Name: Mastering Sheet Metal: Advanced Tips & Tricks for SOLIDWORKS Users
Uploaded: 2026-03-26T18:30:05.717Z
Duration: 1 h 15 min 6 s
Description: Mastering Sheet Metal: Advanced Tips & Tricks for SOLIDWORKS Users

Transcript for "Mastering Sheet Metal: Advanced Tips & Tricks for SOLIDWORKS Users": Hey, everyone. Thanks for joining today. I'm Brady Daniels, a senior applications engineer here at GoEngineer. So today, we're gonna be talking about mastering sheet metal and SOLIDWORKS, looking at a mix of best practices, useful tools, and some tips and tricks along the way. We're gonna cover a few fundamentals, but we're all we will also dig into some areas that tend to trip people up or get overlooked. The goal here is to give you some practical takeaways, things that you can apply right away to improve your workflow and avoid common issues. So whether you're newer to sheet metal or you have been using it for a while, there should be something in here for you. Here's a quick look at the agenda for today. We'll start with bend calculations just to make sure we have a very solid foundation there. Then we'll move into different design approaches and when you might wanna use each one. After that, we'll spend some time on flat patterns and how to work with them effectively. From there, we'll get into multibody design, which can be really powerful for more complex parts. And then we'll wrap things up with a few additional tools and recommendations to help improve your overall workflow. First, let's take a look at how bend calculations work in SOLIDWORKS sheet metal. So whenever we bend sheet metal, the material behaves differently across the thickness of that part. The outside of the bend is being stretched. That's the tension side, while the inside of the bend is being compressed. And somewhere in between is what we call the neutral axis. That's the layer of material that isn't stretching or compressing. When we create a flat pattern, we're really calculating the length of that neutral axis. So where that axis sits within the material thickness is what ultimately drives our bend calculations. Now in reality, that neutral axis doesn't behave per perfectly like you see in these diagrams. As the bend is formed, the material actually thins out slightly, and the bend radius changes shape a bit and deforms. And because of that, it it shifts around as well, and it's not sitting perfectly in the middle of the material anymore. K? So when we talk about bend calculations, we're really working with approximations. The values we use to predict our flat pattern length come from testing and experience, either, you know, standard industry data or values developed in house based on real world parts. And in SOLIDWORKS, there are three main ways to define how sheet metal behaves during a bend, but they're really just different ways of describing the same thing. We have k factor, bend allowance, and bend deduction. As long as your inputs are accurate, all three methods will give you the same flat pattern. It really just comes down to which one your company or your manufacturer prefers to use. So let's take a quick look at what each of these mean. K factor is simply a ratio that tells us where the neutral axis sits within the material thickness during a bend. It's defined as the distance from the inside face of the bend to the neutral axis divided by the total thickness. So it's always a value between zero and one. If a k factor is 0.5, that means the neutral axis is right in the middle of the part. In reality, it usually falls somewhere between zero point three and zero point five depending on the material and your bend radius. And when we enter a k factor in SOLIDWORKS, it uses that value to calculate the length of the neutral axis through the bend. Right? And that's what we call the bend allowance. That's essentially what SOLIDWORKS is doing in the behind the scenes. Once you define the bend radius, bend angle, material thickness, and your k factor, it uses that information to calculate the bend allowance and then automatically applies it to generate the correct flat pattern. And in practice, k factor is probably the most commonly used method because it's simple and flexible. It works well across different bend angles, and SolidWorks handles the math for you even when you have multiple bins going in different directions. So we're gonna take a quick look at a visual inside of SolidWorks to get a better idea of what this does. Alright. So I have a pretty simple part here. It is one millimeter thick, and it just has a 90 degree bend. And what I'm gonna do is try to illustrate where that neutral axis is. So what I'll do here is edit my sheet metal feature just to show you that my k factor is 0.33. So one third of the way through the materials where I should expect my neutral axis to be. So let's actually test that out. I'll create a sketch here. I'm gonna use offset entities from the inside of my bend, and I'm a set that to 0.33 millimeters. And I'm actually gonna redo that so I get the whole thing. There we go. Grab that and that, and then we'll click okay on this. And there is our theoretical neutral axis. And if I go ahead and measure this using the measure tool, drag that over, I can get a total length of 20.09 millimeters. So keep that value in mind because I'll exit my sketch here and then go into my sheet metal tools and flatten this out. And then if I measure the edge of my flat pattern, we should end up with exactly the same value. K? So that's that gives you an idea of what the k factor is doing. It's finding out where that neutral axis is, and then that's being applied to your flat pattern length. K? Another thing that's important to note whenever we are entering our values, specifically our bend allowances for our bins, is there's a hierarchy in here. So if I right click my sheet metal folder here and edit this feature, I have a bend allowance and a k factor that we just saw. I also if I have multiple bodies, if I have multiple sheet metal bodies inside of my part file, both of those are all of those are gonna show up here, and I can actually change my BIN allowance for those bodies individually as well. So that would be higher on our hierarchy. But there's actually another level. If I go into my actual bent features, my base flange here, and I go to my base bend and edit feature, there's another bend allowance in here. So we have the ability to set our bend allowance for each bend, for each body in our cut list, or as a a whole for the whole part file. K? So that's important to know if you're, you know, back at home working on your sheet metal parts and you're changing your k factor and nothing's, changing in your model, it might be a hierarchy issue for your bend allowance. Alright? Let's jump back into the presentation here. Now while SOLIDWORKS can calculate BIN allowance automatically using the k factor, you can also define it manually. If you have access to a reference chart like the one shown here, it can actually be easier to just pull the bend allowance directly rather than figuring out the right k factor. Right? This approach approach is especially useful when you're working with established shop data or trying to match a specific manufacturing process. Now the third option, bend deduction, works a bit differently than bend allowance. Instead of defining what gets added to the flat pattern, it determines how much to