SOLIDWORKS Tutorial - 'Advanced' Sheet Metal

[Music] so we're talking about Advanced sheet metal today um the event or the agenda I want to go through on this though is kind of an interesting way to approach Advanced um the word advanced in CAD terms people always think complex or when it comes to a shape a very organic shape and when it comes to sheet metal Sheet Metal By Nature is actually advanced in just what it's doing so I want to talk a little bit about what's under the hood a bit and then some ways to set your system up in an advanced way that's going to help you quite a bit things that people should be doing but often don't do frankly we'll do a little bit about Advanced shapes because that's always necessary and the features that are used to control those and we'll talk a little bit about flattening because that is the Magic Bullet of sheet metal is it it really is a different type of geometry and style Works than other things because it has a life in a flat pattern as well as a folded and then very many configurations in between so again it's a very unique type of thing so really what is sheet metal now sheet metal is one of those terms that we use but the fact is it really just defines thin materials we can use it for a lot of different things people with corrugated cardboard use it it's all about how you calculate the bends and of course metal is going to fold and bend where corrugated corrugated cardboard technically collapses in on itself in a Bend but if you use the proper calculations we can go ahead and get a nice flat pattern that's going to be quite accurate what's really happening though is that we're mapping cylinders to a plane so when we talk about sheet metal we're really talking about for the most part is linear bends that's always been the traditional thing so we're talking about things like this box here where things fold over and flaps collapse on themselves and there's tabs and other types of features but we're really taking these bends here and just mapping them to a flat pattern the common features that are typically used will make a part like you'd see here a lot of bracketry and enclosures and the things that you're seeing on the floor and on the wall here um I think fog filler uses some sheet metal but I'm not well it's pretty obvious what kind of sheet metal you're using here now sheet metal again is a couple of different things when we talk about it fold unfold is traditionally what the cat approach is and these are the kind of features that you'd end up creating here so flanges and hems and and you know in this particular case we're just using a lot of corner breaks but it's a lot of very repetitive stuff when it comes down to it base flanges are pretty common again these types of brackets are the things that you would use quite often but the calculations that we're using to create these parts are the difference between an okay part with pretty loose tolerances versus an ultra accurate part which some people do go for in these scenarios as well so let's get into the first part about this what's so Advanced about what I just showed you well the reality is is what's happening here is some pretty funky stuff under the hood and to really make your sheet metal Parts accurate it's really embarrassed to understand this a little bit better so when we're talking about the way that we calculate these things the K factor is generally what we're talking about but there's two other areas called bend allowance and bend deduction that are used to calculate how we determine the difference between a folded versus a flat I'm sorry I'm doing hand puppets up here but folded versus flat versions of a part because the reality is is when you go ahead and apply these types of calculations you can change this based on just again tweaking these numbers and your part will be different in a linear Bend when it's folded versus its flat pattern it could end up being longer in the flat versus shorter in the flat depending on whether there's tension or compression as the primary component inside of your bends so when we're talking about these types of things we're talking about trying to get your Machinery predictable and your parts coming on the end of the Machinery again in a predictable size and and the point of this is that I'll show you how these calculations work but there's a lot of examples that come with the style work software that are just examples for example we don't provide you with an accurate Bend to use for your parts we give you an example Ben table and the reason is is generally is because it's based on how people process things so when we're creating what I'm about to show you here when it comes to these band tables and K factors a lot of times there's a little trial and error in the beginning to where you take a known part and build it in 3D measure it in 2D and then use that to kind of reverse engineer what your calculation or your K factor is based on how your Machinery Works how your press brakes work or if you have CNC tools there's a lot of variability when it comes to sheet metal and a lot of looseness when it comes to the tolerances typically as well so the K Factor this is generally a number that is put in as you create sheet metal and it again determines whether the part is the same linear length flat as it would be folded measured on the mid plane versus longer or shorter again with tension and compression in each of those Corners now this is some Voodoo here that the graphics that you're seeing here this is just miss hours help file so you can find these these particular Graphics here but it has to do a little bit with the inside radius the actual arc angle itself and then this thickness value here happens to be the distance the mid plane is from the inside of the part so what we're really talking about on something like that is the neutral plane that's used to calculate this so no matter how thick your sheet metal part is it really is an infinitely small surface that is being calculated to fold and unfold at it's where this neutral plane happens to be the default is always 0.5 which is right in the center of the part and what that tells you is that it will be