Video: SOLIDWORKS Simulation: Bolts Beginning to End | Duration: 5448s | Summary: SOLIDWORKS Simulation: Bolts Beginning to End

Transcript for "SOLIDWORKS Simulation: Bolts Beginning to End": Okay. It looks like we have people filtering already. Yeah. Welcome. Welcome, everybody. We'll get started in about a minute or so. Hope everyone's having a great Tuesday. Taco Tuesday. Right? So welcome. We got a few more people coming in here. So we'll get started in about a minute. Give everyone else a chance to to come and join us for this, for the presentation. K. See, I will be, we'll be monitoring the chat and, the q and a as much as possible there. So Alright. I think we got a good I get a good you're doing. Yeah. Maybe we'll ready to go? Let's kick it off here. Sounds good. So I think for the camera controller, Enrique, we'll probably leave it on for the first few moments, and then we'll we'll likely switch it off here in a bit. Totally agree. Thank you for the help of recording. And then, audio, you sound great, Enrique. You're still picking me up okay too? I I am as well. Absolutely. Alright. Great. So let's dive right in. We got a lot to cover today and very little time as always. So starting off, my name is Sean Bentley. I've got with me my esteemed colleague, Enrique Garcia. So a little intro. Enrique, I'll turn it over to you for a moment. Perfect. Thank you so much. So as Sean said, my name is Enrique Garcia. I'm one of the senior simulation specialists here. I'm located on the West Coast out of beautiful, hot Arizona. Still a 100 over a 100 degrees here, so don't come. Not until mid November. A little background about myself. I'm a tanker by nature, a bioengineer, by education. Like to take things apart. Yeah. Just had had fun doing that as a kid. Took apart the family computer and, freaked my parents out, gotten grounded, but upgraded the, the computer. So definitely enjoyed taking things apart. Kinda fell into engineering just because it's it's naturally tinkering, and you have to be methodical. And so, yeah, that's a little bit about myself. I'm also a big advocate of education. I I taught high school band as a woodwind instructor for over 10 years here in the valley, in Arizona. Couple of bands, did clinics, woodwind clinics, and, marching clinics and things like that. So, lastly, big foodie, enjoy. We have a family business out here in Arizona. We own the Jewish Delicatessen. So, yeah, it's kinda a little bit about myself technically, technical wise. I, I gravitated towards the simulation products. I learned SOLIDWORKS in college, and learned what not to do, to be honest, and been learning SOLIDWORKS, through the prestigious school of hard knocks. Just learning it as I go along, which I think a lot of us can probably relate to that. And, once I jumped into the reseller channel here at GoEngineer and some others that I've worked at, learned all the best practices and learned to and picked up a and, discovered a few of my own. So whenever possible, we're we I'll I'm a bit a big advocate to show best practices for SOLIDWORKS and simulations. So it took me a lot of effort and, blood and sweat and tears to get this information. I wanna give it out as much as possible. So just a little bit about myself. I'll hand it over to Sean here. Go ahead and, Sean, give us a few words about yourself. Awesome. Thank you, Enrique. So briefly about myself, just, related to the content for today. Well, this is a continuation of, Bolt, a pardon me, a series for beginning to end from vibration, thermal, structural, and, this is the, this one's gonna be on Bolt's, getting started with Bolt's. So these are, projects that I've worked on throughout the years, to try to get information on simulation out to our customer base and, up to the general, general engineers too out there in the world. So, passion around simulation, and I've been doing this stuff for nearing 20 years now. Also generate, bit of bit of different content, a lot of different content pieces up there to just try to show different use cases, mostly again for simulation. So diving into our agenda for today, we sort of have 3 major chunks that we'll cover. We'll start off with some introductory materials and fundamentals of bolts. Then we'll move on to our main story where, we'll show a bolt hand calculation, kinda move up into some of the simulation tools, how to simulate bolts using things like the bolt connector, and different, levels. And then finally, we have sort of an appendix of different other, use cases for bolts. So here we'll we'll show Topics. Right? Yeah. Variety different topics that, that will will lead into, later on. So so to begin, what is a bolt? Bolt fundamentally is, in a way, nothing more than a spring in with a pretension, a pre compression on it. And with the the spring, when it gets compressed, it creates friction in a lot of these zones that holds the 2 parts together both in in tension, holds them together axially, but also keeps these two parts from shearing relative to each other. So, here we have on the left an actual spring model, showing with, with a sort of preload, crushing the spring down and and compressing the bolt members. On the right, we see a model of a bolt that we'll showcase later on in the presentation. At this point, I will hide my camera as well and, you know, maximize the layout here. K. Alright. Now, the bolt connector tool that we'll be using in this presentation is available in a variety of the different simulation packages, but there's primarily 2 of these packages where it can make a big difference. So narrowing the scope down a little bit for our presentation today, we're really just gonna focus on these couple of tools primarily. So simulation standard, which does we call we sometimes call it linear static for assemblies. However, it is capable of some non linearities and importantly, some contact nonlinearity that we'll be using quite a bit today and also simulation premium which allows you to do full nonlinear dynamic analysis. These are the primary two tools where we'll make a lot of use of these volt connectors. So next, what I'd like to do is talk about, our main storyline here where we'll walk through a specific example. In this use case where it's gonna be a simple example where we have just 2 bolts and a a, kind of a bending load applied to the end of it, and we'll run we'll solve it at at various levels here starting with a hand calculation, then I'll be turning it over to my colleague, Enrique, who'll show us, running a static study on it and then also a nonlinear full blown nonlinear dynamic with, a shock loading on this thing too. And we'll evaluate how how do these bolts hold up. To start with though, let me lay out this problem with a simple hand calculation. So here is the, fundamental dimensions that we'll need in order to estimate using some hand calculations, how these bolts will hold up. Now this is a very simple system, so our hand with hand calculations, we I think we