subtract from the total outside flange lengths measured from the virtual sharp to get the correct flat pattern length. K? So this diagram shows a side by side comparison of the two methods. One, where you are measuring from that virtual sharp and then subtracting material for bend deduction, and then where you're measuring, the actual flange length outside of the bend and then adding the bend allowance. And here's the bend deduction equation. If you're curious, you don't really need to calculate it by hand every time, though. There are reference tables that list precalculated bend allowance, bend deduction, and k factor values for common materials, thicknesses, bend radii. And we can build those tables inside of SOLIDWORKS, which is what we're gonna look at next. So that is where bend tables come in. Bend tables allow us to specify a bend allowance based on the angle of the bend, the thickness of the part, and the bend radius inside of an Excel table. There are also tables available for bend deduction and for k factor that come with SOLIDWORKS. So SOLIDWORKS will tell you that the out of the box bin tables are just samples and shouldn't be used for production, but they are a great starting point, so you can set up your own data. And some are actually extracted directly from the machinery handbook, which is pretty cool. The BIN tables that come with SOLIDWORKS are usually found in the install directory under Lang and then English and then sheet metal BIN tables. However, it's a good idea to set up your own folder in your file locations for bin tables and for the other tables that we're about to cover next just because it's easy to accidentally lose your data by overriding the default locations during an upgrade or during a repair or something. So keep that in mind. But let's go ahead and take a look at an example. So I'm gonna switch over to SolidWorks here, And then I'll open up my file explorer, and I've navigated to the location that I need to be already. So in my c drive program files, SolidWorks Corp, whatever you name this this, install directory, SolidWorks, lang, and then English, we have our sheet metal bin tables. And the bin tables that come out of the box, the samples are blank, and you can use these to create your own custom bin tables, which is pretty cool. We also have in the bin allowance and bin deduction folders some completed examples that you can work off of. You can see that these were extracted from the machinery handbook, twenty sixth edition, with permissions from industrial press. K? So this is what we're gonna look at using in our models. K? So I'm gonna go ahead and close this. And at this point, what I'll do is change my sheet metal feature, and I'm gonna switch it from a k factor to a bin table. K? Now I'm gonna select well, I'll browse first. I'll browse to my BIN allowance tables here and select that folder. And then I'll select my metric BIN table because I'm working in metric units here. K? So I'll click okay on that. That will load in that Excel data table. And now it's working in the background, and it's influencing how my, model, the geometry of my model. And I can tell that it's making changes. I know it doesn't look like anything changed. But if I flatten this and I measure this value again, go to evaluate and measure, the, the value has actually changed. It's now 20.2. Okay? So that, just changing to a bin table has changed how what happens with my flat pattern. K? Alright. I'll go ahead and unflatten this, and we'll go back to the presentation. So bin tables are nice, but there is an even better option. And that's the SOLIDWORKS gauge table. So they provide a consistent set of options for gauge, bend radius, and bend allowance every time you create a sheet metal part. And because these options give us so much control, I usually recommend that anyone working with sheet metal takes advantage of them if they can. And let me show you how they work. So the gauge tables are very similar to a bin table in, format, and they're in the exact same location as your sheet metal BIN tables, just under a different folder. And we have a couple of really good examples. But, essentially, what we're well, how they function is you have multiple tables for, different gauges, and those gauge values are gonna be what's available to you in your options when you set up your sheet metal part. And under those gauges, you have different thicknesses that are available. You have different angles. You have different radii that are available, and then they give you, in this table, the available bend allowances that it's going to assign automatically. K? There are other types as well. If I just look at this one, this one's a little bit different. This is just a, a bigger list of gauges, gauge thicknesses, and then our available bin radiuses, but it fixes the k factor. So, there's cons and pros to both, but we're gonna use this one for our for our example. K? Alright. So let's jump right back into SOLIDWORKS, and then I'll switch over to a gauge table. So the gauge tables are a little bit higher up in the property manager right here. You select use gauge table, and then you can select whatever gauge table you need. And I'm gonna select this bend allowance millimeter sample. And when I do that, my options in my tree or in my property manager completely change. I now only have a couple of thicknesses that I can select. I just noticed my part is missing. That's interesting. But regardless, I have a a set list of gauges that I can select. I have a set list of BIN radii, that I can select. I can also override those with checkboxes if I need to. And then my bin bin allowance is being controlled by my gauge table. K? I can click okay on that, and then it will, once again, load that new table and give me my component. Alright? And this one obviously made quite a few changes. But if I flatten it, just so, you know, I'm not lying to you, I'll measure it, and we're gonna get a different value. K? There we go. So that's the basics of the tables, but there is a really cool way that we can set them up in a really it's really handy. What we can do is we can link a gauge or bin table straight to a custom material. And you can see that option here in the sheet metal tab of the material die dialogue. Once it's set up, whenever you assign that material to a model, the right sheet metal properties come with it automatically without the need to set them up every time, which is very powerful. So let's go ahead and take a look. So, again, to make this function correctly, what we need to do is assign a custom material. So if I edit material here. Oh, and before I do this, actually, let me go ahead and just mention one thing. You can set this up to be the default for all of your new sheet metal parts by going to your system options and then going to document properties and then sheet metal. And then there is a use sheet metal parameters from material option for new sheet metal bodies. So if this is the workflow that you want, make sure that you go in here and turn this on and then save your settings as a template so this setting is always turned on for you. Alright? So let's go ahead and apply a material. And I'm gonna apply a custom material that I've set up here. And this will not work for the SOLIDWORKS materials, so you have to copy them or create new, materials for this to function properly. But we just go to our custom material