a one-to-one ratio measure your part through the center here will be exactly the same length as if you unfold it and measure one long Edge so that was where 0.5 comes in [Music] I'm not sure what that means okay exactly what it means good so we're really talking about this neutral plane I'd say 98 of the people we deal with just plug in a k Factor now this is where things kind of get interesting because when you're talking about a k factor of 0.5 you're basically talking about a mid plane right down the center of the part as we would see here but what happens when your part isn't a u-shape and it's an S shape and you start to change where that K factor is more inward or more outward so what I'm getting at is that if I do a k factor of Zero versus a k factor of 0.5 that actually makes the neutral axis the inside face of the part okay so on an inside of a bend the length is actually going to be much shorter because it will essentially as it unfolds it as it will compress this outside Bend so that it actually flattens and has some in real life some some wrinkling some oil canning some other sort of bunching in those corners now I'm going to pull up this part here for a second because what I really want to do is kind of just show you a little overlay that actually shows how this thing is calculated so back in Saladworks here for a second if I could we're going to go ahead and pull up these two parts I just want to illustrate this with a little bit of a sketch overlay that we've got here so when we're talking about calculation I want to look at the u-shaped part here first just as my example here when we're talking about a k factor of 0.5 what we're really talking about on something like this is a sketch that is essentially right through the center of the part now if that K Factor moves towards the middle what you're talking about now again is calculating the length of the part based on where this plane is so in this scenario the part flat will be shorter than the part that is folded up now if the K Factor again is 0.5 you're talking about a one to one ratio it'll be exactly the same flat as it is folded and then again to the outside now you're talking about some compression on the inside and some tension on the outside but it's a different ratio to those now what I was concerned with initially when I talked about K Factor being set to the inside for example is when you're talking about the inside bends here it concerned me when we got to a part that was s-shaped and the reality of it is is the software knows enough to know that it's going to calculate the inside of a Bend regardless of what direction that bend goes so in other words the straight sections here are going to be calculated as straight but if we had this K Factor set to 0.1 it would be inward on this Bend and inward on this Bend so effectively the sketches that you see here is what actually gets measured so I was concerned once upon a time that it would actually do a line on the inside and then as it went around this direction it would also be on that predominantly right side versus left side of the part so over here so when you set your K factors the basics again once again is that if you go ahead and start unfolding your part it will change that length relative to the folded version of it but it's all based again on processing equipment so a little trial and error we'll go ahead and nail that to get the accuracy of your processing when Bend calculations are upped a bit there's more factors here but again at least a little bit more Ultra accuracy we start to calculate things using the bend allowance or the bend deduction now what it comes down to as a k Factor that's the number we're still going to find but it comes down to a k factor that is so granular that based on the radius of an edge the thickness of the material and set angle it will be a different cave factor that it gets used to calculate each individual Bend of apart so if you had a super complex part that had 50 bends and there were different radiuses and all different angles theoretically each one of those bends will be calculated with a different K factor using a table like this because it would find everything that's at 16th and everything that was a thickness of the part that was whatever the thickness is it would take those K factors and essentially I'm sorry I'm scrolling through um is it would essentially go ahead and roll those K factors based on the different radii that are there and when you're talking about forming equipment or press brakes you're talking about very you know tight wedges versus very loose and round and that's again a difference in tension and compression but these are where companies up things when they want to get that Ultra precise thing you're not just using one number of a k Factor you're using an individual unique number for every Nuance within the part and those again get incredibly granular now as I mentioned before um these are things that we provide with the software as an example and I'll show you where that is because the gauge table is another thing that we also provide as an example and they both kind of live in the same spot um gauge tables are something that I would implore everybody to use Bend tables again that's based on the accuracy that you need a lot of people make sheet metal Parts with larger holes or with slotted features so that they do have that variability on fit up but what a gauge table actually does for you is it changes your SolidWorks interface and it only allows you to select these particular values as thickness of material so you go ahead and fill this out the material you keep on hand the radii which would be the tools that you have available to you and that's so somebody who's designing a sheet metal part isn't just keying in numbers out of the blue right you've got to make custom tools to be able to go ahead and make custom radii but if you use a gauge table like this what you're basically doing is changing the SolidWorks interface so that pull down menus appear and users can only choose the gauges that you've determined now I'm going to go backwards one on this for a second because um I've got a little hyperlink