CNC Router with Fusion 360, Bookshelf Tutorial

okay in this tutorial I'm going to take you guys through creating this bookshelf so we're going to start in fusion 360 by creating some parameters we're going to set up a sketch we'll create a full 3d model and then show you how to take that 3d model and prepare it for manufacturing by laying all the parts out putting on some dog-bone fill it's setting up your cam to create g-code simulating that ultimately loading it all up into the shopbot cutting it out and finishing it up and creating the final product so let's get started so here in fusion when you start up you're always in a new design if you want to create a new design you click file new design and now you're in a completely empty project or part or assembly or whatever you want to call it and before we do anything for a project like this what I first want to do is I want to create some parameters so I'm going to create some parameters by pressing the little green check box for example the first one and most important is the ply thickness so let's say I've measured that exactly at point seven two five we want to put this in and we're going to use this all over the place so that as I develop the design I'm always referencing this one parameter of ply so if I go to rerun the job and I measure at point seven three five or whatever for each time I cut a new piece of material I can adjust this one number here and all of the pockets and tabs and Heights and everything else are going to all adjust to accommodate the exact ply thickness that I've defined I can also use this to define overall things like if I wanted to make a configurable bookshelf let's say we wanted two Heights to be 26 inches and we want to create a width of 30 or a depth of 14 etcetera I can keep creating these parameters and I'm going to use them all over the place so fast forward here I've created all of these parameters so you can see I've defined a width a height the depth for the overall bookshelf the ply thickness also defined the cutter diameter I'm going to use so this way I can change this cutter diameter and if I do things like create dog bone Phillips later the diameter of those is going to be reference to the size cutter I'm using so it's nice to be able to reference this here some things I didn't even end up using like this tall if I wanted to put a tolerance gap somewhere I could be referencing that things like shelf kick the tab width also something here like a blind tab or I don't want to go all the way through the material I'm going to say only go about 60% of the way through the material so these are the types of things that you can you create these parameters and then we're going to use them as we go work on this design okay so the first thing we want to do in this design is going to be to create a sketch to represent the profile of the bookshelf so I'm going to say sketch create sketch I'm going to sketch on the side profile face and then we'll come in and start by creating a rectangle and we'll draw this just some arbitrary shape and then we can give it a dimension so here we're going to leverage those parameters we created so instead of typing in the number I'm going to type in the word height and then it's going to show me what that value is same here depth now I can come in and create some more rectangles and these are going to define the different pieces so like the top will have a shelf I'll have a bottom shelf have a little kick plate here and then we'll have a piece along the back and now it's just a matter of creating some more dimensions to define the sizes so the thickness of all of these is going to be ply this is one of the real advantages is by adding this parameter all over the place so we'll create these dimensions apply and then you know once you actually are ready to cut this and you go in and you measure your material very precisely you just have to go in and change that parameter our four ply and then all of this will update and then all your thicknesses and everything else will be all up to date same if you decide you chain you want to change the design we're going to just type in the word kick here again we'll do up to here we change this this is called shelf so if you ever want to change some of the stuff you can just modify those parameters if you do want to use a specific value for example like this maybe you just know that no matter what that's always going to be fixed we just always want that to be one-inch you can type in a regular number at any time in these dimensions as well and now you've got your overall sketch profile defined now that I have this sketch done this is going to kind of outlines all of the parts in the bookshelf now what I want to do is start creating individual components so to do that I'm going to create and extrude and then I want to pick the sections of this sketch for the given part so in this case I'm going to start by creating the top so that's going to be that profile on that so you should pick two things and you can either just start dragging this out but in our case we want to extrude this a specific value and that is width so that's going to be again place where we're leveraging those parameters so you can do that here in the extrude commands as well and when I do that it's going to hide the sketch by default so if you want to do something more with that sketch you can always come back over here to your tree in sketches you'll see sketch one you can show that and we'll do it again because we want to create another piece here so again I'm going to say extrude and here I'm going to create the side piece now this is going to be one two three four five six seven eight nine ten eleven and twelve sections so again this side represents all of those sections so you just need to make sure that you grab all the sections and we want to