in the tree here, then go to the right, click sheet metal, and then I can set a specific gauge table, a specific bin table, or a thickness range where we're doing different tables at different thicknesses. There's a lot of things that we can do in here. But the basics basic thing we can do is set a gauge table to be applied every time this new material gets applied to a part. So I'll apply this and then close. And now if I go to my sheet metal, I need to make sure that my used material sheet metal parameters are here. Yes. And then we'll click this. Again, this is why you wanna go into your, document properties and make sure that that, option is checked. And then the correct gauge table is pulled in automatically. It's really sweet. And then I can, you know, function and change the properties of the gauge table, like I normally would. K? So that's really cool. Again, that's only gonna work with custom materials. So you do have to go in and create custom materials and then go to that sheet metal tab to make that function properly. Alright. Now let's take a look at the different design approaches you can take when designing sheet metal parts in SOLIDWORKS and when it makes sense to use each one. So, generally, it's best to start with SOLIDWORKS native sheet metal features. They give you the most control and flexibility. But if that's not an option, the insert bins tool works well as an alternative. And converting to sheet metal is also a handy tool, but it's usually something you do only when the standard features don't give you enough flexibility for, like, complex shapes. Now when we're using standard sheet metal features, you all almost always start with a base flange. Think of it as the foundation of your part. It's the first feature you create, and everything else just builds off of it. And once that base flange is in place, you have a full set of dedicated sheet metal features to build out the rest of the part. We have edge flanges, miter flanges, jogs, hems, and more, etcetera. And because these are native sheet metal features, SOLIDWORKS handles all the flat pattern calculations automatically as you go. Alright. Let's show a quick example of this type of workflow. This is the very basic workflow. So what I'm gonna do is I'm just gonna start from scratch. I'm gonna open a part, set my units to inches, and then I'm gonna create a base flange. So to get started, I can click base flange, select my top plane here, and then I can start building my, my component. I'm a switch to a corner rectangle, go up into the right, give this a dimension. We'll say 10, and then we'll say 15 here. That looks good. Now when I exit the sketch, it's going to apply automatically a thickness to this component based on, the bin calculation and the thickness that I select. So I'm gonna say, for this one, I'll use a gauge table, and I will use the sample steel table here. It's gonna always apply a 0.5 k factor for me. And, three gauge works for this. And one thing to note is once I set this these values for my first feature, they're gonna carry through to my subsequent features unless I override them. So we'll click okay to that. And then now I have a good base that I can build off of. So I can do things like add edge flanges at a certain distance. I can add that to multiple edges at once if I want to, like so. I can edit flange profile. This allows me to actually control the sketch for my flange profile. So I can actually get in there and change the way that looks entirely, then click finish. That gets me kind of a more unique shape. We have other, other tools in here as well, like like a hem tool, for example. I'll go ahead and create a closed hem. Drag that out. Oh, flip the direction, and then we will pull that out a little bit. Click okay. So we have, a hem on that side. We can also do, more complex flanges. Like, maybe I wanna do a miter flange on one of these. So let's say on this face, I wanna create a more complex bend. So let's go here. We'll go out like this and then go back up kinda like that kinda shape. Obviously, I would add dimensions if I was in a production environment, but we'll just leave it like that for now. Then I can select from my different options for each of these. Each of these has their own set of of options. Some of them that are consistent are, like, flange flange position. It can either be at the virtual sharp outside of the material thickness or the entire bend outside of the thickness, and that just changes where the that bend actually happens as you can see there. Click okay on that, and we get a pretty interesting shape. K? And we have, you know, a whole host of other types of tools in here. Some of them we'll talk about. Some of them we won't have time to talk about. But that's kind of the basis of this workflow is you start with a base flange, and then you build on that base flange to create your final component. Now your base flange doesn't have to be a rectangle. It could also be something more complex, which I'll just show you real quick. So I'll say on this front plane, for my base flange, instead of doing a rectangle, I just wanna do something kinda complex. And I'm just gonna do this disconnected from my other component. Let's say we want something weird like that. K? I can draw, just my my line here, and then I can go sheet metal, base flange, and then it's going to apply a thickness to a thin feature that I can use to create a new base flange. K? Again, my gauge table is in is active, and I have options for, you know, how far this this extends, etcetera, etcetera. But when I click okay, it creates that base planche, and then I can go in and add all my other stuff that I showed you earlier if I really want to. K? Alright. So that's the basis of, this workflow. You'll also notice that I created two separate, solid bodies. We're gonna talk about multibody design later. So just keep in mind that we can do multibody design in sheet metal. But let's go ahead and talk about our second workflow. So our second workflow is insert bins. This method has actually been in SOLIDWORKS since '97 or '98, so it's actually the same age as me. So it's been around for a while, and it's definitely the older approach to sheet metal design, but it's not obsolete. It's great for creating sheet metal parts from imported geometry, but only if that geometry has uniform thickness. If the part is multi thickness, then you'll get an error, and you'll need to use a different tool. It's also great for rolling out cylinders and conical geometry. And I'm actually gonna show you an example of taking a a cylindrical shape and then using insert bins to create a sheet metal pattern. So let's jump over to SOLIDWORKS. I'm gonna go ahead and open up my cylinder. And this is just a regular cylinder that was shelled out. And all I've done is I've added a sketch with a sketch point for reference. And this is actually a pretty cool enhancement that was, I can't remember the year, but it was somewhat recently. The rip command can actually be used to create, rips inside of cylindrical, components. In previous years, you would have to, like, create a circular, or, like, a a central sketch where you, you know, create two lines and then connect them so you can do, you know, an extruded cut. It was just a little clunky. But now what I can do is select an edge of my cylinder and then select my sketch point. It's gonna create a a rip for me, which