place an endpoint down here and then it's kind of want to select um the the midpoint of it now if i move it down here you see that i it snaps and i get a tangency see if you look at that little icon of that tangent arc that actually shows up on my part here and shows me that i got this so this is actually pretty good so i'm going to left click to place it and that's good now it's blue because it's underdefined but i'm going to go ahead and create another one in the same kind of way down here place it here and snap it down to the tangent like that okay so what people many times will do is that they will say all right so let me go ahead and put a dimension on that so d for dimension and i'm going to make that 40. that's good okay i want to do another one the dimension oh and i'm going to make that 140. now now we see that the sketch is fully defined then if we go up and we use the trim and i say i want to remove this i'm going to move this i'll move this this and this suddenly you will see that things turns blue and people are like why is it turning blue suddenly well the reason it's turning blue is because when we are trimming uh these different items we are actually removing these dimensions if you see it because we are we're deleting we are trimming this line what means that this line gets created into another segment just between the two radiuses and that means that the 60 will get lost so or that section between that will get lost it still keeps the line if i go ahead and select this top line here then it's losing that line when i create those two there so it loses those segments when i i'm not sure if this is a good way to show it but when you do these trims you're losing segments and things can turn blue that's a warning because now your your sketch is um is under defined so that's a thing to kind of keep in mind and now you the only fix here if you're going this way around it but there's nothing wrong with it but is you you kind of got to go in and and redo these dimensions again to to make it fully defined so how would i do this well i would normally not put any dimension on it until i got it to where where i want it so i wouldn't put any dimensions on this thing until i got all the all the things drawn up it's kind of what you saw i did on the one before so i would draw all this stuff up and then i would start dimensioning it so let me show you a couple of tricks to do that so if we go ahead here now we could go ahead and we can trim these and we're not running into any issues with with things going like work we have done already becoming um becoming like that all right so let me show you a couple of tricks here that you might find useful so one i probably would start out with is this 85 so let me just you know move this down a little bit so the first one here was 85. now if i just finish to stop the sketch for a second you know that we have 85 over here and there's a couple of different ways we could do this we could do like a projected at a point from here in our sketch and then we could we could align with that so let me show you that so we could go ahead here go back into our sketch here and we could do a p for project and we could find that in a section see that's right there and i could project it up there and now i have that point so we could go ahead and do a incident of this line to this point now make sure you don't select make sure you don't select the point and make that coincident if i select the point to there then it would actually blow up you they would bring the line over let me undo that but if you're selecting the point that the line and then the point then it will do the coincident another trick that i want you to know is if i get out of this sketch is that every dimension let me go back to this sketch every dimension has a a name and a number or a letter and a number you see how this one says d3 85 so what we can actually do i'm just hovering over it that's how i got it to appear just hover over the dimension what we can actually do is we can go back into our other sketch edit sketch and we can go ahead and select d for dimension select this line and then i can type in d3 now when i do that you will see that it shows up fx what means that this dimension is driven by something else this dimension is driven by the other dimension so if we go back into this dimension here of this dimension and we change this to 75 and we go back into this one you will see now this is 75. so our second sketch is now driving this one okay now another thing we can do that can be helpful is that if we go ahead here and select d for dimension and i'm going to make this one 53 now we can also now you we used it before we can go ahead and use the equal command and say i want this line to be equal with this line and now those two lines are the same length so i don't have to place two dimensions that also of course goes for d for dimension for this if i know i want this to be 40 there's no reason to place another dimension down here i might as well say that this one is equal to this one and then that will always stay 40. and then the last dimension we need is from here to here and make that 60 and our sketch is fully defined let me just move the 60 down here so they all are kind of like in one corner by itself so i hope this is somewhat useful different ways you can do things in here so we created three sketches and that is all the sketches we need to create this toolbox now we have created these different sketches and we can now go ahead and rename this one so this is the front side sketch or front right side sketch whatever so we now have these three sketches that is driving different areas so if we go ahead and change this to 600 that wall will update and if we go and change that we know that this sketch is updating so these the fewer dimensions you have on your sketches the easier it is kind of going in and making modifications all right so now we are ready to go ahead and make solids but we don't we we are not going to we're going to have these sketches up on top and then we're going to have our bodies further down so what i'm going to do is i'm going to right click and say new component and i get to give the component a name and i'm going to call this one bottom so i'm starting with the bottom and when you do that you get this little fish eye showing us that this component is now active and that's why everything kind of like got shaded or cloudy is because this is now active we go up and we click up here then the whole assembly