say new body and for the distance here this is we're going to use that ply parameter to use our material thickness and again make sure the operation is set to new body that's very important and we'll say okay and then we can hide this sketch if we don't need it right now okay now rather than Reese catch this what I can do is I can just take this side piece and mirror it so to do that the first thing I need is a plane mirror about so we're going to use construct and we're going to create what's called a mid plane what you do here is you basically pick say something like this face and this face and then that is going to create a mid plane right between it so you can turn off all of your construction or you can turn on and off this plane here that is going to be a plane that I'm going to use quite a bit through the rest of this design and now create mirror I'm going to mirror you want to select bodies in this case so our pattern type is bodies and our mirror plane is this one and we've picked this body to mirror and now we've got that part so that's going to be a technique that I use throughout this which is to basically create one body and then mirror it across the center plane to leverage it over on the other side so the next thing I need to do is to create the shelves and the back piece they're going go from this inside face to the other inside face so to start features that start from this inside face instead of from where we originally sketched it so if you look you know that sketch is actually on the outside we want to create some features from the inside the easiest way to do this is to quickly create a new sketch on this inside face and then let's just hide some of this stuff for a second and I'm going to use the geometry from the first sketch so project include so what you're doing here is you're basically saying I want to just grab a reference to all of these lines from the first sketch that way if anything changes in the first one you can it'll be updated here and then we're going to use though this new sketch to create some parts ok so now we're going to use that sketch to create the rest of the component so again create strewed and here rather than specifying a value we're going to say we want to go up to the inside face there that way you don't even have to worry about figuring out what that depth is supposed to be and instead of join again we want to use new body and now we've created the back now we'll go ahead and just repeat that process so create extrude and we'll pick this which is our bottom shelf and we will say we want to go up to this inside face and it will be a new body you can right-click and drag up to repeat a command which is kind of nice sometimes so do that say new body up to that face and then again down here can see the kick plate and we'll go to that inside face that looks good and remember to always set it to new body and we'll hit OK now you can hide that sketch another thing that's nice to do here at this point is I'm gonna apply appearance so again I right-click appearance and you can browse into woods you can see here I've got into wood finished and I've got oak glossy Oaks and my gloss let's use oak semi-gloss that looks pretty good and you just can drag this out onto your parts obviously this isn't a necessary step but it looks pretty good when you're modeling in you're kind of looking at it the way it's going to look I like it so now that we have the basic parts I want to create some tabs so that we can create the press-fit joints between all of these components so I'm going to hide all of the parts except for the kick plate and you do this easily by selecting on the light bulbs here in the tree now I've got the kick and I want to create a new sketch I'm going to create a sketch on front-face here I'm going to go and grab my two-point rectangle tool and we'll just draw these two tabs in kind of at a rough shape and then we can go get dimension tool so here I want the depth of this to be apply so it's the ply thickness here's the nice thing we can do to which is I can say okay I know that I have a parameter defined called kick but I want this to be kick divided by three and then the same here so we'll make the tab a third of the depth so if you change that kick parameter this will all update over here also apply and tab and another thing we can do that I use a lot is I'm going to create a quick little construction line so I'll create a line that just goes from that midpoint you'll know you have the midpoint when you see that triangle you can select the line right click say you want to make a construction that way it's really just there for reference and now I can create and quickly create a dimension from the origin which remember this is going to represent the actual edge of the bookcase this is inset by the thickness of the side so I want to go from here to the center and then we want this to be equal to the overall bookcase with over three and that should put us right where we want to be now we can use that sketch that we just created to create the tab so I'm going to create an extrude and we pick the two profiles and here what I want to do is again use the extents I want to set this to be two and go up to that back face and we'll go ahead and leave that as a join just so we can show one way of doing this which is to use that as a join and then I'm going to go ahead and create a mirror and there's different choices here I can either mirror faces or bodies next I'll show bodies but in this step let's use faces just you can see the difference so with faces what I need to do is pick all of the faces of the component that I want to mirror so little more steps so I'll pick those three faces and then for the mirror plane again we'll use that mirror plane that we created and get the result that we're looking for okay so no let's to