is pretty awesome. And I can you know, there's options in here for for different things. I can switch to offset, all kinds of stuff. And when I click okay, I now have a component that can be turned into a sheet metal part. And to do that, I'm gonna use the insert bins tool. So we'll go to insert bins. The insert bins tool asks for a fixed face. For this, we don't have a a fixed face, but we do have a fixed edge. So I can select an edge. And then all I need to do is click okay. And now I have some, sheet metal features that are processing the bends for this cylinder. And I can click flatten, and I get my flatten component. K? That's the the real beauty of insert bends is doing things like this. K? Alright. Now the last method we're gonna talk about is convert to sheet metal. As you can see here, it takes an existing solid body and converts it into a sheet metal part, which makes it particularly useful for complex angle geometry like this hood shape that would be difficult to build from scratch using the standard sheet metal features. Convert to sheet metal also works really well in a multibody design workflow. You can convert a section of your solid body to sheet metal and then optionally keep the original body to derive additional sheet metal features from it, making it a very efficient way to build up multiple sheet metal, components from a single solid. It's also the go to option when you're working with imported parts that might have a nonuniform thickness. In those cases, insert bins actually won't work. So convert to sheet metal gives you a way to still get a usable sheet metal part and a valid flat pattern out of it even though you can't with insert bins. Alright. Let's switch over to SOLIDWORKS and take a look at what this workflow entails. So once again, I'll open up a component here. We're gonna work on this stack. And all I have done for, for creating this is I've created one solid body. So this whole thing is one solid. And what I'm gonna do is I'm gonna use the convert, to sheet metal tool, which is right here, to produce multiple sheet metal parts from this solid body. K? So I'm gonna go to convert. I'll select a fixed face. I'm gonna start on the top here, this top section. So I'm gonna select a fixed face. And then once you select your fixed face, you need to select the edges where you need bends. K? So this edge, I will need a bend. I'll also say this edge will be a bend, and then I'll also add a bend on this side. K? And then it gives you a couple of visual indicators on screen. The blue edges are your bends, and then any pink edges are the gaps or the rips that are gonna be needed to, create a flat pattern. So we have a couple of, pink edges on here as well. Alright. And then once again, I can apply a gauge table. I could use my, you know, material sheet, metal, parameters that I showed you before. I'm just gonna accept the defaults for now and click okay. Alright. And I did forget to mention that I have keep body checked. If I turn that off, it's actually going to create my sheet metal part and then get rid of that solid body. So I wanna have that on because I'm gonna create an another part using the same technique. Alright? So here we go. We'll do it one more time. And this is gonna be a multibody, component. So I'm just going to do the same thing for this lower section. So I select selected a fixed face, and then I can select my bins. Bend here, bend here, bend here, and I think my yeah. There's a bend here, so I'll match that on my lower component. There we go. I'm gonna use the same settings as before and click okay. And there we go. There's our sheet metal component. And in that second op, convert to sheet metal, I can uncheck keep body and click okay to completely get rid of it. And now I have two distinct sheet metal components with complex geometry. And creating this would be somewhat difficult using the standard features inside of of sheet metal. So that's, a case like this is a good use for that convert to sheet metal tool. Alright? And just to show you that we do have two multi bodies here, we do have two bodies inside of this multi body part. I have a body here, a body here. I can flatten those individually if I want to, which we'll talk about later on as well. But, yeah, that's the basics of convert to sheet metal. So let's dive back into our presentation. And next, we're gonna take a look at how flat patterns work in SOLIDWORKS and how we can manage and control them. So one important thing to understand is that the flat pattern is actually just a feature at the bottom of the feature tree. That means we can suppress and unsuppress it just like any other feature. When it's suppressed, we're looking at the formed part. When it's unsuppressed, we're seeing the flat version that would be sent out for manufacturing. So, really, you're not creating a separate model. You're just switching between two states of the same part. The other key piece is the format of your feature tree when working with sheet metal parts. Basically, everything that defines your sheet metal part lives between the sheet metal feature and the flat pattern feature in the tree. So any features inside that range will behave correctly when the part is flattened. If you create features outside of that range, you can run into issues where they don't show up properly in the flat pattern, etcetera. So a good rule of thumb is to keep all of your sheet metal related features inside of that sandwich. And if we need to add a feature that would be easier to create in the flat, we don't want to unsuppress the flat pattern and work there. Instead, we use the fold and unfold features. This lets you, temporarily flatten out specific bends, make your edits like cuts or holes, and then fold the part back up. That way, the feature is created, correctly and will behave properly in both the formed model and the flat pattern. Also, make sure that it, stays within that sandwich we were talking about. So let me show you what I mean here. Switch back to SOLIDWORKS. We're gonna work on this component here. So, again, the flat pattern is just a feature at the bottom of the tree. Inside of that flat pattern folder, there is a flat pattern feature that we can do a couple things with that we'll talk about in a moment. There's a sketch for the bin lines, a sketch for the bounding box, and then we have features that track all of the bins inside of that need to happen to flatten out the component. K? And we can reorder these. I will show you that here in a moment. But the the bend order does matter. The order that these show up does matter, and we'll talk about that here in a moment. So, again, it's just a feature, that we can unsuppress. The best way to unsuppress it is to just click flatten in the sheet metal command manager. Just click that, and you get your flat pattern. K? Pretty simple. Now whenever you're working with multibody designs, which we'll talk about later, there's a different workflow. But for right now, just remember, click flatten. It's the easiest way to go about it. K? Another thing is that sheet metal sandwich. So we have a couple of features inside of this component that are not related to our sheet metal body. We have a boss extrude. We have a shell, and then we have a rip like so, and none of those are related to the sheet metal. After that, we did an insert bends where it will actually process the bins needed to flatten