here that takes you to where this is now your your install directory is going to be different than where mine is so mine happens to be and frankly I've been doing this for a long time on this laptop so the gauge tables I'm referencing are actually a sours 2019 folder even though I'm on sellers 2022 right now but what it will do is it will take you to your cellworks install directory which is generally program files SolidWorks a localized version potentially or Saladworks Corp will be yours and then we end up getting into give me one second here and then we get into language and English because everything is going to be localized so when you get under your sheet metal gauge tables here and this will be what your full path actually looks like what you're looking at is just Excel spreadsheets and any of these gauge tables again can simply be double clicked go ahead and open it up make changes to it and then just save it as any old name and these are something that we can point to when we're actually again defining um some sheet metal features here so at this point I'm looking at a gauge table where I would only be able to select thicknesses once again that are on hand those gauges are just corresponding to a number so if you don't know the millimeters or inches number of a gauge then you just go by that General value but then the pull down menus for the radius are actually going to roll based on what the selection of the gauge happens to be and it will again only select those types of radii for input not just any number Under the Sun so those things are incredibly important when it comes to the consistency of how people design things again based on what you can do manufacturing wise so once I get some other parts up here I'll go ahead and pull up where the gauge tables are and you can see exactly how the interface does change as a result of that okay an advanced feature that you should be using if you don't is called the design library in this particular case design libraries for a lot of areas in SolidWorks but for this one it's called our forming tools now the design library is pretty important because it allows you to have repeatable things for stamping tools that you would have in a turret punch for example many companies will process sheet metal by putting it in a turret punch in a deep or nips off a bunch of things with straight features takes coining operations punches out tons of holes or even stamps in things like louvers and embossments and those types of things and these types of stamping die features are something that you can create for yourself the beauty of them is that they represent the male half of the stamping die but you can drop it on any thickness of sheet metal material and as long as the radius that's in the part matches or will work for the thickness of material you're using then things will function properly so in other words if I have a very small stamping tool and I'm putting it on half inch sheet metal it's probably not going to work because I don't have enough radii to stamp that out and we have had customers that have half inch Sheet Metal by the way and up to one inch actually in military applications so it's pretty impressive to see that but the process of it is um is something that is very open-ended for the individual user and what I mean by that is you can create your own very very simply and we implore you to do that because we want you to have whatever tools you'd have on hand in a typical manufacturing operation now what these things do for us really simply is again provide repeatability to the stuff we use all the time when you're in a sheet metal part and SolidWorks it's the library books over here on the right hand side so you basically just go ahead and tap that little set of library books and it's got all kinds of other things in the style Works default directory as examples which is a great thing to use once again this is going to be based on one of your style Works install directories mine still might be yeah point to 2019 but it gives you a bunch of examples of little assemblies features that you can drag onto your part like keyways and Slots again anything can be modified and used for your own purposes but then there's also these forming tools now what's interesting about what you see here first of all is you can see obviously the folder looks a little different for each of those the only difference between a folder with forming Tools in it and a folder with parts in it is that somebody right clicked on it and actually triggered this little thing called IMA forming tools folder same as the one with assemblies because if you see this one right here I right click on it you'll see there's a check mark right there because the reality is is the things that are consuming this particular folder if you were to open them up by a little right click these are no more than part files they're just a part file but it has to know when you're dragging it in that you're not dragging a part file into another part file or an assembly you're actually dragging in a sheet metal forming tool so what we have here is nothing more than a regular part file that was built up in a particular way and I'll show you one of these in another way here this is one from the training files that we've got but this enables us to go ahead and take this little forming tool and have something that I can very very easily just go ahead and drag out onto my part so these forming tools are wonderful because as I go ahead and grab them and drag them in place you get a wonderful preview of what it looks like on whatever face you're putting it on the tab key allows you to go either inward or outward with the preview and once you place that feature it's a lot like a whole wizard component where even in this case I can flip the tool if I want to but if I need more than one there's a positions button up here at the top that'll enable me to go ahead and add additional points you can either do this ahead of time or after the fact but it just allows you to go ahead and put these in quite quickly and they actually create an embossed or in an indented feature in the part now not only that but it also removes