Designing Sheet Metal Parts in Fusion 360

today we're going to talk about designing sheet metal parts in fusion 360 so we can generate a flat pattern cut them out on the mill and bend them to shape welcome back to cloud 42 i'm james in a previous video we manufactured this sheet metal bracket shown here in red to mount the remote vfd operator on the new spindle for my grizzly cnc conversion mill and in that video we focused on the process of actually cutting out the bracket on the cnc mill engraving it bending it and installing it on the head but we completely glossed over the process of designing the sheet metal part in the first place and that's what the video today is about we're going to look at the sheet metal tools in fusion 360 and talk about how to actually model a part like this so that we can then unfold it into a flat pattern and cut it out on the mill i think the easiest way to illustrate this is to start with an empty design now when we when we normally are modeling things for 3d printing or for cnc milling i normally work in the design workspace in the solid tab and this is where we you know create sketches and extrude to actually model our solid model that we're going to use to generate stls for 3d printing or code for the cnc mill to mill this out but there's some other tabs here and one of them is the sheet metal tab and if i select this there are tools in here for making sheet metal parts now we're going to start with a sketch i'll go ahead and just create a rectangular sketch here on this plane click finish and now i've got a sketch and i'm going to create my what's called my base flange so everything in the sheet metal workspace is you're usually working with what are called flanges and that's the basic unit of sheet metal part so i will select this sketch i will select this profile and click the flange button to create a flange you can see that's going to create a sheet metal part based on that sketch if we look at what we have here there's some that you can choose which side the sheet metal is pulled out from on the sketch or whether you want it symmetric but the key operation here i'm going to say i want a new component but the key operation here is to choose the sheet metal rule that you want to use and the sheet metal rule has information about the thickness of the material and how it bends and how you want to handle corner relief and other properties of the sheet metal part i'm just going to take the default right now we will come back to that now that we have a base sheet metal part we can add more flanges to it so i can just select an edge and i want to create a bend and a sheet that comes up so i'm going to select that top edge click the flange button and then i can pull a new flange at an angle off of the edge of that part now there are some parameters out here that control how that bend operates so the first thing is the bend position here and i have this set to inside now what that means is let me pull this up so you can see it and get it lined here is as i pull this part i have my initial edge here that i selected and the bend will all occur inside that dimension so the outside surface here of this uh flange that's going up will be in the same plane as the original edge of the sheet metal that i pulled that flange off of you have other options you can also say outside and it will pull the bend outside of that dimension so that now the inside face of the bent flange will be in the same plane as the edge the end of the sheet metal that you pulled this off of and you have some other options like adjacent which will put the entire bend radius outside the end of the of the sheet metal part that you pulled this off of and so you can choose how you want the dimensions controlled here i generally use inside but it really depends on what i'm trying to accomplish in this case i'm going to be designing a part where the flange is going to come out make a turn and i'm going to mount something at the outside and i on the outside of this and i want to control the distance to that so inside is is what i want for that and then you can continue uh messing with this and adding flanges off of other edges before we go any further though let's stop and take a look at the root the sheet metal rules so if i come up here and click on this button i can open the sheet metal rules dialog and this shows me that in this design i'm using the aluminum millimeter rule and then i have a library of other rules and the one i actually want to use here is this aluminum inch rule because i am using inch dimensioned aluminum parts and inside the rule there's a bunch of information about the thickness of the material the k factor which has to do with how it bends miter rip and seam gaps bend conditions uh radius on the bends and other things so since i created a component here i can go into this component and it shows the rule that's being used for that component and i can click here to switch rules and i'm going to come down to my library and i'm going to choose the aluminum inch rule click ok and now i've switched over to use the aluminum inch rule i can come in here and i can edit it so here's aluminum inch click edit and i can change some of these parameters now i know i'm going to be using eighth inch material so i'll enter 0.125 and so that'll change the thickness of the material and you can see after i close that this is now shown thicker i also want to mess around with the bend radius because i'm going to be using a press brake with a sharp corner so i'm not going to be i'm not going to be using a large radius on the bend so bend radius i'm going to say let's say 20 thou yeah that's about how it's going to come out because i've done a little bit of bending and that is a very aggressive bend for metal that thick but i've had good success with it so far and the other thing that i want to look at here is the k factor now k factor has to do with how the sheet metal bends and where the neutral line is so if you take a look at this is a diagram from wikipedia showing how sheet metal bends and this in this case we're bending this sheet metal around a radius and it's illustrated here this thing called the neutral line and what's happening here is as the sheet metal bends the material on the inside of the corner is being compressed