create a sketch for the tabs on this shelf so sketch create sketch and pick this face and now we're going to create just the tabs on one side and again we'll create a lines for the midpoint I do this because it gives me like a nice way to create a dimension to the midpoint of these rectangles they don't really have to be straight or anything and then what you want to do is pick them right click construction now those are just kind of some reference lines to give you that reference point at the center it's not necessary but I just do it up habit now we'll create some dimensions so we can again leverage our parameters so the width is going to be tab tab tab and then the height of all of these tabs is going to be equal to the thickness of our ply now again remember the point of this is that when I if I was to after I measured my actual material thickness and I go modify that parameter apply all of these tabs are going to adjust as well so you're always going to have a nice perfect fit when you do it this way and we'll also take advantage of our other parameters here so this is going to be depth over 3 this one will be depth over 3 and then here again you hear you want to make sure you're going from the from the edge over to the center of that not from the edge of the shelf and we'll call this one with over three and that should give us the sketch that we need to create these three tabs now we can create an extrude for these tabs so grab the tabs in distance up to that face but again we want to make these new bodies because we're going to really leverage just creating these three and then mirroring them around so we'll take those three then we'll create a mirror of them so grab the three bodies and we'll Muir them around our construction plane here now we've got these up let's go ahead and leverage that for the shelf as well since we want the same exact tab pattern on that shelf again let first thing I'll do is I'll just quickly create a mid plane between that face and that face and that gives me this plane here I can turn these on if you want and then we can create a mirror and this time we'll grab all six of these and then mirror it about that new mid plane that I just created say okay turn the view of that off again lightbulbs turn things on and off and I'm going to use my combined feature so set the target and then all of these are the tools join don't want to keep the tools and now I've got that part that we want and do the same thing here so this is why I like to make these tabs as individual bodies and sometimes it's really just super convenient to mirror them around copy them and then combine them later it just saves you a lot of work in the long run okay let's create this sketch for the tabs on the back so again we'll create the sketch we'll do that here sometimes you might want to rotate around so you're looking at this from the front so you have the right perspective and we'll create our rectangles so just kind of draw these an arbitrary place to start with and then make my reference to the midpoints to make it easier to dimension later and then we'll make these construction so right click construction and now create dimensions so again we're going to leverage all of those parameters so the width of tab for all of these and then the depth on these sides is apply so we want to just have that go all the way through the thickness of our material and then on the top this is going to go into one of the blind pockets so we'll call this one line tab and then for the position we'll go from here to the center we want that to be height over three Center to Center also be height over three and then here we just want to measure from the actual zero point not from this inside edge you really want the outside edge of the whole bookshelf to this point to be width over three and there we go all right again just take these create and extrude of the three tabs to the inside face create new body this way we can get mirror those three tabs about that initial near plane and then do the combine there we go okay so let's create a sketch for the tabs on the top of the side so create a sketch on this face back here we'll create two rectangles and again we'll create dimensions so we'll create all the dimensions that we need and this is going to be depth over three and then we'll just create the rest of the dimensions real quick you so you can see there's a little bit of a problem where we've got the tabs coming right to the edge of the top piece so we really need to make a little bit of a lip to be able to have room for a pocket so rather than try to refigure out where that could be in the design changing sketch planes or anything like that all I'm going to do is come in here and say modify press pull and now I can just grab these faces pull them out we'll just go like a half an inch and that'll just give me a little bit of a lip to create room for a pocket you can repeat that grab this face move it out half an inch and then the same thing over here and now we've got a nice design note that the width and the depth now would be off so the width would be actually one inch longer than we have originally defined if you want you can go back and modify the parameters make a different equation whatever for now I'm just going to leave it now we want to create the cutouts for all of these tabs we're going to do that with a combined feature so with combined I can pick the part that I want to cut the tool is going to be this kick so basically I'm going to use the tabs in the kick to cut the pockets out of this bottom shelf and we're going to say keep tools because we want to keep the part after it's done again repeating that combined let's say we want to cut out the back and the back has pockets for the two shelves tabs so the two shelves are going to cut the back do it again now we're going to cut