is now active we go down click here this only component is active all right so with that active i'm going to go ahead and say extrude and i'm going to select that bottom and i want to go minus here so i'm going to go minus 12. so that is uh is my bottom pretty pretty easy that was the easiest part of the whole thing uh let's go go ahead and create another component and i'm going to call this one my my side like this and i'm going to go ahead and hit extrude again and i'm going to select our side view here now notice how it's actually extruding from the center and that's one of the in the standard extrude command one of the options you have here is where do you want the profile to start from that's a lot of great information over here so we can go over here and say well i wanted to start from an object and then i'm going to select that face from that solid we just created and then i'm just going to drag the arrow the other way and say i'm going to go minus 12 millimeters and hit okay and now we have a side here that um that sits on the bottom starting right on that intersection right there if we go ahead and we make the bottom active we will see that that becomes active and the whole thing looks somewhat like that now i'm gonna cheat right now and actually just mirror this because i need two of these so i'm gonna go to create i'm gonna go to mirror and instead of the default faces i'm going to go ahead here and select components because that's what we have here this is components i'm going to select the object and the mirror plane i'm just going to select that plane right there see now i use symmetry again and i have that other one sitting right there so now we got that so that's pretty good now as i'm doing this i'm realizing that i might run into a little bit of a scenario here that my my third sketch my front side sketch actually interferes this should probably just have gone to to where these are ending but i'm gonna deal with that and show you a little trick on how i can do that so let me go ahead here and right click and say new component and um actually as you probably call the these let me just cancel out of that actually this is not this is not a side this is an end and slow left click and that's better i want to call the next one aside new component i call that a side and i'm going to do what you saw me do before i'm going to hit extrude i'm going to select that thing right but again it's not where i want it to start so i'm going to say from object and i'm going to select that face there and this is the same as before i want it to be minus well that's actually plus plus 12. and just go ahead here make sure new bond is on and hit ok and um rename that because i didn't do that when i created it i missed something outside and then i'm just going to rinse and repeat what you saw me do before and i actually don't have to be in the in the top document to mirror i could be in here it's still smart enough to know where to place it so mirror it remembers now this component and i'm going to select that mirror plane right there and hit okay let me move up to our top component here so we can kind of see the whole thing and this looks pretty good but we realize though that we have do we have an issue here like i'm you know demon wrestler is good but there's no way we can merge these two corners together without cutting something away so we can cut away and the technique we're gonna use is this it's it's called combined but it's a little misleading because it actually does other things so i'm going to click on on that and instead of of joining i'm going to say cutting and i'm going to show what body is it that i want to to target and in my case i decided just because of the 85 and everything that i'm going to cut these panels shorter so i'm going to select that and then it says select the tool bodies and the bodies you can only cut one body at the time so i have to do this twice but i can use two tool bodies that's gonna be these two they're the ones i'm gonna cut with but if i just hit okay they're gonna go away so i'm gonna make sure check keep tools hit okay and now that got cut a little shorter and then i'm just going to repeat that so i'm going to right click repeat combine select this panel and then i'm going to select this one and this one to cut and keep tools and hit it like that now somebody would say well you're adding too many too many in here because what i could do was if i just go back and i just select this one down here hit delete see we mirrored this over here right um we mirrored over that body to that or that component to that component well what would happen if i dragged this one hold down the left mouse button and i directed over here so you can reorder this timeline where things are depending on one another so instead of doing two instead of doing i'm now doing if i move this back i'm now doing the cut before i mirror there's many different ways to do this all right the last one i'm gonna go ahead and do is i'm going to do the handle but my sketches are gone because as you are doing extrusions fusion kind of consumes the sketch well we know that if this gets up here i can just turn it right back on and it shows up and now we can go ahead and do another new component what we're going to call handle i'm going to extrude here and we can go symmetric like this and we can either choose if we want to be the whole length it goes or you can kind of divide the measurements whatever you want to do i'm going to do a whole length here but instead of giving it a distance i bet you that the overall length of this is d1 on my dimensions i'm going to hit d1 and now it looks like that that is the right dimension if i hit d2 then it would be the 200 we all remember what d3 is that's the 85 right so d1 is that 500 the first dimension i placed for the length of this box what means that going back to to full circle that if we go i'm gonna turn that sketch off again if we go into our first sketch here remember that 500 added that sketch if you made that 150 that will update that didn't update that is interesting review warning the profile reference is lost try to edit the feature to reselect the profile so something went wrong here i want to edit the profile sketch oh see something gets screwed up up here i bet you that's why it's you see so this is a typical this is a typical issue so you see how you get these yet i get a yellow warning and of course it didn't update the reason it doesn't update if i go ahead and edit that sketch that's