SOLIDWORKS - Sheet Metal 101

hello guys is Steve Darcis with NGO engineer and today I wanted to talk about sheet metal so thanks to Tandy bakes I got a really cool little brake press I can come down and hit I've got a little assembly for this and a lot of times you do want to model up your tooling just so you can see if something's going to work or not work in this case I got to kind of turn my die in order to use it correctly and that's kind of one of the issues is if you don't know how to manufacture the part then you may not design it properly so today we're gonna spend a lot of time on sheet metal parts for the most part for you guys that are new to this sheet metal part is done where the thickness of the material is consistent and you can of course fold it and unfold it but before we do get a little bit too crazy with that let's just start something from scratch so I'm gonna go ahead and start with just a new part file if you guys have just started SolidWorks it may look like this you can just start with the regular part file I have some templates for millimeters and that kind of stuff so I'm gonna start with my part and SolidWorks straight out of box comes with extrudes and all that stuff sketches if you right-click there's some little hidden gems in here I'm gonna go and turn on my sheet metal toolbar now what that's gonna do is it's gonna add another little tab up here and we have now tools for sheet metal now as we start to sketch and create sketches and things some of these things will become more active as we can we can use them now I've got a lot to show you in a little bit of time so let's get started I'm gonna call this guy sheet metal Oh too and we're just gonna start sketching on the front plane and I'm gonna start off with just a simple box start at the origin let's go ahead and make some dimensions so we know about what the size is I want to make this guy eight inches by five inches and instead of going to my features and doing an extrude or revolve I'm gonna go to my sheet metal tools and you'll see the only one that I have available other than this guy we'll talk about him later is the base flange or tab so when I click on this then you'll see it automatically gives it just the thickness of whatever that sheet metal part is and of course I can change it I'll have some other videos and stuff for using gauge tables and stuff for this we're just gonna use K factor and I'm not gonna go too in depth on this you can go to some of our training events too to learn more so I'm just gonna hit OK and we got a consistent thickness now we also have some other little features in the browser tree and I'll get to some of these a little bit later as well but for right now let's go ahead and make a little bend now you can see that I've got a lot of tools specific for sheetmetal that I can start to use so I'm gonna start with the edge flange just pick on the edge pull it up a little bit click your mouse that'll kind of set it and give you a nice little preview on what you want now because I made this guy 8 inches by 5 inches I may want this to go to the inside on the other hand maybe I wanted to go to the outside well we've got a lot of tools and buttons and features in the dialog box to give us exactly what we want in this case I want to go to the outside I want to tell it the flames length is exactly two inches so we can click on that I can also do two edges at the same time now when I do that now I got to just decide on what I want to do in the corner okay I can also put a custom Bend allowance and a custom relief type but for this I'm just gonna leave it the way it is so we'll go and say okay and it creates our flanges that's pretty nice click down two edges typed in two inches hit the ok check box let's go ahead and go with one more so again edge flange pull that to the outside this one I'll make a little bit longer may get three inches and we'll say okay if I want to put holes on there I can I'm just gonna do a sketch on that face just draw some circles I can use the hole wizard if I want let's go ahead and select all of those make them equally spaced or equally same diameter in this case and we'll go to make them half inch now of course I can dimension them to the edges if I want to and from that to the edge of the top I'm just gonna leave them there and the main thing I want to show you is that when we go to just a regular features like an extrude cut I have a little secret little thing here it says link to thickness so if I check that box I don't have to type in what the thickness of the material is it already knows sheet metal so I say okay and there we go got my little part in there now we can also trim some of these little edges if I want so let's go to sheet metal go to corners I just want to do a break corner and I don't even have to zoom in I get just will automatically get any of those sharp corners that are in there and go and put them out of quarter-inch and that's gonna put I can't have the option for Phillips or chamfers on there so that's pretty easy for a simple part simple sheet metal part so now we want to create the drawing for that now before I go to the drawing maybe I want the guy to cut it and do