a little bit of this little face on the inside now the way that I just created the one that I showed you right there was basically an automatic function within the software you build up a feature that just has to represent what you want to be the side that's removed so what you basically see here on the screen again is just a basic series of an extrusion another Extrusion and this feature down here on the bottom by the way is only so we can get that fillet to go outward if that wasn't there of course the fill it would go around the other direction and then in this case I put a fillet on the top and a little feature here for a split line that split line allows us to designate an area to actually get removed so what you do is you go to your sheet metal tools here it's a little button up here called forming tool now it walks you through the process and actually couldn't be even couldn't be any simpler it's asking you for a little feature here called a stop face excuse me a second I'm not sure if I can actually hit that one since I've already got a form tool built into this one let's kill that you see the colors that are there they're done by the way that you select things so when you start with a forming tool it's asking for two things a stop face which is when you stamp it where does it stop when it hits the part so what that designates really is this face the rest of this would be part of the embossed feature um faces to remove we'll simply dictate something that's going to go away so if you do have some sort of on the real stamping die some sort of cutting feature or Edge that'll dictate where something gets removed so you just select that now when you do that it's going to give you a nice little color-coded feature anything that's yellow will be embossed anything that's the Blue Area there that's the stop face so that's going to stay out of the part and anything that's red there actually gets removed so there's a lot of different ways to do that and you know I actually had a different file set up to even show you how to do this oddly enough um but that's really the process that it takes to go ahead and make any one of those your own I'm gonna try and find my own one here there we go so same kind of thing I was talking about and again build it any way that you want to but the main thing is is the radii that are sitting in here have to work for the thickness of the material that you actually put in there so when you do go ahead and run through that basic process here I'm going to take a little longer on this one because I want you to see what this looks like but I'm going to use a removal feature here where I actually select a series of faces now because of the geometry that I've created here my right click select tangency doesn't seem to be there so if anybody's asking in your head why Garen isn't doing that it's because it doesn't happen to be there but based on this it's really worth the work that I'm about to do because essentially all these spaces that I'm selecting on the inside are going to be the stuff that gets ignored or removed now geometrically what's interesting about this is that the part you're looking at doesn't really have the geometry that would be necessary for that cut there would be a protrusion that would have kind of a knife edge to it and it would actually slice these areas out but as far as this feature is concerned it just has to be designated in this red 255 green blue zero color in order for this to actually work now once this is done like this what you're basically doing is just dropping it onto the other component and for this particular one here we're just going to go ahead and drop that into a particular spot and it will give us this embossment so the beauty once again is you can make anything that you want here oh shoot give me a second here sorry pilot here I'm using two different ones there we go um when you're dragging this thing out what you'll get is that beautiful preview once again so as you drop this onto a face the tab key allows you to go inverter outward and once that's in place really it's just a matter of either dimensioning this feature if you need to sketches will allow you to go ahead and dimension that with the position tool or you can go ahead and add additional ones through again clicking additional points but placing that is no more than just dimensioning sketches the result of it all gives you this wonderful embossment once again it's going to go ahead and take the thickness and it will take the radii and roll those up as if this forming tool that we had sits right on the inside of this cavity so again whatever that thickness is it grows independently outward from whatever the form tool happens to be so put those in your library and it's basically work on it once get it done and from there it's all just drag and drop pattern features mirror features all of those do support this type of tool so drop one in pattern it at will mirror it to the opposite side and keep rocking any questions on that one yeah one end do they maintain their parameters that's actually a fantastic question um I did not mention that and I meant to mention that so appreciate that there is an option with that like with everything in SolidWorks I've been doing this a long time and I'm a demo guy so there are some things that are very very much demo-y and other things that are reality one of the awesome things about style works of course is that if you change a part it changes everywhere it was used one of the horrifying things about SolidWorks is that if you change a part it changes everywhere it was used and that's where data management comes in because that can throttle that process but when I drop this form feature in you will notice not only here but in a lot of places in SolidWorks you end up with this little option over in the feature tree called link two now if that check mark is left and I go into the library I open up and edit that tool everywhere it was used will expand or it will contract so this turned off this check mark to the link to form tool if I turn that off this is more or less a poppy if I leave it on it is very much associative to the feature in the said