and the material on the outside of the corner is being stretched but there is some point within the sheet where it is neither stretched nor compressed and so everything inside of that is compressed everything outside of that is stretched but the neutral line does not change length and the importance of understanding where that is is so that you know how much additional material is going to be consumed by the bend or how much the material is going to stretch and get longer when you bend it so if you want to control the distance from the end of the part to the outside of the bend and then have the end of the flange that's bent up be the correct link length you need to know where that neutral line is and so the k factor indicates where that neutral line lies in the thickness of the material that you're bending now you can look this up in tables and you can actually go make bends and take measurements and figure out for your particular material what this is the default in the rule here is .44 i've done a little bit of testing and on the material that i'm using and the bend conditions under which i'm using it 0.33 is a little bit more accurate i'm not going to go into all the details of that there's lots of material on the web you can read about how to determine the k factor and how to actually take measurements to get that so when i change that nothing changed here in the model because it doesn't change how the shape of the part is modeled it changes how the flat pattern will be generated so uh now that i've got those conditions set up we can go ahead and you know just generate more bends and and mess around with the parts so you can pull flanges off of anywhere you want and fusion will automatically generate relief so in this case if i want to pull this bend and i want to have it inside the dimension i'm going to have to cut some material out of this corner in order to make that bend possible and fusion automatically calculates that and there are some parameters you can use to control exactly how this is done but in general you can just come in here and pull flanges wherever you want with whatever dimensions you need and it will take care of figuring out how to generate the relief assuming that what you're what you're making is something that's actually possible to create okay now that we've got a sheet metal part designed here and this is you know not a particularly useful one i'm just messing around then we can go in and generate a flat pattern and to do that there's just a button up here i can just say create flat pattern click it it wants to know what my stationary surface will be and i'll just pick this one click ok and it will then unfold this part into a flat pattern and on this flat pattern it's actually showing me the uh the the fold locations the bend locations and there's some additional data around this around the extents of the bend and where the actual flat surfaces will be after the bend and so then we can actually generate our cam off of this but i think that's enough messing around with a fictitious part let's actually go over to the design and design the part that we actually want okay i have the model of the spindle and the mount here and i also have a rough model of the operator panel and this is just sort of roughly positioned where i want it you know i can move this around it's not locked into position but it's just sort of roughly there as a guide so let's start with the base flange and we want to mount to these two screws so let's create a sketch here and i will start with a construction line select construction hit l for line and draw it between the two screws so that i can pull the mid point now i'll say create a center rectangle and we'll pull it off of the midpoint there not construction so that it'll be centered over the screws and put some dimensions on it i think i want this to be about two inches high and we'll make it three quarters of an inch wide finish that click here to generate to select the uh the the the profile and then click create flange and that will give us our flange let's make sure the dimensions are right here should be an eighth of an inch thick yep i have the rule set up correctly okay now we want to take that flange we want to extend it over and attach it to the back of this operator panel so i but i have a little bit of a problem here and that is that the spindle is slightly wider than the mount and that's because the spindle is ever so slightly wider than the back plate here so i want to jog out a little bit so i'll click here on that surface create a flange we'll pull this out but we don't need 90 degrees we just need 10 degrees that should be fine 10 degrees great and we only need to jog that out maybe a half inch okay great and then we'll select this inside line and we'll create another flange pull that out and again we only need 10 degrees and let's pull that out to about where the operator is four inches a little bit far 3.5 a little bit more than that three and three quarters okay great so now we've pulled that out to about where the operator is now we have a problem and that is that this is coming over way too low to hit where that is and so we want to actually move that up so what i'm going to do is just create a sketch on here and reshape this so l for line and i'll just draw some lines here on the side and then i want to create a parallel line on the top and that should be fine and now i can do a couple of operations here let me move this out a little bit we'll cut the bottom part here off just by extruding and we'll just extrude through the part that's fine and then we'll take have to turn the sketch back on here take the top portion here extrude distance to object and we'll select that back point and now we have reshaped that flange and the system doesn't care that we just drew on that and sketched it it still thinks it's part of the sheet metal part so let me grab this back corner here create one more flange pull that out an inch yeah that'll be fine to give us a place to screw on the operator in fact we'll just make that three quarters of an inch that should be fine now we'll make it an inch okay now let's round a few of these corners so i'll select this surface that edge and hit f for fill it say quarter inch that's great now let me select the some