some Rd fold it up see if it's gonna work see if it's gonna fit so to do that you just hit the flatten button it's gonna flatten this guy out it's going to give you an automatic outside extents of the park so you can quickly select on that edge and find out what the length of that is click on this edge here length is right down here in the status and then if I want to I can select it right click and go ahead and say export to DXF for DWG file so you give it a name this case I'll make a DXF you can put the output alignment on where you want the origin at in the X and y direction that looks good to me make sure you select on sheet metal sometimes people will actually etch the binned lines and if you do that then you're also going to want the bin lines in there so I'm gonna go ahead and select on those it'll put them on a separate layer for a DWG DXF so they can actually turn that off and they're CNC software as well so there's a preview of what it looks like hit the Save button and I'm done I've got a DXF for a DWG whichever one you select and it's out there now if I want to create a drawing it's just as easy so I'll hop out of my flattened State go ahead and make a drawing from the parter assembly I'll just pick on abbé sieyès landscape once this comes up I'll have all my different views so if I want the folded then I'll just drag that out automatically go into projective View mode we can do that shade that make it look pretty we could get all our dimensions I'm gonna go right to sheet number two and in here you'll see that I also have the flat pattern I'll just drag and drop that in any bin lines that are on there automatically be on there if you have a whole bunch of bin lines we have tables for that so you just say you do a bin table select on the view I have to tell it I'll just hit OK plop that out there and now each of these are a B and C we can go to the table to actually see what that thing looks like pretty simple so again I could put the dimensions on we have other training videos for that so we're gonna get right back into sheetmetal so next I want to show you different ways in which we can create sheet metal parts so I'm gonna start off with this guy right here and in this case all I did was a took a sketch a rectangle extruded it and when I extruded it I checked the little box for draft we put 10 degrees of draft on there and we've got that part so what do we do with this guy well you can see as we got a solid model I've got a couple extra little buttons up here so I'm gonna say convert to sheet metal I usually select on the the face that I want to that's gonna be flat the one that I'm going to bend around so I'm gonna pick on that notice that the offset is going in the wrong direction so I'm gonna reverse the thickness so it goes into the part it's a little bit harder to see then I want to tell it what the bent edges are so I'm gonna select on the edge and then it's got to put a little bend radius in there and follow that on down I'm gonna pick on all of the tops of these I'm a designer and I like to make it very difficult for the manufacturing guy so this is gonna be pretty rough now in the inside it also has to rip the edges so we have a default gap that we can put in there and everything looks pretty good just gonna go and say okay I'll go and turn off I probably should have set this turn off the solid body and there's my part so pretty crazy little part I'll have to maybe get some specific tooling for that I can flatten it out flatten it back up but let's keep on modeling from this point forward maybe I've got some outside flanges that I want in there so again we can do edge flange problem with this one is notice it's going 90 degrees up off the top so a nice little trick is to come in here instead of putting an angle in selecting the little box pick on a flat face and it's gonna automatically make this parallel to that and it puts the right angle in there so in case I says a parallel face so then we could tell it how far these are so maybe they're one and half inches want to make sure it's flat on the bottom looks good so I'll say okay so pretty easy let's go and do one more little fun thing we'll do a sketch I'm gonna go and create a slot let's do a centered slot just kind of put this guy out here I want to put it a mention from the top of this let's make that half and then I'm gonna do something a little sneaky I'm gonna go from let me hit escape I'm gonna go from this edge hold down shift pick on that little edge and I want to keep this about a half inch away from the the sidewall of that thing a couple other little things I want to make sure that it stays centered so I'm just going to draw a construction line make sure that guy is vertical that's good and if you drag this stuff around you can see what's constrains what's not constrained so all I really need to do next is to give us a radius I'll go ahead and say 0.25 looks good and I'm going to cut it straight cut check the little box link into the thickness and now we've got a little cut of a slot in there now I want a bunch of these coming on down so I'm gonna do a linear pattern the direction here let me go ahead and select on my future and when I do