folder that I dragged it from which again can be awesome or can be horrifying but um when you talk about standards standards generally don't change right or if you're talking about these standards these standards are something you very much have your thumb on what's going on with them there's not something that's changing you know for no good reason so I like to have these things linked but uh yeah absolutely 100 associative there and that's part of the whole Arc where this is a part file still and it's a part file that's referenced by another part file as a result of our little Telltale external reference arrows there so that would actually turn off right there I had to turn that link symbol off as well all right good question very good question no matter what happens though I've dropped it on the face and hitting flatten it just lives on the face that you've dropped it on so no Voodoo to make that happen it will stay put and it will go in position we don't take the form features into account when calculations are done though I know in real life there's probably a little stretching or a little bunching or thinning in these areas because it's grabbing material and it's pulling it into other spots there's a little bit of stuff you have to kind of suspend disbelief on but in these particular respects it's not really germane to the geometry there and it's going to be something that's just easier to do in a repetitive process ah customize good okay one of my favorite features here is called convert to sheet metal we have a dozen things for creating complex corners and and extending things and doing all these really weird merges to get very very complex multi-angle compound angle parts but this feature is really the magic to create in the easiest sense some of the more you know compound Hoppers and other parts that just have several angles of crazy edges coming together and the feature kind of speaks for itself so I'm going to go through it here um convert to sheet metal really simply is is just taking a normal extruded part part created with normal features and then sort of shelling it to create it into a sheet metal part if you want to just use very simple terms for what our our tools do um for this particular process though some incredible flexibility the second one I'm going to show you here would be a situation where we have a it's a milled part it's a milled part that could be very heavy could be very expensive depending on the material and it might just not be worth it based on making it as a machine part where making it as a sheet metal part in a box bracket or something to that effect might be much more you know cost effective especially but lighter in the design and that's where you can kind of pivot mid design in order to do this so let me show you what I'm talking about when it comes to a convert to sheet metal feature so this one here is my favorite because again it takes a lot of the disciplines that even seasoned sheet metal people had and when this was added to the software it even expanded some of the most you know seasoned users capabilities for what they could make what I have here is essentially a hopper okay and that Hopper can take a lot of different forms but to make this from sheet metal from sheet metal features it's actually fairly difficult because it's not straight edges there are a lot of straight edges but then those edges have to be extended and overlapped and there's just a bunch of features that you can make it that way but it really is much easier to make this geometry by just doing what we have here which is essentially a a really simple extrude I believe it's an extrude from the side shape there if I show you the sketch right basic extrude then we went ahead and took that extrude and added some draft to some of the faces and then we did a cut that just slices right through here and there's another cut from the side and that slices the bottom off on an angle and now we have compound compound compound angles well I want to make this a sheet metal part I want to do it in a very simple process so again the Magic Bullet is this wonderful button called convert to sheet metal now if you've been using SolidWorks long enough and your software has been installed since before convert to sheet metal existed um this could be with any feature frankly more times than not your it installs new versions of cellworks by inheriting the toolbar settings from your previous version most of you want the tools and options and hotkeys and all that other stuff the same the rub is that new buttons in the new version aren't going to show up with your old toolbar settings because they're simply not aware of it so when you find something like convert to sheet metal or a tool that you use rarely I want you to use this tool up here called commands search to go ahead and help yourself out generally by default it's going to be a file Search tool people really kind of stay away from it because all they see is this little thing up here called cellworks files and models Nobody Does that but you might come up here and hit the commands search button and what happens when you hit command search is you have the ability to type in a little bit of a command so if I go ahead and say c-o-n-v what I have is convert cut convert to Extrusion convert to mesh body convert to sheet metal so it basically gives you the wild cards of what those words match now I can run this button here called convert to sheet metal if I want to but what I could also do is I could run that little guy right up there and I could just drag it over to my toolbars and actually put it on your toolbar here so you can use it next time so that's a little special one right there I love doing that drag it to your toolbar if not you just want to use it once you can just go ahead and run it just by clicking on it and hitting the button or hit the little creepy eyeball and it'll actually take your cursor and it will show you on your interface where your button actually is so it took my cursor and it jumped it over to where that button was actually over the left hand side not this one that I added another little side benefit if you have too many buttons