out the part. So this flatten bins and process bins feature need to stay between our sheet metal feature, sheet metal full sheet metal folder, and our flat pattern. Alright? Doing that will make sure that they always function correctly. Okay? Now if I wanted to make a change let's say I wanna make a change where I I make a cut at the center of this bend here. Now if I went into my flattened state and I started, making changes, making cuts, those features would show up below the flat pattern. That's not what we want. What we want is those changes to show up in between our sandwich. Right? And the way that we do that is with the unfold and fold feature. So at this point, I'll click unfold, which is up here in my command manager. I'll select a fixed face for this unfold. So fixed face just means it's not gonna move, wherever all of the bends are on are, unbent. And then I'll collect all bends and click okay. Alright. So now I have an, an unbent or an unfolded component. I still have my flat pattern, but at this point, my unfold is above my flat pattern. It's still inside of my sandwich. And what I can do is make it changes. So I'll create a sketch here, and and I'm just gonna do a a simple, corner rectangle cutout here. I won't even bother dimensioning it, but we'll cut that out. Say through all, and then click okay. And now I've created a cut directly in the middle of a bend. But at this point, what I can do is go back to sheet metal and then fold it. So I'm basically just doing the opposite of what what I just did with unfold. So I'll collect all bends, click okay, and then it rebins there. K? So, again, if you have a feature that you need to add and it would be way easier to do in the flat pattern, use the unfold tool and then the fold tool after to make that change. Alright. Let's keep going on here. So now that we've seen how to work with the flat pattern, let's take a look at some of the options we have to control it. One of the most important settings here is the fixed face. This is the face that stays in place when the part is flattened, and then everything else essentially unfolds around it. Changing this can affect the orientation of your flat pattern, which becomes, you know, important when you're creating drawings or sending this out for manufacturing. Another useful option here is merge faces. When this is turned on, SOLIDWORKS will combine all of the coplanar faces into a single face in the flat pattern. That usually gives you a cleaner result, especially if you're laser cutting it or exporting to a DXF. And if you turn it off, you'll see all those individual faces broken out, which we'll see in a in a moment, which can be helpful in some cases. But most of the time, leaving this on is the way to go. Now the last option here is grain direction. This controls how the bounding box is oriented around your flat pattern. By defining the grain direction, you're essentially telling SOLIDWORKS how to align the box. And this becomes important for, you know, nesting and then calculating material usage. And, also, the bounding box properties are something that we can link to in the cut list, so it becomes important for linking properties as well. And, yeah, let's go ahead and take a look at how these settings affect the flat pattern. So we'll go back into this component, and I'm gonna go ahead and edit my flat pattern feature. So I'll just right click flat pattern and then edit feature. And this is where all those settings that I just mentioned stay. So right now, my fixed face is right here. So everything so this is staying stationary, and everything else is unbending around it. If I change that to this face, the orientation of my flat pattern is gonna change entirely. And that can be important whenever you're, again, making drawings from a flat pattern or, you know, sending this to manufacturing. K. So I'll go back to the original face. Let's also take a look at what happens when I turn off merge faces. So you can see now we are seeing, those bends at the tangency point. There's a hard edge, and that's now being shown. Again, the default is that it's gonna merge those spaces, and you can leave that on most of the time. But sometimes it is helpful to know that that is an option. Alright. The other thing that we mentioned is grain direction. So if I click okay here and then I look at my bounding box sketch, I can see that it's oriented in a pretty, you know, intuitive way, just the the smallest rectangle that can be applied to the model. Right? But if I wanted to change my bounding box direction, what I can do is edit my flat pattern, go to grain direction, and then select, you know, an edge or something. I'll go ahead and select this edge here to get something interesting, and then click okay. Now if I look at my bounding box, it's maybe not intuitive for, you know, this mod this specific flat pattern, but you can, change it here. And that affects quite a bit. Namely, if I go to my, cut list and then look at my property summary and look at, like, my bounding box area and my bounding box length and width, all of those values are gonna change based on, that change to the grain direction. So all of those are important. K? Now the last thing I will mention here is when I right click my flat pattern feature, there's an option to reorder bins. So the in some cases, the order that your part is unbent matters. And I can, go into this list and move my actual bins up and down in the the bend order, if I need if I if I need to. In most cases, it's not necessary, but there are specific cases where you need to do that. K? Alright. So that's our flat pattern options. Let's show one more advanced technique that we can do. And it revolves around, one challenge you might run into with flat patterns that is long flattened times, especially with more complex geometry like this, the the model on the screen. So we're gonna show you a way to work around that so you're not stuck waiting. K? So let's dive into that. And the reason that this model specifically takes a long time to rebuild is because of this pattern. And that's clear to see. SOLIDWORKS doesn't love patterns. It takes a long time to rebuild, and I can attest, it takes a long time to flatten. Because when I was setting up this demo, I, have apparently, I have a habit of clicking flatten too often and had to wait a couple times. But, there is a way to work around that. And the way that we're gonna do this is I'm gonna have SolverX create a derived configuration. And then all I'm gonna do is suppress the original pattern in the original configuration, and then I'm gonna recreate the pattern in the derived configuration so they are separate features. And I don't have to wait for solvers to calculate the pattern when this is, when this is flattened. And it's gonna make more sense whenever I actually go through here. But, the first thing to do is I need to suppress the pattern. Oh, actually, one thing before we get started. Just a a quick recommendation, especially for something like this where there's lots of small detail. If you go to your system options and then performance and you're having rebuild issues, especially with, you know, a a model like this, you wanna turn off verification on rebuild. Now I would always recommend when you're doing sheet metal design and you're not having rebuild issues, turn this on. K? It does a more advanced body check whenever you're it's