if we want to cut one of these sides so we're going to cut the side and all the parts that we need to use to cut the side that have tabs that intersected are all of these so say okay can repeat that again cut the right side and again we'll pick all of the parts that are going to cut it and then finally one more time pick the top and we'll cut that with this part this part and this part so now for example if you look at one of these if we were to hide some of these parts you can see now that this sides have all of the pockets cut out now that the models done what I need to do is lay these parts out flat before I do that one thing I like to do is to just quickly create something that's going to represent the stock so if I do that I'll go ahead and pick this plane I'm just going to sketch out a rectangle so I'm creating a box feature and we'll make this 96 by 48 and then for the height we'll give it that value of ply and then we'll say we want to create a new body and what this is going to do is just give me that reference piece to line everything up against now I want to take all of these parts and lay them flat so before I do that right now we've been modeling as bodies and what I want to do is I want to take all of these components bodies and I want to make them into components which is a distinction in fusion so I'm going to select all the bodies from the tree right click create components and now I could come in here and rename them now that we have components what we want to do is we want to create joints I like this just because it makes it really easy to move things around and lay it out in a flat pattern the way you want it's not a totally necessary step but I just think it's pretty quick and easy way to do it so first thing we're gonna do is are going to take this stock right click and say we want to ground it that's going to basically fix that one piece now we're going to come in and create a joint and what we would do is we'll pick the face that we want to line up so that face on the top and then we'll notch that to this face on the stock and we can set the type to be planar and then flip it and now it's essentially lined up with the stock and then what's nice about that is then I can take it and I can just drag it around and it'll stay in that plane so we could get things oriented the way that we want okay now what I like to do is just to make it easier is to just hide the one and then create the joints for all the others so I'm going to hide this from the tree and now we'll go ahead and start creating all of the rest of the joints now that we've applied all the joints we can just drag these things around in the plane one thing that makes that a little easier is you can right click on the stock and make it a slick selectable unselectable if you do that you see the little red cross out circle that means that it's not going to be selectable which makes it easier to just pick all of these parts without that getting in the way and you can just grab all these little the parts up from the bookshelf and drag them around to lay them out on the sheet if you want to do something more if I want to rotate it I can actually the best thing to do is to pick it from the tree that way you have the component selected and then hit right-click and say move and now you can do things like rotate it and you'll notice that it snaps to ninety can still drag it around while you're in this command and then hit OK and maybe the last one I want to do is take this guy and again I'll grab this and say move and we'll go ahead and rotate this one as well and then move it into place and now I've got all the parts laid out flat the way that I want now that we've got this all laid out what I want to do is apply dog-bone fill it's to all of these internal edges so we've got a nice little add-in that somebody wrote Casey Rogers which allows you to create dog-bone fill its and we can either apply this to each edge individually so I could pick all these edges or you can actually just pick the bodies and if you pick a body it's going to find all of the vertical edges that are inside corners and apply it to all the edges another thing we're gonna do here is just put in our parameter of cutter this way if I change my mind about what cutter size I want to use it will adjust the dog bones accordingly and we'll just go ahead and hit OK and this is going to take a couple of minutes to process so just be patient if you're processing like this with a hundred and fifty something edges just be patient and here we can see the result of the dog bone fill it's being applied to all of the internal corners pretty nice ok the last thing I want to do is create a little bit clearance in these pockets for the blind tabs are currently modeled exactly flush so I'm going to do a press pull and then I'm going to pick all of these faces and then we're just going to offset them down just a little bit so you see I can just drag this as much as I want we want to make sure you do a minus point zero for whatever clearance you want but the important thing is to put in the minus sign so you know it's going in that direction okay so now that we've got this all set up the thing that we've got to do is now create toolpaths so I'm going to switch over to the cam module and now we can start creating it so what I want to do is create a new set up so set up a new set up and the first thing we're going to do is define our origin so we want to set the direction of X so I do that by clicking on the back half notice you can pick the back half or the front half of these arrows click the back half of the arrow and give it something to reference just to get the direction oriented and then I'll click the front half to switch it then I can click on this point right here and say I want to align it to the lower left corner of my stock another thing