that'll pop up my dimensions so the direction here I'm actually gonna select on this dimension for the direction so it's gonna be normal to that edge line there so it's gonna come straight on down there let's go input of these about a half-inch nope that's too small so a little bit more there we go give it a little bit of an edge there and then I've checked the little box down here for very sketch now if I don't vary the sketch it's just gonna go straight down of course I can flip that but if I have very sketch then you can see it's keeping this consistent half inch width across there so we can say okay looks pretty cool I want that on the other side it's good to take advantage of symmetry so I'm gonna mirror just pick on that and there we go got it on both sides so cool thing is you can make this stuff up pretty quick you can go to the sheet metal tab hit the flatten button then we can export this to a DWG DXF make drawings of it whatever we want to do from there so some fun little modeling practices for that guy let's just keep going so this one is going to be very similar to that a little bit different I've got a couple little parts in this case I use the loft at the very beginning but I just did two rectangles okay then I did a little extrude on the top did a little cut give it a little opening where we can put some material in and then a little boss on the bottom so I can funnel this stuff into into something so I call it a hopper in this case we'll do again convert to sheet metal I'll start with this little side flange and then we can come all the way down inside here I can also bend this up on this side and then also come down this side and the good thing about this is I get a consistent rip on that little edge so if I'm gonna weld this up I know I'm gonna weld that up makes it pretty easy on this one I do want to keep the body cuz I also need another sheet metal part for the backside of this thing so go and hit the keep body button I'll go and say okay and we'll do it again convert a sheet metal this time kind of same thing I'm gonna start on this side make sure it's going to the inside looks good we'll select on our bins looks pretty good and we'll say okay a kind of same thing on this one if you want to turn off the solid body you'd also if you're doing a bill of material with weld nuts cuts list you'd want to exclude that guy or delete him get him out of there I'm just gonna hide him for now so you can kind of see I've got a nice little hopper everything's gonna stay to the inside you can also flip it to the outside if you want to make sure that you're a consistent amount of volume on there and of course this one has to sheet metal components in the same part so it's a multi body part in this case select on the face that you want to flatten and then it will automatically turn that one off in flatten it okay so again following to flatten this guy click on him and hit flatten I'm just gonna flying him out so pretty cool then I can make my drawings of this another way to make drawings is of course to use the use of configurations and we'll get to that guy in just a bit so another fun way to make some sheet metal parts really quick to keep on going so let's go to process plan occasionally you may want to indicate to the manufacturing guy exactly how to unfold or fold this and so of course I can hit the flatten button or the unflattering button but maybe he's supposed to bend one before he bends the other because we have tooling for a left side or right side or something a little bit different okay so in this case we will use configurations and really that's what's happening in the background is that this flat pattern I'm going expand him out what happens is when I hit the flatten button up here at the top what it does is unsuppressed these features so each of these little flattened bins that it puts in here it can actually be suppressed or unsuppressed so I can make a configuration one that's folded one that's a flat pattern and then if I want to add to this which is a right click just say add configuration I'll just call it step one and then we can go to the configuration or the feature manager tree under the flat pattern and I want to find the bin that I want to do first and I'll Unser press it so maybe that's the one I want to do first okay then we can make another step and it's gonna copy this guy step two this guy is already suppressed so make someone have been this one up again I try and make it hard for the manufacturing guy it's gonna drive me a little crazy so let me put my little space in there there you go let's make another one step three and hopefully you get the point we're just suppressing a ton suppressing features so there's that and then of course the last one is the whole thing fold it up so that's the fourth one so once we have configurations for this then the cool thing is let me go ahead and save that real quick is to make a drawing so make a drawing this guy again just use be size landscape landscape and I'm just gonna put an isometric in so this is the folded now before I do this notice that this is the configuration that we're using so there's folding I'm gonna go and put a note in here make sure that