other places i also want to round so i'm just holding ctrl and clicking some of these other edges and it's applying fillets to those okay that has that reshaped and now we want to actually put some screw holes in this uh but in order to match those up we need to join these hit j for join i'll just pick the center point there and attach that to the center point of the front of this and we need to offset it slightly because the connector is in the way maybe what half an inch nope yeah just a little bit just enough to keep this connector out of the way so that it doesn't hit that okay great now just create a sketch on the inside here make sure we're creating that on the right plane okay create sketch and i will just project the back surface that has those holes so now i have my references for my holes and i will put a couple circles around those set those equal and dimension those up let's make those four millimeter because i know those are m3 screws and that'll give us a little bit of adjustability and then we'll just these through and that will make the hole in our sheet metal part and that is it we now have the bracket modeled and we're ready to manufacture it and in order to manufacture it we just have to create a flat pattern for it so i can click up here create flat pattern once the stationary surface i'll pick that one okay and boom we now have a flat pattern now in the case of the engraving uh that i put on the part when we actually made this uh in the last video you can actually just go ahead right here click create uh click on this surface create a sketch import your graphics and actually do your uh your sketch for your engraving right on the flat pattern and that will be retained as a part of the flat pattern workspace i can just click finish flat pattern and it will take me back to the original design and i can see here that i missed a couple of fillets let's go ahead and put those back in and then once i've actually created a flat pattern it shows up over here in the browser and i can just click the little button here to activate it and there it is you can see it's been updated with the fillets that i just added and i think that's it i think we're now ready to manufacture this okay to actually manufacture this we need to go over to the manufacturer workspace formerly the cam workspace and as soon as we do that you'll note that it pops back to the 3d model but over here in the browser you can see we have a models section and we have the original design the spindle head assembly and then we have the flat pattern design so i can just select the button next to the flat pattern and that will bring that up and we will use the flat pattern then as the basis for the manufacturing operation so we can just go ahead and create a new setup now we do have to select what kind of setup word what kind of operation we're doing and the default when you're working with sheet metal is cutting and cutting is what you would use with a laser cutter or a plasma cutter but i want to change this to milling because i'm going to cut this out on a milling machine if you don't do this then you won't have any of the operations that you're familiar with for actually uh performing the milling operations you won't have the adaptive clearing and the contouring in the other operations you'll have operations appropriate for a laser cutter or for a plasma cutter so i'm going to select milling and then i need to choose orientation and i'm going to if it's because this is at an angle just because of the shape of the part i actually want to flip this over so these lines are horizontal so i'm going to select the x and y axes so the x axis will be this and yeah that's good enough and then for stock i'm going to have a fixed size box in this case uh six inch by three and a half i actually have six by four by six inch pieces of aluminum that i bought as drops from an ebay seller and it is 125 thick and then for the model select what my model is and i'm done so now i have my stock here and then i can go in here and just set up my operations so in this case i'm going to start by contouring it and i'm going to pick that bottom there and we have to pick a tool i'm going to go into my iso 30 aluminum tools pick tool number 15 and set up a contouring operation 12 000 rpm 54 inches a minute and this will generate a contouring operation that will cut out the part now in this particular scenario i don't actually want to enter right there because that will plunge directly into the part i'd prefer to enter on the end so i will edit that operation and over here on linking entry positions and i'll just select an entry position here and now it'll regenerate the tool path entering in that location so that it will come in from the side and not not plunged directly into the sheet metal part and i could add extensions and because the material that i'm using here is actually fairly gummy i probably want to do this in multiple depths but for the purposes of this we won't worry about that and then we can come in and add a boring operation and use a smaller tool in this case a an 8 inch aluminum end mill and we'll just pick all of these holes to bore and then if we actually had a sketch on here for engraving we could then select that and add our sketch operation and then this allows us to generate the g code that will then cut out this sheet metal part and bore out the holes and we'll use the typical super glue machining operation for this so we'll actually use the blue painters tape and super glue to hold this down if you haven't seen the video where i actually cut out engraved and bent this part i will put a card up here in the corner and you can go check that out but as far as actually modeling the parts using the sheet metal tools in fusion 360 and then setting up the cam workspace to actually mill this out on the cnc mill that's really all there is to it i've done a number of parts this way and i've been very happy with the process if you enjoyed this video give me a thumbs up feel free to subscribe to the channel and leave me a comment i'd like to know what you think thank you for watching [Music] you

Channel: Clough42

Views: 11,165

Keywords: Fusion 360, Sheet Metal, CNC, Design, Modeling

Id: t5_Thg1lxGE

Length: 23min 26sec (1406 seconds)

Published: Sat Oct 10 2020