that you should do is select on model this way we're just going to define exactly what parts we're cutting out maybe you have some extra bodies extra parts that reference model of the stock things like that that you don't necessarily need to be computing toolpaths for we just want to do it for this so we've selected our models now we're going to go over to our stock and we're going to give it a specific size so we know that this is 96 by 48 and then the height again this is the other place so you need to change it over in the model on that ply parameter and then here in height we need to set it as well so here we're going to set it to something that we measure so again you want to measure your stock very precisely and then input it here and this is just another small thing you want to say offset from the bottom in minus Z 0 as long as this and your ply parameter were the same it wouldn't matter but it's still good practice I think we've noticed so we'll do that and now we've got kind of the base setup for where is my origin point and how is my stock to find one thing I like to do is to just kind of name the setup with the tool I'm going to use so I know this is going to be for a shop bot and it's going to be a three I'm going to use a 3/8 compression end mill so that's just wait if I'm going to use multiple tools what I'll do is I'll create a setup for each tool and then all the operations for that tool will go into one setup it makes it really easy to post it out in groups and then just run one program at a time on the shopbot I just like to one one program for each tool do the tool chains and run the next program for me that's what's been working really well so now I'm going to go ahead and create first operation the first operation is going to be to create a 2d pocket and we'll do that here so I'm going to create a 2d pocket to cut out all those blind pockets we'll pick a tool in this case I'm not really worried about getting the exact parameters of the tool just because I just wanted to narrow a generic 3/8 cutter because all I'm really worried about for right now on the router is just getting the tool diameter right and then I can set some the spindle speed I can set my feed rate in this case I'm going to use 60 and then I could set the lead-in feed rates as well and it's going to do a little calculation for me and let me know what my feed per tooth or my tooth load is as well which is kind of nice for geometry now what I need to do is pick the exact pockets that I want to cut out so here I'm going to pick these pockets so again all my blind pockets now this happens sometimes you got to remember you got to notice with this arrow is on the outside of the pocket you need to click it and it'll switch the directions basically saying which am I going inside or outside on that edge you just picked and I want to go on the inside so you need to make sure that on all of these pockets that you pick that again happen again you just want to always make sure that you're cutting to the inside of the pocket not the outside and we'll get these last two from this part remember there's six on the on the one and then again I need to flip this when two on this one so the first thing I'm going to do is my blind pockets that I want to completely clear out okay Heights we don't really need to change anything here under passes there's a couple things you definitely want to change um we want to do write conventional milling so climb milling uh more for like a very rigid CNC machine doing high precision metal cutting the other thing we want to do is a step over so if you want you could just step over by the entire tool width or you could cut this down it's up personal preference I believe their stock to leave if we were going to come back and do a finishing operation later we would maybe want to leave a little bit of stock to cut off if we were doing like a 3d contour thing or something in this case we're just profiling out these pockets so we don't need to leave any stock but what we do want to do is take multiple depths so here are going to set the step down to be half the cutter diameter seems to be about the rule of thumb and then also for a finishing step down you don't really need to do an extra finishing pass here so I'll just also set that to be the regular step down that I want and that way we'll just basically just take steps all the way down to the bottom of the pocket in half the cutter diameter and then the last thing is over on linking one thing that I like to do here ramp this is how the how its tools going to enter the material and you can see a nice preview of all these things you can see a nice preview if you just hover over the option you can see what they are what options you have so you can see here pre-drill plunge helix etc so helix is nice if you're trying to enter into a very very hard material like aluminum or something but in this case we're just going into plywood so we'll just do a straight plunge and it just is much faster and what that will say okay and we get a preview of the tool pass so you can see here what the tool is going to do as it goes from pocket pocket so the next thing I want to do is cut all these through pockets and I'm going to do this by using a 2d contour so a 2d contour will come down and just cut the profile so if the cutter was less than half the width of this pocket then you'd actually end up with a little sliver in the middle in which case you might want to use a pocket doesn't really matter you could use a pocket here or a contour really it's going to accomplish the same thing in this case but again I would say 2d 2d contour and I've already got it set up here so you don't have to watch me pick all the pockets but again I using the same cutter set my feeds and speeds under the geometry you can see that I've picked that what you always