doing a rebuild. So we can actually catch things that are going wrong sooner. Definitely turn that on by default. K? That's, what I would say. But for this, I'm gonna leave it off and click okay. And then what I'll do here is suppress the pattern. So whenever I flatten this and when I'm working with it, it doesn't explode. And what I'll do is make sure that it flattens. That looks good. And by default, again, this is just a the flat pattern is just a feature. If I go to my configurations, I just have one default configuration. And the way that I can have SOLIDWORKS create that derived configuration is I can go into a drawing and make a drawing from this part. When I do this, what I can do is drag the flat pattern from the view palette and just drop it directly onto the, the drawing sheet, and that's all I have to do. I don't even have to save it. I can go ahead and just close this drawing file. I don't need it anymore. Just close it. I don't even save it. And now when I go to my configuration manager, I have a derived configuration for that flat pattern, k, which is pretty pretty sweet. Alright? And I can flip between those if I want to, and it kind of just changes your architecture a little bit. Instead of clicking the flatten here, it makes more sense to go to your drive configuration, click here, and then go back to your default. K? Now how are we gonna deal with the pattern? The first thing I'm gonna do is I'm going to right click the pattern and then configure the feature. K? This is important. Since we're working with a derived configuration, any changes made to the parent are pushed to the derived configuration. So I need to tell SolidWorks, hey. I want you to suppress this in my flat pattern config. So I'm gonna unsuppress it in my default configuration, and then it's again, that change is going to propagate to my flat pattern. But then I need to tell it again to suppress it in that flat pattern. K? That's very important. If you if you just unsuppress it now and then try to switch to your derived configuration, you're gonna be sitting there for some time. K? I'm gonna apply that and then click okay here. It'll take a second because it's gonna rebuild that, that pattern. I'll click okay on that. And now what I can do is go back to my default or not my default, my derived config, and I can recreate the pattern on my flat. And the way that you do that is just the manual method. You just go to linear pattern, select the direction. We'll do an up to reference, here. We'll go by the centroid. That's fine. And then, for the feature, we're just gonna select the, cut shirt. So this is a, you know, a typical scenario here. There we go. Set our spacing, and then I'll select a direction too. Again, we'll do up to reference, which is which is fun. And then, I'll say my spacing is going to be 0.24 like that. And then my offset I forget the offset that I set for the other one, but I'll set my value to something close. I don't actually remember what that value is, but I would go in and make sure it it matches exactly. Alright. So I click okay. No longer in the model. Here we go. Click that. Try that again. It really doesn't want me to do this for some reason. So I'll say selected reference. Oh, this isn't super important. So I'll go ahead and just click okay, and we'll pretend that it's exactly the same. It'll be alright. The important thing is now I have a pattern that should match my original pattern, but it only exists inside of my drive configuration. So now I can click save and make sure, it should be fine, but I will make sure that this configured feature is only available in my, derived config, which it is. I can click okay. And now I can just flip between the two, and it doesn't take thirty minutes to flatten it, which is pretty awesome. It'll take some time because this is a a big, pattern, but they are now separate but equal. K? Like so. There we go. That's really, really sweet. Now the problem with this type of workflow is you have you now have two configurations to manage. So I would only recommend doing this if the model that you are doing it to is completely done from a design perspective. You know, then you can go back and make small edits and everything, but you don't wanna do this right away. You wanna have something that's ready for production, and then maybe, you you do this technique So you're not having to manage two different configs. Alright. Awesome. Now one of our last topics here is, multibody design. So we'll shift gears here, and talk about multibody design for sheet metal and why it can be a really powerful approach. Now there are a few big advantages to using a multibody approach. First, it allows for faster modeling with with associativity in a part file. Since everything lives in that part file, all the changes are gonna update together automatically. So you're not chasing references across multiple files like you would in an assembly. It also enables hybrid modeling, so you can mix sheet metal features with other solid features like weldments when needed, and it gives you a lot more flexibility. And finally, it supports a master model approach where you can build and control an entire design in one place, then break it out into individual part files or individual bodies later. K? So let's just take a look at a multibody design in SOLIDWORKS. And I close this, this guy here. And we're gonna look at our cage. So this is a design of a cage, and it's pretty simple. It's just two bodies that were created, an enclosure and a shelf. And it's really cool to see if I make one change to my width, the other solid body is going to update with it. That's the big benefit of working with multibody design is that associativity. It's also easier to make, if you have complex, mating, between two components, maybe there's complex angles and you need them to fit together pretty precisely. That's easier to do in a multibody design when compared to an assembly as well. K? Alright. That's the basics of the benefits there. Let's talk about how we can create them. So one of the simplest ways is to create a multibody part by, disconnecting bodies within the same part file. Instead of building everything as one continuous piece, you're creating separate sheet metal bodies that all live in the same environment. This works really well when you have assemblies made up of individual components like panels or brackets, but you still want to design them together and keep everything aligned and associative. So to do this, the key is to pay attention to the merge result option. By default, Solvers will try to merge new geometry into an existing body to create a single body. But if we clear this option, it allows us to create a completely separate body instead. So anytime you're building multibody sheet metal parts, this is something you wanna keep your eye on. Another way is to create multibody sheet metal parts by using convert to sheet metal. This is the method that we saw previously. Again, this takes existing solid geometry and converts it into sheet metal bodies. The nice thing here is that you can apply that to multiple bodies within the same part, which makes it really flexible, when you're working with more complex or imported geometry. Another approach is mirroring. This allows us to quickly create additional bodies based on existing geometry while keeping everything aligned and associative. And it's not just the