stand a reasonable chance at coming up with good estimates. If this were much more complex with a lot more bolts, it becomes nontrivial. But even here, it's fairly trivial, but you'll see along the way a lot of, assumptions and some creativity. So to begin with, to come up with a hand calculation for this example, we I have to look at that load and then the shear loads, the shear reactions on those couple of bolts. And already right away, you can see that load a and load f have to be equal to load b. So we have bolt a and b, load b has to be equal to load a plus f for the forces in the y direction in the vertical direction to cancel. So we can come up with one equation to help us figure out what are these bolt loads. Another equation we can come up with is to figure out if this thing were to rotate, do a sum of moments as you might have done in an engineering status class around point a. We can see that b has a, a distance from a of DB and f goes the opposite direction and has this distance DF. So those 2 will have to balance and be equal if this thing is to stay in stack equilibrium. So we have now a couple equations that we can use to figure out our bolt loads. So rearranging this, we can see that we we can figure out what bolt b is gonna be because we already know our force, we already know these distances. So plugging that in, I we come up with an estimate for bolt b of £675. Now that we know bolt b, we can go back to this original equation where b is equal to a plus f, rearrange, and solve for also bolt a. Bolt a will have to be equal to £540 in order to keep this thing in equilibrium. These represent the shear loads that are acting on the bolt but notice I'm not accounting for the fact that that bolt has a pretension on it and will have friction as a result of that pretension and that friction between the member surfaces will help. It will help reduce these shear loads. So here is a summary. 135 on is our load, applied load on the right and there's a 2 bolt shear loads that we've come up with so far. But next, let's take into account, the actual bolt we'll be using, the amount of torque being applied to it and we'll make an assumption as to a reasonable friction factor in this hand calculation as well as a friction coefficient between the two members being fastened together. So in order to figure out what the ache seal preload is, we first start with, in this case, a torque. A torque of 24 inch pounds, pound inches here. And for those of you comfortable with foot pounds, it's about 2 foot pounds of torque. Now that torque, the more torque you put on something, the more axial preload you get on it. The equation that relates the 2 is going to be the torque divided by how much friction is in that joint. The more friction you have, the less axial load you're going to get, but also divided by the diameter of the bolt shank. Come, based on these, this 24 inch pounds, we'll come up with £600 of axial preload. Now the next question I wanna ask is how much friction force do I have between these two members before the two members slip relative to each other? And if we only have a coefficient of friction of 0.1, we can take our 0.1 and multiply by this 8 ciel load of 600 pounds to come up with an estimate for that friction load of about 60 pounds. Now here you can you can tell 60 pounds of friction force is a lot less than the sheer loads that that bolt is experiencing. So what's gonna happen here? The bolt's shearing at 675, we have only only a measly £60 of friction force to to try to hold the bolt steady, we're going to have slip. Now the friction will help with reducing that shear load. Here, the original bolt load which was 675, if I subtract off that friction force, I'm gonna get 615. From here on, I'm going to ignore bolt a, it's got the smaller shear load on it. We're just gonna continue our calculations just looking at bolt b from here on. So so when I look at bolt b, I see that if I subtract off that friction force, this is my currently my best hand calculation estimate for how much shear that bolt will actually experience. So we we've come up with 2 loads on our on our bolt b, 600 pound axial force, a 6 115 pound shear load on it. What about the bending moment? The bolt will also bend. If it's attached to the top and bottom, we could see the distance between the top and bottom for our two plates shown here, 0.5 inches. And since there's a moment on both sides, I'll divide this, these both both these moments help with countering the rotation the shear is trying to create. I'll divide this, calculation, the 6 15 by times 0.5 by 2. So I come up with an estimate for that moment, 153.75 pound inches of a bending moment. So now I have all my loads, all my bolt loads. 615, 6 100, and 153 for, for our bolt. What I can do next with this is we've developed a spreadsheet that will mimic some of the safety factor calculations that SOLIDWORKS Simulation does. If I pull this spreadsheet up and I plug in those same loads, the sheer load of 6 15, an axial force of 600, and what was that bending moment again, 153.75, I can come up with an estimate of a safety factor to decide whether or not this bolt will pass or fail. Additional parameters I'll need to key into this equation these equations are the how course the thread is and also the strength that I wanna use for the bolt, whether this can be a proof strength or yield strength. And based on these estimates, I'm coming up with a safety factor of only 0.32. So it looks like according to my hand calculation, our bolts in this situation, they're not gonna they're not gonna last. So my can calculation comes up with, shear loads, a bending load, a bending bending load, bending moment, and also an axial force as well as a safety factor. Let's now turn it over to Enrique who's gonna run a simulation with a lot less creativity involved in trying to come up with all these hand calculations. He'll be able to be much more direct and and, run the simulation and get some, potentially even better estimates of what's going on than what my hand calculation could have possibly shown. So, Ricky, I'd like to turn it over to you now. Perfect. Alright. Let me go ahead and share my screen here, everybody. Alright. So, effectively, we're gonna be reproducing what Sean did here using SOLIDWORKS and the tools available in SOLIDWORKS Simulation. So then we can start at that particular point where Sean left his hand calculations, start iterating, start working with, these numerical methods we have with our solver to start to get more mature results. We can start looking at friction, other additional result conversions factors, then we can start talking about, nonlinear responses, linearization of the response as well. And so that's that's the goal here. So let me move this out of the way. And and my goal is to to show you how we can step through this step by step so you can see the workflow. For those of you that are new to SOLIDWORKS Simulation, you'll be able to see what