the view is active and I'm very lazy I don't like to type a bunch of stuff so I'm gonna go link this guy to a property it's the model that this is linked to current drawing view and the property name we're gonna get the SW configuration name so notice it's automatically grabbing folded there say okay let me go ahead and I'm gonna shade this I like shaded views go and put him way over here because that's our end result so I'm gonna select on this guy do a ctrl C for copy pick inside the drawing view and do a control V for paste put him somewhere pick again control V so I have a step 1 step 2 step 3 and of course if we select on the view change this to maybe this needs to be flat pattern so we'll start with that and notice it changes the view note as well so this one be step 1 let's go right here it's gonna be step 2 and I'm your paste one more step three and then of course the last one is my folded view so this is a really quick and easy way in which we can use configurations to show exactly a step-by-step process plan of how to fold up a sheet middle part so hopefully you can use that to create some really good quick drawings pretty easy alright let's get to the next one so let's do some gussets and louvers I've already showed you some edge flanges so this is pretty simple when we have some tooling it's really good to be able to take that tooling and save it into a this is a design library so in this case I have my forming tools folder underneath there I can go to louvers and this tool we can just kind of drag and drop this thing in we can flip it if we want 90 degrees this works a lot like the whole wizard in which we tell it what the type is first and then we position it so maybe I want these guys in there and then we just hit the green check and it puts some louvers in there now we can also on the sheetmetal toolbar do some some gussets and I always oh there it is sheet metal gusset so we'll select on that guy he's always hiding from me so I select on the two faces you'll notice it's putting a little gusset in there and this is usually a secondary operation so we've already made our bend we've made another Bend and this is actually forming the material around us so it's it's and that's kind of same thing with these guys too so we have a lot of tools and buttons for doing the width putting draft on it I'm just going to go and accept it so you see what it looks like and kind of what happens is these are secondary again secondary processes so when we flatten this guy out you may or may not want to see what these things look like and so we do have some tools if you go to your sheet metal document parameters here you can see what do you want on the flat pattern do want to show that the tool form or do you want to just so the the flatter or do you want the tool centers you know we have a lot of options for what you want to see on that thing so pretty cool stuff usually things that you don't think you can flatten you can let's go and do one more there's a cool little emboss gonna drag that guy on there and I'll just hit the okay checkbox so any type of embossed features we can we can do those as well and again put that tooling into a library so you can just simply drag-and-drop we fully support configurations so if you wanted to picks different sizes of embosses or louvers then we can we can do that so keep them in a centralized library keeps them fast couple more this is a really good tool and it kind of depends on your process on how you want to do something say for instance I need a circle going into the bend of this thing well we've been playing for the most part with flatten but there's two other little options for unfold and fold so the way this works is I need to temporarily unfold this so I pick on my fixed face I want to unfold this bend and this bend say okay and it temporarily flattens this guy out so now what it allows me to do is I want to create a sketch just draw a little circle here looks good then from here I want to do a cut we also do have the cut on the sheet metal toolbar so extrude cut link to thickness say okay and there that looks pretty good and then so this is if I actually want to cut it with a pure circle and then I'm gonna bend it bend it back and when I bend it I need to fold it back so I'm gonna use the fold command I can select on the individual bends or I guess I collect all the bins it's gonna grab all those say okay it folds them back up so that's kind of the cool thing is usually you can't unfold that you have to do an incorrect process but in this case we can temporarily do it make cut and go to town now this gives me a little weird cut now some people will say okay well I want to put a pipe in there well that's not really circular so how do we make something circular so I'm gonna play with some planes real quick I'm put a plane right here on this face and then I'm gonna select on the edge and I want this to be at 45 degrees let me flip that so that looks pretty good if I want to create a plane off of that and this one let's just do five millimeters I just want to get it kind of off of that little edge there so say okay well hide our first one hit the little eyeball there and we'll do a new sketch