the same as the as the front side sketch you see how the sketch is intersecting itself what's what means that fusion says dude i can't i can't solve this and therefore it stays the original length now it simply just means that because i made these two 40 and the way with the 53 they can't be this small so let's go in and edit the sketch again now what happens with mega 200 now it updates because now they don't radius a stone inaccept so that's one of those small things it's just uh kind of that was a lunch pail this is one of those things that oh wrong sketch this is one of the things that i hope that um that you learn something from so we can update that the handle updates and um and the side updates too so this gives us um this box here now the last thing i would probably do is we maybe want to put some appearances on it just to make it look a little bit more realistic and the way we can do that is out in space we can right click and well right click on one of these parts and we can do appearances and you can actually search so let's uh probably make it out of pine so there's a pine right there and if i drag it up here on this ring up here then the whole thing will will change appearance and now it looks more like this box here now we're almost done um a couple of things i would not i would not put screws in this thing for for me to go and make this one i would not place the screws you could we could go up here to insert and we could go to mcmaster components we can put all the screws in and things like that you could lay it out like that but i'm not going to do that but another thing that we still have to do is this became an assembly and well to fix that we have to do something because every component here can move and that's not what we want so we're gonna have to lock this down now we're gonna have to select one part that is gonna be locked in space and i'm gonna select the bottom just makes more sense to me i'm gonna right click and ground it so right click and ground it so you get a little thumb tag and now because of the way i model this up with these layout sketches i know everything is where i want it right now and then i can use this as build joint and the sbill joint just let me click on asphalt joint and i'm going to select on this component and the base here the bottom and i can say that those two should be rigid and then that is locked in i can't drag that off anymore the other ones can still drag off but not that one and then we can just go ahead here and repeat as build joint say this component this component are going to be rigid right click pds build joint this component the side right click this component on this side right click and maybe this component of this component right side and then it's all we got all the the rigid joint down here and now nothing moves a bit i'm gonna click the little eye here to turn off my my joint icon there in the center alright so now this box is actually how i would model this up and uh and be good to go now like i said next week we might do this in a cnc and then we're gonna do some other things we're gonna have to lay it down flat uh to cut it out on the cnc router but because i gotta build this part uh on like old-fashioned bandsaws and stuff like that i'm actually going to make a work drawing for this so to do that i'm going to go up here and i'm going to say a new drawing from design and i'm going to be asked here to to save it so i'm going to call this uh the rest toolbox and i'm just going to select the default uh new assembly here click ok so that's and it's going to open up the 2d drawing so we have now a new 2d drawing here and we have our our toolbox is still sitting up here and go between the two all right first thing we're gonna do is we're gonna insert a base view i'm gonna click on that and our base view come in here now when i did the what's new in drawings i showed you how to create a build material and all different kinds of stuff i'm not going to do this for this one because this is a work drawing really for me just to um to be able to to make this part so what i'm going to do is i'm going to place this box about right here and i'm just going to hit ok to that and we get kind of this box here now when you do that you get all the different components but what i actually want to do is i kind of want to show everything on one drawing so i'm going to insert multiple base views and one of the things you could do is i could go over here and say i want to have a i don't know an isometric view like this here maybe i could place an isometric view down here just so i can see what the heck i'm trying to build and i'm going to make that shaded right so then i kind of have the box here so when i insert uh new base views you will see that i get uh the different components now i can turn them on and off of whatever i want so what i can now do is i'm actually going to insert another base view and instead of here the front i'm going to select the right view remember that i'm just going to place it somewhere over here so i'll line this somewhat up and i'm going to select another view and i'm going to make that the top so i'm actually selecting the views that that you saw me using before but what i'm going to do is now i'm going to turn off the components that i don't want in that view so for example on our top view over here i'm going to uncheck bottom and i'm also going to uncheck the ends so it only shows the side and the handle and on the next one not that one we're going to leave that alone this one i am going to turn off the bottom and i can turn off one of the ends and i can turn off the sides and i can turn off the other side and i can turn off the handle right so i'm kind of like cleaning that up and the last one i'm really just going to show the bottom so i'm using these different base views to show this now we can go ahead and add some um and actually what i'm missing here is i'm missing a thickness so then we can use a projected view if i click objective view of this box here and i move my mouse over you will see that i kind of get a projected view so i'm going to click here and place a projected view of that box all right now i'm going to show you how to put some dimensions on it so our our rod here was 25 and remember what this one was that was the 85 we did before i probably want this one oh i thought that we made that one 53. i'm gonna go and we're gonna go and look at that oh that's because we're actually looking at uh we cut it in half so that's right this is gonna