this workflow is going to look like. And for those of you that have been using this tool, we can just, get a little more granular look at bolts in this case. So let's start by creating our first static study in this case. I'm gonna go up to my my new study icon here, and let's start a new static study. We can call this one hand calc replication. And the way I approach setting up SOLIDWORKS SOLIDWORKS simulation study is I address the folders from top to bottom. In this case, we can look at assigning materials to all the components here. The materials database in simulation is the same exact database we have inside of SOLIDWORKS CAD, so there's no need to go in and flip flop and maintain different databases. In this case, we're gonna be applying a AISI 304 steel. We have a yield strength, which I'm gonna make a mental note of here for that. We'll hit apply and close. Apply that steel here. We have some feedback simulation. Works with great feedback. We can see we have a little green check mark indicating that we have the material already selected in there as well. So that takes care of the first folder. Let's keep on going down to connections. Connections is how we can go in and address how the model is gonna be respecting the different components, boundary conditions between them or interactions between them, contacts, etcetera. So I'm gonna start here by assigning a contact interaction between the two components. So this way I get, some reaction force is pushing and pulling between the components there so it's more realistic. So I'm gonna go in and apply. You can do this in many different ways. I'm choosing to apply this just locally on the 2 contacting or interacting surfaces here. I can go in and pick on one of these faces for 1 and then pick on the other there. Down below, we have some settings, that allow us to, maybe help Armwave small gaps and things, especially if you're importing geometry, that, maybe or you have some unintentional gaps or some well gaps if you're doing, like, weldments, for example, so that we can still detect things that are non touching exactly. It's good so it's more of a kind of tolerance of these contacts, if you will. But, also, we can start to now add the coefficient of friction. So just to kind of simulate, or to be as equivalent as possible to Sean's calculations, we're gonna enter a point one friction coefficient case friction coefficient there for that. Although, I'm gonna click okay on that. So that takes care of our contact interaction. Let's now focus on the bolt feature. Once again, I'm gonna right click on this connections folder, and we have this quite a bit of different virtual connectors or or or fasteners that we can potentially add to the model. The one we're gonna be looking at right now is the Bolt connector. So Bolt connector, there's many different flavors to bolt connectors. If you decide to change your mind on the connector type, you want a pin or you want another type of connector, you can hit the pull down on the fly in the property manager to easily switch and change your mind. We have different ways we can apply these, bolt fasteners. We can do foundation bolts or some with specific threadings. In this case, we're doing a, a particular standard, with a nut down to tie this thing down. And so I'm gonna go in and just start with my first instance of these holes I have here for the two components. I'm gonna select that particular edge there where the the the head of the the nut or the fastener will meet the surface when I click on the next box. And SOLIDWORKS Simulation tries to be intelligent here, and it looks at the stack of components. And it noticed that there's just an ending to that stack, so it automatically selected that edge. Again, it's it's a great way to we're trying to make this a as as streamlined as possible, so it helps us along here. Down below here, because we're working in English, I'm gonna just switch my units there to English. My current template is set to, SI units just like in school. But, again, you can change that in the in the in the settings globally, or you can change them on the fly like I'm doing here. So you can work with multiple engineering teams. And, I'm gonna make sure that, I'll stick with, with what we had here for the shank diameter of the holes, nominal hole of 0.2 inches, and the head diameter of 3. We're gonna be exploring this in a little bit. And, actually, just to give you a a little foreshadowing here, ladies and gentlemen, the the shank diameter here, we're entering and it's intuitive to enter the actual nominal shank diameter, but we're gonna explore this a little further towards the end of this presentation. We've discovered some interesting information. You're gonna wanna know about how to enter these shank diameters. So it's gonna help with accuracy. So keep that, for a little for a little little little later. Also, we have the connection type. This is how the head of the bolt fastener is gonna be related to the surface, you know, this contacting surface of the model. There's different techniques to this. We will explore this a little bit further, but there's also something that's a little bit interesting that you should know about these 2 coming along. We'll just kind of pick something for now. We'll pick this rigid, option for now, but, we'll we'll expand on that a little later. Next, let's talk about the material. So we can pick any kind of material for our virtual fasteners. If I click select material, this will open up the regular database that we're used to now looking at. We can pick anything in here. I've had customers that needed, resin fasteners as well. We can do that as well. We can make any kind of custom material as well. Everything is fully open that you're used to when it comes to the material database. So we're gonna be leaving the allosteal fastener there for this. Next, let's come down to the strength data area. This is an important area to consider for what we're wanting to do for grading this bolt in a moment. So the first thing I wanna do is I wanna make sure I put in the thread count here. And so maybe I want this to be threads per inch, and I believe it was 10 threads, I think. Right, Sean? I'm gonna be popping in 10 threads per inch here to kind of mimic what we were seeing in the hand calc. The bolt strength is grabbed directly from the materials database. And then we have a a factor of safety or safety factor, multiplier here. So for us, because our goal is to see if these bolts are gonna pass or fail. And in this case, the the failure criteria is going to be the bolt strength in this case or the yield strength of this material. So what I wanna do is I wanna switch this to 1, a factor of safety or safety factor of 1 so that later on when I grade these bolts, I can see a very clean pass or fail. There'll be a nice, feedback that you're gonna be able to see here pretty easily. So this is my best practice if you're gonna be grading the bolts here using this virtual