on that one so this is in the case I want to put a circle I got a piece of pipe let's go in to mention it for fun sixteen millimeters we can also dimension from edges if we want good enough and I wanted them pretty much in the center there alright so in this case when I extrude cut I can't really do linked to thickness there right I've got to go actually through the park now that this is a something that's only in 2018 so let me not link it to the thickness there and now I should be able to drag this on down so I'm gonna make sure it goes all the way through the part looks good and that will give me a pure circle so if I want to weld a pipe into this little corner here and this is pretty much the way to do it all right the other checkbox that I have here again this is for 2018 is optimized geometry so I'm gonna hit the okay checkbox and what it's gonna do I'm gonna hide my plane temporarily is that I'm gonna use that same sketch and do a quick extrude just so you can kind of see what's going on here so let me drag that on through so again I got a pipe that's going through here and look at the way that it cut this cut this on the side correctly and then it's also normal to this face you kind of see it that pipe can fit through there and it's giving me the cut to the outside same thing down here it's actually flipping its going down and it's the cut to the outside on the bottom side normal to this face so that's a pretty crazy little cut that it has to do and of course it's easy to do in SolidWorks we just got to check the box alright so it's good and got our sketch got him turned off and again if I want a circle that's the way I want to do it if I want to unbend it put a circle through there and then bend it back up then I can do it in that procedure so too quick and easy ways in which we can create circles across bends let's keep moving so let's do a swept flange on this one it's a little tricky sheetmetal toolbar this didn't come straight out of the box I'll show you how to customize this in just a bit but in this case I have two sketches I have this little weird zig zaggy guy with the three lines and then I have another sketch and just did a line arc a line arc no line alright so let's go have some fun with this do you swept flange pick on the profile that guy pick on the path that guy I okay I'm gonna do a K factor so that's good I think everything else looks alright and we do want to tell what the thickness is in this case I'm just gonna use one millimeter and the bend radius is always the inside of the bend so in this case it's a 1 millimeters to the inside on this guy it's going 1 millimeters to the inside on that so it looks pretty good we'll go ahead and say ok so not something you typically this is kind of also a two-step process is you first you're gonna have the extruded part and then you're gonna bend this thing around a mandrel you're gonna have a lot of thinning and stuff that's happening here but we can flatten this guy out and when we flatten them we not only get our Bend lines for the original extruded shape but then we also get them for this formed part of the shape as well so pretty crazy if you're doing ducting or something like that this is a really good tool for doing that so swept flange get a little crazier let's go to a cone this one is I'm going a little old-school so some of you old guys you kind of like this process I just did a circle extruded it up with some draft did the shell command and then I did a little cut extrude so I used a little sketch and the sketch is I did it normal to the outside of this thing so if I pick on this inside on the top or the bottom it's still normal I got a 90 degree cut on that guy right there okay so pretty simple that way I've got this cut if I got it cut then I can unfold it let's go ahead and update that let's go to sheet metal in this case we're gonna use this thing called insert bins this is what we used to use all the time this one I'm just gonna select on the inside edge there everything looks pretty good let me make sure that I have everything set I'm go ahead and say okay and with that we get this old-school method of flatten bins and process bins and this is where a lot of the configurations for suppressing your run suppressing can come and play but I can also use again flatten and then flatten so that's kind of the cool thing is when this guy flattens out there he is I can also use some some crazy things if I want to say unfold you know try and select on that little edge the bin son fold is gonna be that say okay we can do a little sketch create some circles that's good enough go and cut it link it thickness again so it only goes through that and then we can pull the bins back up so we'll go say fold just say collect all bins and then it folds it back up so anyway some kind of cool ways in which we can flatten this guy out and then flatten them this is a new one for 2018 so you guys I don't have 2018 sorry about that upgrade you'll get this one this is called tab and slot what it does is it makes it really easy to where I can select on an edge when I do I need to pick on the the bottom face that it's going to end at and then what it's gonna do is put some