want to do is just pick one edge on each profile and it will find the profile and then again also make sure that the arrows on the inside of all of these pockets not the outside or else you'll end up with the cutter going around the outer profile so in this case there's 18 of them Heights nothing to change passes same same adjustments that you make here that you made on the previous pocket so I want to definitely say I want to make right conventional milling I want to set the maximum step down to be a half the cutter diameter and same for the finishing and then on linking I just turned off ramp if you want you could ramp in doesn't matter it would be maybe nicer it put a few did a little ramp on the way in you could say you want to come in at an angle and you can see the result there of those pockets so now what I need to do is cut out the actual pieces the outer profile so again I'm going to use a 2d contour to do that by default picking the last tool I use which is good for me here then for the geometry I'm going to pick all the contours so these profiles here should zoom in and make sure that these are going in the right direction so again some of these were on the wrong side and here all good so now I've created all the profiles that I want now on this one I want to do something else a little different I want to add some tabs so we're going to add tabs to keep the parts from flying off once they're fully cut out we can either do rectangular triangular I'm going to do a triangle I'm going to do 3/4 by point 185 so just under my step height and I could either say by distance which would put these every three inches on any side that's at least three inches long or I'm going to say by app points and so in this case what I can do is I can actually come in and I can just specify I'll just pick like say four points on each part that I want where I want to put the tabs at and this way you can kind of specify it yourself so fast forward for a second and then where you can see I've picked all of the places from my tab so all those white dots represent where a tab is going to be and like you just I just placed them so in this case I got 28 for per part underpasses again make sure you set it to write conventional milling and we're going to have set the the depths again some multiple depths going half the cutter and then under linking just really taking the defaults here as well and what that would say okay and now you can see again the blue lines represent a preview of the toolpath and you can kind of zoom in you can see here the tool is going to take that little jump right there the little jog to make the tabs looks pretty good once you've created all the tool paths the nice thing to do is to be able to simulate it so if you select an individual tool path you can simulate just the one or you can select the entire setup folder and press simulate and you can turn on the stock which I like to do and what that's going to do it's going to let you is going to show you actually the mature being removed when you press play it'll show you the material being removed can do things like skip just right to the next operation so done with the pockets and now it's doing the through pockets again this is like nice to just see what's happening I've caught many errors by looking at the simulation realizing the tools going and cutting somewhere that I didn't expect or it's cutting the wrong side or it's not finishing where you thought it was going to be finishing the other thing you can do is just kind of jump to the end so after it's done everything and then you can take a look at what you're going to be left with so here we can get a nice visual on you know where are my tabs are they in the right place do they look good does it look like they're all done is there a big chunk of material left in here that I wasn't expecting all those types of problems that you might find on once your cutting you can find here in the simulation and once you're done simulating same thing again you can either post out an individual operation or you can post out the entire setup which is why I like to do one per material or one per tool and now I'll pick this and I will say post process here I can select either any post processor in this case we have two four shot bought one that will create open SBP file so shop bot language and then regular g code the shopbot iso post and if you want to go in and adjust here in the properties if you have some specific properties that you want to adjust for your specific machine you can change those here in this case I'm going to take the default and export this g code and will overwrite the one that I have say save it off somewhere where I know where it's going to be and then you know if you're not doing this on the machine that you're actually have hooked up to your shop bot then you can then just take that put on USB key or whatever move it over to the machine and load it into the shopbot controller and run the job all right thank you guys so much I really appreciate you taking the time to watch this please leave comments if you have any questions and I'll keep an eye on it and I hope you guys enjoyed this and let me know what you think Thanks

Channel: Patrick Rainsberry

Views: 172,656

Keywords: CNC Router, Numerical Control, shopbot, Fusion 360, Autodesk, CAM, woodworking, CNC, CAD, Flat Pack, Furniture, Design

Id: VZU_Jpyyc5M

Length: 43min 43sec (2623 seconds)

Published: Wed Sep 23 2015

Reddit Comments

[u/skookumasfrig]

As the title says, I'd love to see a tutorial similar to this but for FreeCad. I'm in the process of building a 4x8 Lowrider CNC and I'd like to use it for cutting out bookshelves, cabinets and similar furniture. I only found out about FreeCad a few days ago, and I've ben looking at the tutorials but I haven't seen anything like this.

Any ideas?