fastener technique. Lastly, let's talk about this preload. We're gonna be putting in a preload. Again, we're picking English just it's a little bit easier. And so we have it an inch and pound inch, and that was 24 or about £2 there, but £24 inch. And, we'll leave the the friction cofactor there of point 2 just, just for for sake there. Now after we've gone in and we've set up this particular bolt, because we're in the SOLIDWORKS ecosystem, it's connected to the CAD software. There's intelligence behind this. So whenever I click okay, the software is gonna notice that this hole is part of a family of holes. We call this a hole series in SOLIDWORKS. It's gonna say, hey, Enrique. We see that we have other instances. Would you like to conveniently add this instance or this feature to other instances of the feature of the whole series? So I'm gonna say, yeah. So this is gonna help us with, again, redundancy. This is gonna limit human error quite a bit. So it's, it's something that helps us streamline these small redundant tasks we have in simulation. Alright. The next thing we're gonna do is finish this setup here. We're gonna go in and, stabilize the model. We're gonna be applying some boundary conditions, in this case, fixing the the, the this plate so that it doesn't, float around in the space. We're gonna be applying our external load here, and, we'll see what kind of results we get from that. So when I quickly just add some some fixture features there just to limit all degrees of freedom on that surface. Next, I'm gonna come down to my external loads folder and just apply a force in this positive z direction in the area here. So I'll click on the cylindrical face. Now we need to specify the direction vector. There's many ways to do that here with, using, the the geometry of the model or if you have reference geometry from the CAD, the CAD feature tree as well. But I can go in and specify that with, like, a a plane or or some other reference, or I can just kinda do do something quick and dirty and pick an actual edge. It's only picking the edge for the direction vector for this initial geometry, so there's no worry about having that change during the course of calculation. So we have that direction vector specified. We want it to go in the positive z direction. So let's flip that direction around. And, again, we're picking English in this case, so let's pop in. We had a £135 force on that on that particular surface. Now, again, this is a very simplified preliminary setup we're still setting up here. You can get this you can get more, accuracy with your setup, with maybe putting a bearing load, working with, with some other advanced settings, in general for the contact. You can play with friction. There's a lot that can be done. But, again, we're trying to keep it simple so we can see what the hand calculations are here to to see what we what we get. At this point, the last thing to do is to discretize the model and apply a calculation mesh on this. We're just gonna stick with kind of default mesh settings here. We do have ways to simplify the mesh. We can do simplify features to get rid of small detail oriented features. That is gonna cause, extra calculation resources, in terms of the mesh size. So in this case, it's a simple model. It's pretty small. I am going to show the results here. I've done run this. I did run this already. So let's take a look at this hand calculation study. And let's take a look at these results. So this does take a couple minutes to run, which, again, our time is a little bit short here for us this, today. So I wanna go ahead and maximize our time here. And so let's start by looking at some some some results. We can look at a displacement result there. We get, displacement about 1.2. We can do much to interrogate this both qualitatively and quantitatively. My favorites to show is something called ISO clipping or isolation of the magnitude of whatever you're showing. In this case, something that can be valuable is looking at the yield strength, popping in that as maybe your cutoff, maybe 206, so you can see which regions of the model's response are gonna be going and hitting the yield strength and above. And then we can determine if these are gonna be a little bit on the artificial side. We can see if we're reaching any, singularities or if indeed these are truly, more mature results. But we can kind of do some exploration of maybe how the model is gonna be responding using ISO clipping as well. But it's a great tool to kind of spot check, and sometimes you may find that you're not gonna be able to see the areas that are gonna be failing. And this can kinda isolate that so your eyes will more easily get to those areas. As far as interrogation, yeah, we can go in and use, maybe the the probe tool as well where we can go in and probe different regions of the design here. We can see what those are. We can get close to the the regions around that particular, nut and bolts, virtual nut and bolt. Now as far as results, we cannot see actual stresses, strains, and displacements on that these virtual connectors, but we can get some information here, which I'll show in a moment. But but, yeah, this is there's some ways we can interrogate the general results around the fastener. Something else I I like is maybe the selected entities technique where I can select edges, and I can collect all of the data around maybe a certain path if you wanted to specify a path that was specific to some some workflow. I can collect all the data around these edges or paths, and, I can get some information about that, or I can kinda see the trending in this case, what the stress distribution is gonna be here along these areas. You can map some trends. So let let's focus on the Bolt here a little bit, and, I'm gonna get some I wanna get some comments from you here, Sean. I wanna see what we get. So when it comes to Bolt, forces, we can go in and right click on the results folder, and we can choose a utility that says list connector force. Now this is gonna show us all of the virtualized connectors that we have access to. In this case, the default is showing all of them. And here we can see right away that the connectors are broken down into a couple of different forces, individual forces, and we can see that the coloring or the highlight is set to red. That indicates that the the actual factor, the the, the safety factor that we specified in 1 is being violated, meaning that the failure criterion is gonna be less than 1 in this case or less than yielding. And so in this case, let me switch this over to English. And, can you remind me, Sean, what what you were seeing there for your for your your responses? So let's see. Your bolt b I had bolt a and bolt b. Your bolt b, I think, is number 4. Right? If you click on any one of those, it might or alright. So that's gonna be the sheer load should be £615. Okay. And you got Pretty close. 