mirror tool that can do this. We can also use patterns and other methods to create additional bodies. So let's go ahead and take a look at a few of these methods in SOLIDWORKS. And it does look like I'm gonna run up on time. I will go over, but I you know, if you do have to leave, I appreciate your your attention, and thanks for joining us. Alright. So let's go ahead and open up one of these components. This is the start of that cage component that we were just working on, and I'm just gonna recreate that that shelf component. And to do so, on the plane one here, I'm a create a sketch. I'm a create a corner rectangle from here to here. And I'm just gonna make sure that it lines up with those edges so it stays associated to that edge in the other, in that other component or that other feature. Now I'm I'm gonna set this to always be one eighty, and that's all I need to do. From here, I can create a base flange, and then make sure that merge result is off. That's the big thing here. Make sure that merge result is off so I'm not creating one body. And then when I click okay, I get my two separate solid bodies. That's one method. The other method that I I'll quickly show you is mirroring. So if I have a body like this, for instance, what I can do with it is create a plane to mirror about. So we'll do that here. Click plane, and we'll create just a a reference plane based off of that, that geometry. And one thing that I need to mention before I do this, actually, is if I go to my document properties and go to sheet metal, there is an option to create multiple flat patterns whenever a feature creates multiple sheet metal bodies. That can be turned on and off. Right now, mine's grayed out because I've created multiple bodies in this already. But you wanna have this checked so a flat pattern gets created for anything you, mirror. K? So from here, it's just the basic mirror tool. You click mirror, select the mirror plane, and then you select the body that you wanna mirror. Click okay, and there you have it. Alright. That looks good. So let's go ahead and talk about once we've created multiple parts, the next step is kinda understanding how to manage them. One of the first things you can do is apply materials at the body level instead of assigning a single material to the entire part. So we can assign different materials to individual bodies. This allows each body to carry its own material definition, which is important for accurate properties in downstream workflows. Another key part of managing a multibody sheet metal parts is flattening individual bodies. Instead of flattening the entire part from the command manager, we can flatten bodies one at a time directly from the cut list. And if you just need a quick preview, there's also a toggle flat display option to view the flat pattern without fully unsuppressing anything, which is pretty nice. So we're not forced to flatten everything. We just focus on what we need. And then lastly, is creating drawing views for each body. When working with multibody sheet metal parts, we can create flat pattern views for individual bodies using the select bodies option. This lets us place each flat pattern on the drawing separately, so it makes it easy to document in detail each component even though everything was was modeled together in a single file. So let's go ahead and walk through those real quickly. So I have an overall material applied to this component. If I wanted to apply a material to each body individually, I would open my cut list, find the sheet metal body that I want, right click, go to material, and then apply something else. And that would override my my global setting. K? That one's pretty simple. So we'll, look at the next option, which is to flatten the components. Again, pretty simple. You just right click the body, click flatten, and it's gonna show you the flat pattern for that sheet metal component specifically or that, sheet metal body specifically. K? You also do that by this one got hidden for some reason. Let's toggle that. There we go. You also do that by right clicking the components and then selecting flatten. That's also an option, which is pretty nice. Go ahead and exit that. And another thing that happens here is our flat pattern, folder will have two flat patterns in it. So that's what we're unsuppressing whenever we select the specific body is one of these two flat patterns. Alright. Now if I just wanna, right click one of these and just get a preview, I can right click and say toggle flat display, and it'll give me a little outline preview of what my flat, body or my flat pattern will look like for that body without actually having to go through the process of flattening it. K? So that's pretty nice as well. Now let's talk about drawing views. So I'm gonna go back to my cage here. And I'm gonna go ahead and create a drawing from the part. And let's say I have an isometric view here, but I wanna create views for, my flat patterns. What I can do is in my view palette, drag in a view, say, my top view here. And then I can select that view, and then I can choose select bodies here. I can, choose select bodies. That will bring me back into my three d model, and I can select which solid body I wanna create a flat view for. So I'll click that, and then I can activate my flat pattern. And now I have a flat pattern of just one of my bodies in my drawing, which is pretty cool. For this one specifically, I'd probably rotate it 90 degrees. Looks like my window for that moved on me. Rotate that 90. That looks good. Oh, well, that's okay. We'll leave it like that for now. Something happened there. But then I can just rinse and repeat for the next one. Right? So if I drag in my top view again, select it, go select bodies. I can select my shelf, Click okay, and then activate the flat pattern. Looks like I'm showing sketches here, so I would hide that before I save this. But there we go. We now have both flat, patterns on our drawing view. Alright. That takes us to the end of our multibody design. I do have ten more minutes of other tools and recommendations for you guys just to wrap things up. Again, thanks for for hanging out after the time is over. Alright. So let's take a look. First is I recommend enabling verification and rebuild. We kinda already talked about this. You don't wanna have this on if you're having rebuild performance issues like you you saw earlier. But in general, when you're doing sheet metal design, you wanna have this on. It performs a more thorough geometry check during your rebuild, which can help identify issues that might go otherwise unnoticed. Right? And this setting is located in the system options under performance. We already saw it, so we'll move on to the next one. Another recommendation is to use normal cut along with optimized geometry most of the time. Normal cut ensures that your cuts are made perpendicular to the sheet metal surface, which is important for accurate manufacturing, And optimized geometry helps to simplify those cuts as well. So let's take a quick look at how this works in SOLIDWORKS. Alright. So I'm gonna go ahead and open another demo here. So in this model, I just have a couple of of bins and a cut that originates from a sketch in the center here. K? Now in this cut, there's two settings, the two settings that I just mentioned. There's normal cut, and then if I activate that, there's optimized geometry. Let's