on your toolbars this has nothing to do with sheet metal but you don't have to go into all of the customizing tools to get rid of those just hold down the alt button pick and drag it off the toolbar and it's gone okay so any buttons you don't like just go ahead and hold down the alt button and pick and drag those off of there okay so back to where we were I get a little sidetracked convert to sheet Metals workflow is very very simple now what you see over here on the left hand side first of all is I haven't really shown you much with the gauge tables we have there because right now I can type in any thicknesses I want I can type in any radius that I want but when you go ahead and Trigger this use gauge tables option what ends up happening now is that's going to take all of this interface and it's going to get rid of it it's going to turn it into pull down menus so it takes a few seconds to do this because it's embedding this Excel spreadsheet into the sheet metal file that way if I send it to any of you you've got my spreadsheet so it all works but now what I have for Sheet Metal parameters is a list of pull down menus that I had before and from each of those little gauges what we have is a list of very discrete radii and that's what a gauge table does for you so it's pretty awesome I'm actually going to turn that off right now but I just wanted you to see what that looked like okay so what we have right now is a sheet metal part so the process is just like other sheet metal Parts is you want to pick a stationary face once we do that what it does is it fires up the preview so you can see that there's a thickness here that's available you can go ahead and start messing with that if we need to and then again a radii that's available if we need to deal with that what also is awesome about this is it's very smart so as I continue to incorporate additional edges and faces it will automatically know what to do with those so here's my first face we're going to start with that now I'm going to pick this Edge between the bottom face and this back face and by picking that edge it automatically brings that face into things okay by leaving as it is right now this is what we get okay really simple but very quickly it created something that looks like this which is a really great flat pattern for something I didn't want to make manually now I'm going to go back and edit that convert to sheet metal which is going to leave me right where I was before and again what's beautiful about this is all we're doing is selecting a bunch of edges to bend so as a result of that what I could do is I could select this Edge and it will incorporate this flap and I can select this Edge and it will incorporate that flap but more importantly it also grabs these little edges down here at the bottom and because this Edge is a bend and this Edge is a Bend these two edges can't be a Bend they have to be able to separate so it automatically puts it into this folder called Rip so as I select adjacent faces you'll notice it automatically does all of this if I grab this edge here you'll see that down there it has to incorporate a rip I grab this edge here it has to incorporate a rip so we're really just grabbing all of the edges we want to make these bends and that's going to go ahead and additionally put in all these flaps maybe we'll do that one right there too oh yeah see vertical edges right there now if I wanted to keep doing this I could keep the body of active and make other features I'll do that next time but what I've just done is I've converted this into a sheet metal part which now with the flat pattern is a pretty elaborate flat pattern and that's just by picking the edges of an existing part made with a couple of extrusions and cuts so that will make a very nice watertight body of this really wild Hopper I told you that it would go a little bit different with this when it came to a machined part machine parts are interesting because like I said this thing's got holes it's got parts that are going to have to bolt up to it and it's going to bridge the gap between a couple of other parts but right now it's pretty heavy and it's going to be a big Billet to create this and a lot of chips so it's just not the best really approach for a part like this but if I decide at the 11th hour that I want to go ahead and convert this to sheet metal I can do that now again it's the same process you pick the face to remain stationary and it instantly starts to preview that's a little bit thick for what we're going to do here and then once I start to grab other edges it's going to automatically put those faces that those edges are part of in this particular selection set so I just kind of keep an eye on it I do the side flaps there so maybe that's going to give me what I need there maybe we'll do a little front flap and top flap up here that's kind of fun um maybe a little front flap on that one and again we can just kind of grab different edges and incorporate things as necessary now it will get mad at us at a particular point if we ever have a situation where this part which looks pretty good in 3D is going to collapse back onto itself when it unfolds so it's not yelling at oh it is yelling at me actually right there um warning so uh Ben's intersect uh most space or multiple faces refused together okay whatever we're gonna see it unfold here do we see it hit itself yeah it's actually going to collapse back onto itself um which means it's not going to show me the flat pattern so right up in here because of things and the way they're going to unfold we're basically going to end up having a couple of edges that share material and you can't cut those apart and do that in a 3D so the software is right now yelling at me a little bit on exactly what I've done and why there's a problem there so that's okay SolidWorks being 100 editable I can always go back and start removing edges out of some of these bends if I want to and vet this part a little differently but that flexibility is incredible and it does allow you to not only come in here and make you know a single component from this but if I was to go ahead and leave that component intact and leave