16. Yeah. Real close to my hand. 14. Load is 600 and you got 596. I'm gonna say that. And the bending moment I came up with was 153.75. Oh, right now that's really close, man. Wow. Okay. Very nice. Yeah. Yeah. So I I mean, we're we're we're barking up the right tree. Right? But now everything that Sean has done, right, it's, there's a lot of work to this, but we did this in a couple of minutes right from scratch doing up the setup here. And now the beauty of doing it this way is that we can start to iterate. Right? And we can go in. And, if you look here on my my my next kind of iteration, we can work with mesh controls. We can adjust the, additional items in in the Bolt series or some other advanced options we can go in and work with. We can maybe adjust the local interaction a little bit as well. We can we can maybe adjust if you have small gaps and things a little further, play with friction to be a little more realistic. I if I remember just kind of looking around, dry, dry metals or dry steels, I think, has a friction coefficient of 0.3, so we use 0.1. So we can start to play with these settings and start to make these results a little more mature. We can also adjust the way that we apply force loads. Instead of doing just a force acting on this inner cylindrical face. We can maybe maybe put in something that's more more, parabolic when when it comes to maybe a bearing load acting on half of this design as if maybe there's some sort of pin pushing in the z direction. So we can then start to You know, I think we need bigger bigger bolts or more bolts and more preload so the friction will help us out so we're not experiencing so much bolt shear. That's that's what I'm leaning towards. And yeah. So yeah. And the idea here is so so we've been using a nonstandard size. Right? So let's take a look at maybe increasing that size. And here, this is again the the I think the main meal ticket to using simulation is that we can go into the model itself, we can make an adjustment, and we can add another configuration. In this case, a quarter 20 fastener can be represented. And, let let me show you what that looks like here. So I'm gonna go in, and I can easily just quickly activate that configuration. The, hole size is gonna change to a quarter quarter inch. And, let me show you what I've done to set this up. It's nothing out of nothing different except for going into the the bolt fasteners and adjusting those to be a quarter inch for the diameter here. And for the thread count, I went down and made that 20 threads per inch. So that's all I did there. So let's take a look at results now. Let's see what an increase in diameter. And, actually, this this kinda helped me kind of as we're learning as I'm learning more about bolts, the fact that the finer the thread and Sean can maybe comment more on this as well. The more finer the threads, the better results I'm gonna get and the more robust the model is gonna become in this case. So we can see here as maybe the the diameter the the overall diameter of this model is is larger, but also the thread is finer, meaning that the root, of that, thread is gonna be out further further further out and radiate out further because of how more how much more fine that thread is. We're gonna have a better larger effective diameter here. And so we can see that being reflected in the results. So we can see we went from a fail to a quick pass when it comes to these, these these to this bolt feedback. We think is there anything else you'd like to add to that, Sean? I'm trying to think if there's anything I'm missing here that we can show. Mhmm. Yeah. So I think you're about to ready to move on to the dynamic part 2 right now as well. Is that is that right? Or Yeah. Yeah. Let me let me do a little bit of a primer and then, there there was one more thing maybe we can show on this too. Let me, borrow the screen from you. Sure. Alright. So here was that comparison. Now this is this is me taking Enrique's same out running in my session, just to put them side the numbers side by side. So the numbers may vary a pinch, when I ran it. Maybe slightly different mesh, slightly different solver, but all within rounding errors. And then, one more thing I wanted to show as well, let me pull this up, is very similar to the spreadsheet calculator. There is an option for salary simulation to report a safety factor as well. Instead of using the list connector force, which is a really really handy tool that lists all the kind of forces going on in your model, if I use this to find pin bolt check plot here, this will report the calculated safety factor that SOLARK simulation comes up with, and and I and I do have access to the same, loads. Here's the the shear force, the axial force, the bending moment, and and also in red like, Enrique had showed there. And if I put this stuff side by side, here was my the safety factor for my hand calculation, 0.320 and from SOLIDWORKS Simulation, 0.321. I mean, fundamentally, it's the same loads so it should be pretty close, I would think. So next what Enrique is gonna show you, is some dynamic studies using SOLIDWORKS Simulation Premium. So this will allow him to apply some impact, sort of a shock loading and see vibration issues as well, potentially. So, so, Ricky, I'll turn it right back over to you here. I appreciate it. Let me share my screen. And so let's jump over to this next simulation study. Again, this is gonna be using a nonlinear dynamic study. So this is part of the simulation premium package. And so let's say that before, right, we were working with the the the quarter inch, the quarter 20 fasteners, and we had that force load being applied, that same force load of a £135. But let's say now instead of applying that statically, right, we're now gonna be applying it as a shock load. So it was passing before. Let's see if it still passes with a shock now, a shock load of that same magnitude. And so for this, we're going through and, let me just show, I guess, the the force load anyway. That's the main distinction here. So let me show what that's gonna look like. And so, again, what I'd like to what I'm showcasing here is the fact that we did that same workflow for static studies. Right? If you're familiar and comfortable with that workflow, you can apply that same workflow, I would say, 99% of that workflow to this dynamic study. The only thing left to worry about is some of the the nonlinearity aspects of these of these tools, but the setup will be exactly the same. So so the, the learning curve is not that crazy when it comes to going and and getting going from a static study to a more advanced simulation study. So, again, this is a force, force feature. And if you look go in towards the bottom here, we have a variation with time section. And all I'm doing is I'm telling this particular magnitude what to do with a with basically a multiplier here. So I'm saying from 0 to 0.011 or 11, 11 milliseconds, I want it to basically scale up linearly up to a 100% or a factor of 1, so a 100 to a 135 pound force. And