take a look at what happens when I don't turn on normal cut. In my flat pattern, my cuts are gonna be angled, and I don't know of any laser technology that can do this. But and maybe it's possible. But generally speaking, that's not something that we want to to see. K? So that's the first thing is activating that normal cut, which I'll go ahead and turn on. And the next is optimized geometry. I'm gonna go ahead and leave that off, and then we'll come back and turn it on. But I just wanna show you what it looks like when it's off. So if I go back to my flat pattern, we can see that my geometry looks a little wonky Just by the nature of sheet the sheet metal calculations, we're getting kind of a wonky cut based on that hexagonal cut that I made previously. K? So let's compare that to when optimized geometry is on. Turn it on. Click okay. And we're gonna end up with a much more acceptable result as a result of turning that, that option on. K? It also makes minor changes to my circular cutout as well. K? So, again, I would recommend always having normal cut on and then playing around with optimized geometry. Generally, having it on is good, but, you know, your mileage may vary there. Alright. So I'll exit that and go back to our presentation. I would also recommend that you use design library features. So there's a lot of good stuff for sheet metal inside of the design library out of the box. We can also create custom, cutouts, forming tools, etcetera inside of that design library, and it's especially good if you're using the same features across multiple parts. So I'll just give you a very quick demo of what that looks like. Alright. So I have a a flat piece of sheet metal here. And in my design library, which is in the top right of my screen, I can go to the design library, go to features, and then go to sheet metal. And there's a whole boatload of stuff that's built into SOLIDWORKS out of the box. And just to show you what it does, you just click and drag it in. It applies it directly to your sheet metal component. You can edit the sketch if you wanna add dimensions to to locate it. I'm a leave it alone for now. Then you click finish, and it adds it to the component. It's very, very nice. And this is just a feature. I can pattern this. I can edit it if I really want to. It's very flexible. You can also do custom stuff. So if I wanted to do something like this, this is just a sketch that I have inside of, that that folder. And this one's asking for the center point or maybe not the center point, but, a reference point. And I'll select my sketch here for that, and then I can specify the distance from that reference point. So I'll say four and three to locate it there. I'll click okay, and that, places my sketch and actually use this sketch to create a vent feature. So I'll click vent. I can select my boundary for the vent, which will be my circle here. I can specify a couple of geometry properties there. I can specify my ribs, which would be this construction geometry right here. For spars, we're selecting our circles. And then for the fill in boundary, we'll select this guy here. K? I can click okay. That places my vent, and then, I can reuse that as many times as I want. It's very cool. Another thing that we have is forming tools. So forming tools allow us to create forms on our on our, our sheet metal components. So let's take a look at maybe a Lance. Here, I'll do a lance. I'll flip the tool, and then click okay. And what that does is it creates a cut and removes a couple of faces to finish that form. K? Forms can look like this. They can look like all kinds of stuff. They can look like a a dimple if we wanted it to like that. And, again, these are just features. I can pattern them and do whatever I want to them. And I can also create custom form tools as well. I won't show you that here, but, you can create custom ones if you have specific forms that you're trying to create over and over again. And speaking of custom forms, there is another useful tool called the stamp feature, which is relatively new to SolidWorks. It actually provides a simpler way to create formed features compared to the traditional forming tools, which you just saw. So instead of building out a full forming tool, you can just create a sketch, define a few parameters, and then quickly generate your custom form. So it's really fast and flexible. It's a great way to add stamped geometry to his, sheet metal part. So I'll just show that real quick here. I'll create a sketch. Let's do a hexagon. Now I would I'm you're not doing best practices by not adding dimensions. Right? You wanna fully define your sketches. But I'll go ahead and grab my stamp tool and then change my direction. I can change how far out this goes. I can specify an angle. So let's say 40 well, 45 is probably too much. Let's say 20. I can specify, radii for these bends. Say, one is way yeah. One is way too big. Say, quarter inch. That looks good. And then I can click okay. And it just creates that stamp for me then and there. So it's a very fast way of creating custom stamps. Alright. At that point, that's everything I had for today. So thanks everyone for joining. I really appreciate your time. If you have any questions, feel free to drop them in the chat here. I'll I will go back in and and take a look. I'll stick around for a bit and answer as many as I can. And if you think of something later, feel free to reach out to me, at the email on the screen here. Also, if you wanna see our next webinar, feel free to scan the QR code on the screen right now. The next webinar is SOLIDWORKS tips and tricks, mastering left and right hand parts the smart way. So it'll be good stuff. And at this point, I'll go ahead and check out what's been going on in the chat. Thanks, everybody. I'm glad, you were all able to attend today. I would send a heart to everyone saying thanks right now, but I would have to click too fast too fast, I think. Can we show a tab and slot on multibody to connect them together? I did have that in this presentation, Kevin. I did have to cut it. But if you wanna see that, feel free to reach out to me. I'm happy to show you to do a little a little meeting later on. Okay? Could you show us how to unfold a model that gets imported as a STEP file? Katia Creo. Yeah. John, if you want again, if you wanna reach out to me, I have a demo for that. I just didn't have time to put it into this. So feel free to reach out to me, and we'll get that set up. Can multibody sheet metal parts be converted to two separate single bodies for traditional can multibody sheet metal parts oh, yeah. So there is a way to do that, Sean. And, again, that would be, I believe, the save bodies command. So in your cut list, you would right click your cut list and say save bodies, and you can save those bodies to individual parts. Great question. That's a very, standard workflow whenever you're using a master model approach that we talked about for multibody design. Can you tell us when some of these features made it into SOLIDWORKS? That would take some time, Tim. You can find the what's news for sheet metal, for each year, and that will give you a better idea. But if you have specific questions on specific features, again, feel free to reach out. Thanks everyone for your attention and for all the great questions. Again, feel free to reach out to me with, any anything sheet metal, and have a great day.