the actual solid body there we can do multi-body with all this as well so a little check mark up here called keep body recording region indicator we'll actually go ahead and create the unfold that you see but it will leave that little solid body there so that I can make a second feature if I wanted to so again convert to sheet metal pick a different face pick a different Edge pick a different Edge maybe I've got to make this part out of two separate parts so no big deal so that's really a process that allows you to go ahead and take any part again and turn it into a sheet metal component so we'll hide that guy we'll hide that guy and now I'm left with a couple of separate sheet metal pieces here okay so that's how that all goes but again same form fit and function when it comes down to it at the end make sure we're staying on time going slow all right so that is super super powerful um miter flange this is really something where you can create almost any enclosure type shape this is going to happen on a lot of these boxes out here where you've got a box with electrical pieces in there and then you've got a door that closes over those there's always a lip there's always an overlap and that's the kind of part that you're going to get in something like that so visually here let me just open up quick examples here since we're running low on time and we always go over is you're looking at a part that's really just a basic sheet metal part what I've got right here is a simple Extrusion that Extrusion is just based on the most basic of sketches and as a result of what we've got right now that's going to give us a basic flat pattern right nothing really exotic to that but if you were to come in here pick an edge and start a sketch on that edge which again is a magical thing right here by picking an edge and starting a sketch on there it actually creates a plane right there at the end of that and it creates a sketch for us and a miter flange is something where you can make some incredibly complex edges just by the way that you sketch things so I'm going to sketch out you know pretty pretty ugly looking feature here let's be honest with you on what we're doing here I'm not going to do too many with dimensions but with something like this what you can do with the sheet metal tool here is create an entire compound flange as a result of this little miter flange tool bless you what it'll do initially is it will put that part in place and like all other sheet metal features it's going to give you options to go ahead and change where that radii actually Blends off the existing geometry so if you just want the radius to roll off the edge or if you want this outside face to be tangent with the existing outside face those are kind of the points in between that you get as choices there but what makes this one super powerful is at any point I can incorporate other edges and where those overlap each other they're going to go ahead and give you the proper gapping there this will get really bad so look at how it trims that back look how it trims each of these back and really what's also Happening Here is this little propagate to tangent button pops up anytime you pick these edges so if you didn't want to pick them individually you can just pick one of those and it will just pick the rest of them but you can see how compound this gets we'll wait for my preview to pop out one little sketch creates what's essentially three different bends on this but it automatically trims those in the corner so what creates basically lips over something that could be a box or a cover that's going to close to this and seal up you end up with an incredibly compound flat pattern because of how these things all miter to each other in the corner so we want to build it in 3D of course so that fits in 3D but we have to manufacture this at the starting point which is going to be the flat geometry that's there so miter flange is definitely one that you want to take a look at in more detail okay lofted bends well Lofts by nature and SolidWorks are blending of dissimilar cross sections so what we're talking about with any lofted Bend is taking you know and a lot of HVAC situations Square to a circle now Square to a circle is a ductwork type of a blend but there is a difference between a bent part here which is press break versus a formed part which would be over some sort of die shoe or form or hammered or whatever it is um so there's a couple of different ways that this gets controlled like regular Lofts you could have a feature like this here which is just lofting two splines together to create a sheet metal part now what's interesting about that also is that there's limitations to that it's a pretty cool feature to create that kind of a loft but the reality is is it's only has the ability to use two sketches and you can't use guide curves and those are two things that to me are pretty well Knockouts um what you're doing with something like this just to kind of give you an idea is there's a couple of sketches here and all we're doing in the sheet metal tools is using this one called lofted Bend now when you use a lofted Bend we're blending these two sketches which are just open splines at this particular point but you have to go ahead and use the formed option not the bent option this is too organic for it to have any type of press brake lines that are put in there what it does give you in this situation is the straightest distance between these two sketches like any Loft does and it does do a flatten which is actually pretty cool but geometry in one end and geometry and the other you don't have that which a typical Loft you would be adding additional profiles and guide curves to create something like that so it's an interesting thing to be able to use but for this application this is you know kind of an elaborate shape yeah I'm like with the flat flat drawing of that show where each person this one does not no because it's a formed and that brings me to this example here because that's a very important question when we're looking at something like this this is a sheet metal that would be the circle to a square but we always prep these with a little