then instantly go ahead and shut off. And then for the remainder of the 22 milliseconds of this whole, study, just kind of let it not be a play in the factor, and let's see what happens in the end. Can just let it jiggle and hopefully dampen down. Right? So that's the idea. So that's our shock load that we're gonna be applying to this thing. And so let's take a look at some results on this. I guess the first thing I like to look at, since Sean was showcasing the the the pinball check plot, let's check those out here next. So we went from a passing bolt, and I can right click and say define pin bolt check plot. And because we're dealing with a time domain here, I wanna make sure that I'm looking at the time domain at that, 100% loading, which was 11 milliseconds. So let's type in 11 milliseconds there. Let's take a look at my results at that particular point. So we can look at the details here. We can see that they are not passing again. So we can see here that, yes, First guy here is not passing. And if I go back, I think I hit that. Let me bring that back up here. But if I look here, we can see that we're our factor of safety there is under 1, And they're both on 1 here. So we can get the the direct calculation of your factor of safety, and we can find out the details for each individual bolt here as well. So it's not passing. We can also because this is this is a response due to this time domain that we're dealing with, we we can interrogate a little bit further along. We can maybe we can show stresses as well. So here's a stress plot here. I've sectioned the model in half so we can see the response. And the the response is, pretty the same as before here, when it comes to, the the respecting the geometry in these areas. We can maybe do a little animation as well for for this. This is a great place to start maybe for a design review, showing an animation of this and figuring out what is how we can fix this, whether that be addressing the shock load parameters or maybe changing the way that the model is, is set up. Right? Do we need maybe more robust fasteners instead of quarter 20 to make these? So do we need to increase the the torque? That's a factor. We can play with that pretty easily by just editing the feature. Also something just to confirm that this first peak force magnitude is what it is. Maybe we can go in and do what we call a response graph. So maybe using the displacement graph, I can come in here and, I can use some of my interrogation tools, in this case, the probe tool. And I can select that particular, maybe maximum displacement area, and I wanna see what that is that displacement is as a function of this response time. So, again, my calculation domain my time domain was only 22 milliseconds, but that gave me enough to be able to get maybe 2 wiggles of this of this response. Right? So I can see that the magnitude is still higher at the 11 millisecond, times time step than the second time that the actual part of the the, of of the of the middle piece swung in the opposite direction. It's much less than before. So I can easily say that that is the highest magnitude, in which in which case, I I'm I'm just looking at the right time step. I can verify that by maybe jumping back in here, right, and and maybe editing that time step and either specifying that at 11 milliseconds or instead of going into a response graph, maybe you don't wanna do those extra steps. You can go in and tell the the, the plot here to look at the entire, the entire dataset, for the entire domain and just pick the maximum or in this case maybe the minimum. You can pick which one you want to display, and then we'll get the data from that. So it'll it'll go in and crunch through and and, parse through all that data and give us the maximum values. So that's that's kind of what we're looking at when it comes to using bolts in SOLIDWORKS Simulation. Now, throughout this whole journey of exploring bolts, Sean and I were we found many different little caveats and interesting, pieces of information. And at this point, we'd like to maybe share a few of the, of the gems that we found, some considerations you may wanna make when it comes to working with simulation and bolt connectors specifically. Let's say that I wanted to look at a linear dynamic study. And if if you look here, I'm gonna open up this linear dynamic study. And a linear dynamic study, if I were to go in and try to add bolts, we can see that we don't have bolts that in this particular, selection set or this area. The reason being is because we're doing now we're dealing with, with modal analysis and it's just not a supported feature at the moment. So to kinda get around that, we still wanna get the response of a bolt in the maybe a linear dynamic analysis so that we're not maybe maybe the the materials are not plastically deforming. There's no need to do a full nonlinear dynamic analysis, and, everything is fits within the, the elastic response of the stress strain curve. So you may wanna still approach the model with maybe a linearized response with a linear dynamic study. So there's a couple of approaches. There's a couple of ways you can do that. One could be by experimenting with the load transfer without virtual fasteners. Let me just share this slide here with you. So the first way is I'll show this with a static study, but the same technique can be applied with a linear dynamic analysis. And the idea here is that we're going to be representing these bold transfer points with an edge to face bonded interactions. Also, there's a couple ways we can address maybe the the axial response of this, of this of this fastener. One way maybe if you're doing preloads, you can maybe split up the model up a little bit by using the split line function, like we've done here, and figure out what the field is for the for the response. Maybe make an assumption of what that's going to be. We do have some more information here about how to approach that or what that radius size could look like. So we have some some some maybe some best practices, if you will, of how to potentially approach this range. But let's kind of step through this here. I did an example with with Nobles where let me let me activate this, and I can go in and we can look at my, my local interactions. And the idea, again, is this is a little bit of an assumption we're making. We have to have transfer of our loading through the model, and so I decided to try this out with an edge to face bonded interaction between these two components. Again, it's a little bit of a hot area. We're gonna get some localized, a bit of an artificial response there, But the idea is to see what the response is overall around the rest of the the geometry and to get more to get an accuracy to get an accurate load transfer through the geometry is is the goal for this. So I so we're doing that. And then to apply the preload, I went ahead and I I, I took whatever the the preload, the axial loads were for for for one of