be this is gonna be 41 because we cut a section of it um what else we do we have this one to here or 60. i hope that you got why this is because i cut the side of it and in order to become free that's true um and then we got the this 60 here right you can take that and drag it outside here looks a little more professional um and uh let's hit another then this length is different too it's gonna be 476. this one is going to be the 200 by 500 and then we need a thickness of this little sucker to show us that it's a 12 millimeter thick now i want to show you that and if you remember when we were doing this part over here i when i dimensioned this i dimensioned it um with 150 uh in here and there's nothing wrong with this but i know that when i'm standing down at the shop floor trying to make this that doing 100 doing degrees is always a pain in the neck like unless you're going to go over and find a saw you can rotate a saw or something like that so instead of using the standard dimension tool um be aware of that there is also something called alternate dimensions and alternate dimensions is actually kind of cool because what it will let you do is it will let me do these dimensions in a way that might make it a little bit easier for me to um to measure when i'm out see this is going to be 200 when i'm out there because i can actually now say i can make a measurement from here to here say that's 85 and then i can make a measurement from here in 66.4 and then it would show me that angle that i gotta create so that was a little that's my tip hope it was a good sin and we wanted another dimension to kind of prove ourselves and then do this here like that i should probably spend a little time lining all these dimensions up but i think you get the you get the gist of it i don't know i would make them these out so far all right oh the last one we need is we also need to put a dimension here i would probably just find something that gave me a radius that's close to that paint can or something i don't know um so that is going to be to be our sheet and the only thing we need to really do now before we uh we go ahead and run this part is by going and print this out so go and hit the print and i got my little samsung m2020 and i'll print that so with that we get the paper drawing this is the way we can prove that uh if we make any mistakes i would probably have cut that 500 i'd already forgotten that that was going all right with the printer starting up we will uh we will get to uh to the shop flaw okay so uh the next four or five minutes gonna be uh some giveaways arrested tips and tricks here so you can see that on one side i have uh i have drawn up kind of like the path that i'm gonna be uh gonna be using in the bandsaw and here's a jimmy trick use hot glue i've never seen anybody else use hot glue as much as jimmy the rest of those but this is awesome see i marked where the scrap piece gonna be and that's where i'm applying the hot glue what means that when you get over to your bandsaw these two pieces are now now glued together right when you do your cut on the bandsaw you're gonna get two identical pieces so this is a great way to kind of make two identical pieces this scrap is glued together but the two pieces you actually need are not i would never thought this all right here's another trick um so i have marked our line here this is like our 150 degrees and uh i'm cutting that on my old trust of the vault now here i'm kind of trying to to get it close to the line and look at this using a pencil to draw on the board itself and now now this is not probably super accurate but for this project it was it was super easy to just go ahead and line that up and i was able to make two pieces actually one piece was a little bit long because the cut i had made prior was i made one piece a little bit longer but this was a way to get very quickly four sides that is identical all right next tip here that i and this is where i made a little bit of a mistake but you're learning but this is another thing that i would not have thought about that jimmy taught me was to glue in the pieces and then let that sit for 20 minutes and let the glue harden because that makes it a lot easier to uh to put the screws in later on see i would have thought about i would have been standing there trying to monkey around with the screws and line line everything up but and you can see here on this image that i've actually already screwed in i've already screwed in um the side pieces um but the fact that when you glue it in first and then it's much easier to to align your screws instead of like trying to do it all when everything is loose trying to screw the screws in and stuff like that so i thought that was another another super super cool trick and i also installed the handle here um i just glued i actually just glued that in all right so here is another trick that i would not have thought about and look at how i'm taking the pencil and i'm i'm using my finger as a guide and finding the the middle of the the plywood and then i can literally just trace with along the sides and that way i know where the where the center of my plywood is uh for drilling my holes again i would have been standing there trying to do you know six millimeters in with a tape measure and draw a line but using you know that technique of just taking the pencil and using your finger kind of the guide work worked amazingly so again um one of these other tricks that you know what jimmy thank you i would never have never thought about doing it like that all right it's almost done doing a little bit of sanding and i could probably spend some more time on the sanding here i should have um but you know always under a deadline and then jimmy you know always is good at making sure that his branding is on it so i'll also make sure that well all of this branding is on it so hashtag all of that so i hope that you found this video useful hopefully there was one or two tricks in there thank you to jimmy for always sharing your information and your knowledge love it until the next time take care you

Channel: Lars Christensen

Views: 16,771

Keywords: Autodesk, Autodesk Fusion 360, Fusion 360, Design, Manufacturing, Tip, Beginner, Lars Christensen, #LarsLive, Best Practice, Modeling, cam, cad, tutorial, How to, 3d printing, free software, software, Product design, Mechanical engineering, fusion 360 tutorial, fusion, autocad, design, inventor

Id: ym5TZDzqKVU

Length: 51min 6sec (3066 seconds)

Published: Wed Nov 04 2020