bit of a gap that's a little not a demo trick we teach that in training because it's sheet metal has to be able to open up and close and when you go ahead and do a lofted bend on what is really decidedly two dissimilar profiles when you go from the circle to a square see this one I have to do bent it won't even let me do forms because I've got sharp Corners what this will actually do is it will give you those press break points okay now this one here is going to show you each of those not only in the formed mode but also in the flat pattern because these are legitimately edges and radii okay so you're going to see each of those that is also something that as you create these types of features and you're editing or creating the Loft in general each one of these bends anytime you see a magenta dot you can action on those individually if I want to take this particular Bend here and determine you know not cord length but maybe a number of bends there then I could go ahead and actually put in more or less depending on how quality I wanted that and of course whenever you're talking about facets the more you have the more round something gets created with Flats so you'll see that this one edge here is actually a lot more round even though it's a series of flats but it's 20 versus 12. you know so much more round in that respect um the opposite part of that again is the formed features so now we're talking about um you know something where we've prepped it a little bit for something like this but not sharp Corners in the corner we've actually prepped it with radii features and something like that so same operation let's go formed on this one and with any Loft we're just picking these loss roughly where they're going to bend so now you don't see those individual bends right and what you're basically getting here is a smooth-ish part I guess on this one we did put arcs in there so you're kind of seeing the facial segments but you know if we don't put those arcs in there then you're not going to see each of those features all right um let's just do this last part here I'm going to talk about this for a second there is a flattening tool in Stowers professional and premium that is called surface flattening I'm sorry I think it's only premium is that right Tim only premium um that does allow you to take any compound selection of faces and flatten them out it's basically for creating decals it has some vetting tools for actually doing some some calculation stuff um they're going to start doing some drawings and stuff down there in a second here so I'm going to do this one last one and then turn you guys loose but this is an interesting thing so if you do have access to sauer's Premium you can get the flat pattern of pretty much any geometry that you've created now I I say that with a little bit of hesitation because we have a third party product that's called forming technologies that is for stamping dies it's for doing door panels and one hit type operations with draw beads and and binder plates and all kinds of great stuff but when we're talking about this one here this is one tool here that's again called surface flattening and it only exists in a premium seat of SolidWorks but it enables you to go ahead and select a face like this one here which is actually domed in two different directions so you can see that that is compound in both different ways there's no flattening of that in a realistic sense um but by grabbing it like this and just selecting the face and then any particular reference Edge we create a flat surface from that feature now what generally happens as a result of that is you're going to get a surface that if you right click on actually has a deformation plot that shows you the tension that you get from having a dome in two different directions feature flattened there's a lot of compression that's happening in these areas and what's really interesting about the tool is the tool addresses that by actually allowing you to deal with that particular feature I'm going to just delete this feature to show you a second time we're going to put that in one more time but what it enables us to do is pick this surface and I'm going to utilize a couple of little edges that I put in there called hold lines there's these little blue edges here that I've used to split this face if you put those in as relief Cuts what it actually does is it allows it to separate the decal where you have those lines what that essentially does is it takes all the tension off those edges so now because it's cut there what you can kind of Imagine as this thing relaxes is once it kind of rolls over the face and kind of comes together those edges come back together as a result of that so that's why you don't see any red in there because there's no tension anymore once they lay around the face those edges will kind of end up coming right back to each other again hand puppets is the only way I can do that um so this is a tool that's out there this is actually literal a surface in the feature too it's not just an analysis there's something you've got geometry that you can right click and dxf that bad boy out and be able to go ahead and cut this on a decal cutter or mylar or something like that okay that's it um you can also import parts from other systems if they have constant wall thickness we can unfold them immediately if they don't you can actually use thickness analysis which is in professional or premium to find things like bad radii delete them put new fillets in and then flatten these parts but you can work with parts from other systems as well Mike when will gauge tables be associated with your material selection I don't know they're still not though are they they are not okay um my name is Darren so if you want to send me an email on this uh D grocer at goengineer.com guys and I can send you anything down there so all right I appreciate that rapid fire sheet metal all right take care thank you [Music]

Channel: GoEngineer

Views: 15,608

Keywords: goengineer, engineering, MCAD, mechanical engineering, product design, product development, solidworks

Id: ycDAnSokh6U

Length: 43min 11sec (2591 seconds)

Published: Thu Oct 06 2022