these instances, and I I divided that by half. And that is what I've put in here as a just a force load on these segregated surfaces, but on both sides of my structure there. So this is simulating the bolt head and the nut kind of going in and compressing and having a torque, kind of compressing the model in this way. Just to get, again, qualitatively, the the response that I'm that I would like on that. The last thing I wanna comment on is we're using the SolRx feature called split line to split this service. It's a very very straightforward feature. It's gonna be accessed in the parts, feature set, and, you're gonna go in and create us, in this case, a circle of desired diameter and then you'll initiate the feature and you'll pick the face you want to segregate, you'll click okay, and this is how we ended up with some splits there. And I can show that later in the in the q and a section if you'd like, at the end of the presentation. But, look up split lines. If you've never used them, they're very useful for us analyst simulation. That's a SOLIDWORKS functionality. But then in the end, after that, we can look at, some stresses, some displacements. Again, we're we're looking at the regions around the area, and we can see that we're we are getting a bit a bit of artificial responses in the exact area of the bond. But surrounding the area, we'll start to normalize and, it's a very isolated response that we're seeing in that area. But everything else is quite comparable. If I look at the stresses here in a moment, I can probe some of those. But if I'm looking at displacements here, I'm seeing a maximum displacement of about 6.6 millimeters. I go back and I compare to my my model with bolts as well. I can see that we have, you know, 0.6 for this workaround approach, and we're getting 0.57 millimeter displacement with the actual virtualized bolts. So, again, pretty comparable. And this is, again, a technique you can do in a static study like I showed or apply it in a linear dynamic study. So that's that's one workaround around, not having bolts. The other or actually, here's another example here for stresses. I went in with the probe tool and I just probed a little bit away from the hot region there of the artificial stress, and we're seeing pretty comparable results around the area with the actual bolts and with my current vignette or work around that I just showed here with localized contact localized bonded interactions. So again, it's not ideal. This is a good for a preliminary pass of a response, but it's it's something that you can potentially do as a setup. Something else we can show is using virtual pins instead. So this is a second technique we can use with a linear dynamic analysis if you need to go that route. Here, bolts are going to be represented with pin interactions. We can do a pre an axial load can be represented with those compressive forces like I just showed. You can also maybe address the response or the the stiffness of the of the pins material, in in an area here I wanna showcase in a moment. But, let me show you what that setup looks like. So let me click on this linear dynamic analysis, and I'm gonna jump into the virtual pin. And that's the main feature I wanna showcase here. So instead of the bolts, I'm I'm applying a virtual pin. It's a much simpler fastener, and the way we we we implement is we apply we select the inner cylindrical faces of the bore of the holes in this case. And you can do, I forget how many. There's there's there's a there's not much of a of a limit for those. I've done, I think, up to 10 in the testing of stacked parts. So you can put as many as you'd like in there, it seems. So I haven't found a hard limit at the moment. But now at this point, I wanna make sure that I'm I'm simulating the bolt and the nut and the threads. I want them to be fully engaged. Right? So I'm doing that by turning off the rotational degree of freedom with this particular check mark. Now we, and at that point, we still have an axial stiffness that we can represent. I currently left it at 0, but something you can do if you're gonna be worrying about maybe the response axially, then you can maybe put in, something that's representative of maybe your material properties in here. Let's say that this is still the alloy steel material. We can maybe put in an elastic modulus times maybe the cross section area of that circle, and then then divide that by the length of that shank diameter to give you some sort of stiffness, to represent the material in there. That can be something that you could potentially do as maybe a second pass to add more accuracy to this model. But that's that's what I've done here. I've I've implemented a partial vault by doing a pin a pin feature in that. I've done the same thing with the second instance there. What else? That's that's essentially it. And in this case, I decided to add the the preload here with the with the sectioned faces there with the compressive forces acting on both sides. And, yeah, let's take a look at some results. Maybe the first thing we can look at is the stress results. We can see here that the results are showing a kind of that hour glassing behavior in the similar way that the virtual pins did. I have an example here. I took some screenshots for you. So we can see here the I've I've exaggerated this a bit more on my virtual pin, but we can see that kind of air glassing effect that's happening, or that zigzags or sawtooth effect that we're seeing. And we're seeing that here as well. I didn't exaggerate it as much, but it's just a matter of post processing. We have full control over the magnitudes and how that looks. So so that's pretty comparable result wise as well. I did some spot checking here. We can see our our our values are pretty comparable when it comes to using as far as the response of the geometry around these virtual pins versus the the virtual bolts. So pretty comparable results there. Something also that I wanted to take into consideration because we're doing modal analysis with this model, the the the the pins, right, that that we're that we're representing here, is kind of an intermediary to 2 very extreme situations. Right? So we talked about the first static study with the edge to surface bond. Right? That assumes maybe that the other areas of the geometry are not gonna be bonded together, they're free to respond. The other scenario could be where this plate is completely fused to this secondary metal bar here and that again is the other extreme situation of bonding that we can kind of simulate in SolidWorks. Right? But when it comes to actual bolts and fasteners, that's somewhere in between. So I wanted to kind of verify that situation. And, I went in and I did a couple of frequency analyses to see what the resonant frequencies were where I when I went in and I bonded the edge to surface or when I bonded the full plate to full plate. And then I did a frequency analysis to see what the resonant frequencies