little tabs in there it's gonna automatically connect it this for multi body parts this also works in assemblies with multiple sheet metal components if they're mated together so it puts the little tab in there on one side and then not only that but it also puts the cut in there on on the inside of the sink so I'll go and say okay you know kind of see what it does there's my little tab I've added the little chamfer is in there and if we zoom in there really good you see that I have a little offset all the way around this thing so in this case I think I set it to a half a millimeter so reason why we use these a lot of times is that allows the guy to put it in put position it in this case would be hard to get an actual drawing and put that on there but if I put some tabs and some slots in there now the guy can go in there and you can just weld this guy up and he's it's stuck in place so tab and slot is pretty easy it's just one feature you go in and edit that guy and create these things all day long all right this one's a little bit tricky this was guy said that you couldn't do it so I tried to prove them wrong this is pretty much done with configurations and you can do some pretty crazy stuff to where this is the bent up model takes it a second region there we go and you can see I've also got some little lofted components in here so some pretty crazy looking stuff but for the most part we've got the flat pattern this one was done a little bit different I actually started out with the flat sheet metal part the sheet metal also had let me get to that sketch of some of the bin lines and stuff on there so in this case what I did is a sketched Bend so I just created a line and then bent it up along that line and you'll kind of see that this is pretty crazy comes in like that I have to kind of bend it again on the back side bend it up over over so I got a bunch of little crazy bends in there then almost 180 degree there bends it up just a little bit I've got a little bit of an angle there a little bit of an angle there cuz that's where these big bins come in there's three of them so it's kind of pulled up on that edge and again depending on what the tooling you have will depend on you know what this thing is actually gonna look like alright then I had to actually model in these little slots and so I kind of faked it on these how to actually do some cuttings a little bit of surface work and then once I created them then model them up and that's what I get and that's what the sheet metal part actually looks like when when we're completely done some pretty crazy stuff so main thing we can pretty much model up anything and we can almost pretty much flatten anything all right one more some more food for thought now this I've showed you everything is in SolidWorks standard so everybody has that this tool came in we used to sell for about a five thousand dollar package and I'm gonna go and search for it so you can kind of see how this works it's called surface flatten I'm just going to drag and drop it on there this is only for people to have SolidWorks premium so if you have SolidWorks standard Salt Works professional you're not gonna have this button and for the most part what it does is take surfaces so we're gonna select on the surfaces that we want to flatten out so in this case I got some weird lofted shapes and stuff like that so if you haven't unfold stickers or something then this works out pretty good you do have to select a point that we're going to unfold about so I'm click on this little point here and then what it's going to do is is going to put a whole bunch of little lines across the surfaces and then it's gonna flatten out those lines to where I have a completely flat shape now the thing is when you do that when you flatten this guy out and again he is flat so we can export that to a DXF for an e WG if we want to but something you may want to look at let me right click on that again is look at the deformation plot whenever I'm expanding this thing or contracting it you'll actually see little areas where I'm stretching it or compressing this thing and occasionally you may want to put little lines in there or little cuts in there to kind of help smooth that out or put little holes in there and so you can kind of see where the the maximum amount of stretch or compression is and and make your recommendations off of that so that's pretty cool because we can I'm gonna say almost flatten anything so fabric garments things like that you mod them up you can fly them out but you do have to use solver Premium so I wanted to do this pretty quick wanted to give you some good little heads-up on simple parts it's a very complex parts with sheet metal in SolidWorks so I'm Steve Darcis thanks for watching and use go engineer thanks

Channel: GoEngineer

Views: 76,905

Keywords: goengineer, engineering, MCAD, mechanical engineering, product design, product development, solidworks, part, sheet, metal, thickness, flatten, convert, process, plan, configurations, gusset, louvre, unfold, swept, edge, flange, cone, unroll, tab, and, slot, flat, pattern, folded, surface

Id: LjAiCMOqrLE

Length: 36min 3sec (2163 seconds)

Published: Thu Jul 05 2018