were for only bonding the region with those virtual pins. And these are my results that I got. So again, very, very acceptable as far as the responses for the for the for the modal analysis. We can see the edge to surface interaction or or or bond here. We got about 40, 400 hertz, and then, the more the other extreme case was that the plate with the whole bottom face being fused, that gave me for a first resonant frequency of about 900 hertz. And then using the virtual pins to kind of help, justify this or make it something that could be more realistic, I could see that that was kind of somewhere in the middle to that, about in about 600, hertz. So, again, that's similar to what we are gonna be expecting with the bold fasteners as well. There's it's a partial rigid rigidification, is that even a word, of the actual response there. So, so, yeah, those are the 2 kind of vignettes or kind of, workarounds, showcases I wanted to share. I guess I'll take I'll get let take it back to Sean and, we have some additional, very specific kind of, explorations we'd like to share with you here as well. Let me, switch over to to Sean's screen there. Mhmm. Let's see. Screen. Also, as we're transitioning, I understand we have about 3 minutes left here for our official time over. But, if you guys do need to, leave early, we we wanna respect your time. These recordings this recording will be archived and put on our YouTube channel soon enough, so feel free to catch the end of it there. If you guys are, free to stick around, we have some really interesting tidbits here to share with you. Yeah. Some of the stuff we'll be covering, probably be about another 20 minutes worth of content. A little more on linearization. You'll see, modeling bolts as a solid model rather than using the bolt connector, the difference between rigid and distributed, discussion on tensile stress area, and then some advanced simulation considerations. So if you guys can stick around, great. If not, thank you for coming and just check for the recording for some of these other topics. So to pick up though with, where Enrique left off, we talked a bit about linearizing bolts, and I want to share a little extra on that subject, really stress the point of how important this concept is of linearizing your bolt connections. So, as Enrique talked about, why do we even bother with all these linearization techniques? One of the big reasons is solve time. When you run a study with with sliding contact, here's a static study on the left. It takes it's pretty quick, but it takes about 2 minutes 32 seconds. If you think, bigger picture, larger assemblies, this can be hours, days even. Versus when I take the time to linearize it upfront, I take that 2 minute 32 seconds solved down to 2 seconds. Huge potential time savings. It simplifies the solve of the analysis immensely when you can when you can linearize your bolts. Another motivation that Enrique, covered as well, of course, is that the bolt connector just is not available with some studies. Frequency study, linear dynamic, it's not available primarily because contact, sliding contact is not available. Sliding contact is a nonlinearity and nonlinearities don't factor in to a linear dynamic study or to a frequency study which is also a linear study. So a couple of motivations to help reinforce a lot of those linearizations that Enrique talked about. So those two ideas, faster solve and also supports these linear these linear studies such as vibration analysis. So how do we linearize bolts? Enrique gave a great presentation that can showing some different comparisons of, of how how a variety of methods in order to do this. One extra method I just wanna showcase was considering when you have a bolt in in in compression, it creates a compression zone, and this compression zone is a region of high pressure. And if the axial force is a lot, the friction force will be a lot. So this zone here we if we can assume no slip to that zone, this is a primary candidate for bonding. We can just bond together this region and not use the expensive sliding contact. Another way to linearize that Enrique, mentioned was using things like pin connectors, but also spring connectors are a great way to linearize, bolts as well. Here I can add a spring, even key in attention preload. As I showed in the very beginning of our our presentation, bolts are fundamentally springs at their core. Now these two techniques, revolve around, pardon me. If if you use the linearization technique that we describe, both of them, the spring and modeling the frustum, Here's the difference that we can get between 2 studies. This one has that 2 and a half minute run time. This one has a 2 second run time. The displacements the peak displacement is almost identical. You can see some local, the way the thing bends and twists is a little different, but it gets very close to the same answer under the same loading condition for just things like displacement. So just to show the frustum approach briefly, to illustrate how that can be done. Here we have our model that I'm gonna attempt to linearize. And one way within SolidWorks that you can, create this frustum, and there are many ways, but, one simple way would be to start by moving a component a little bit, separating these components with a, a very small gap. So I'll use the move component command here. That way, when I attempt to combine things, it won't combine any more than just that frustum region that I construct. So now there's a small gap, then I'll draw a, extruded shape, draw with that that head diameter here, which in this case might be around 0.4. And then when I do the extrusion, I can do it as a blind extrusion or actually just go up to this surface here and then add a draft to it to create that frustum angle 30 degrees. K. So now if I take a look at the if I don't merge it, I can take a look at the shape that that creates behind the scenes. So it'll create that contact zone in here. If I were to merge these bodies together then it'll be all be bonded as though the joint as though the bolt were doing its job. Now, of course, it's worth sacrificing some detail versus just using the bolt connector such as things like the actual preload, but that preload is being simulated by the fact that I'm bonding those surfaces together. The preload creates that high friction zone similarly. What's also, nice about this technique is that if I created the bolts using the hole wizard, there's a bunch of points here, and I can, just do a sketch driven pattern using those points and pattern this body that I created around those to very quickly linearize all the remaining bolts. And when I combine them all, it's just doing like a box select here. Now, oop, I just need to add that other back body to this as well. And now if I look inside of here, you can see that they're joined together in these regions here. Now this does have a potential downside of, yes, that we'll have to squeeze a mesh between there, but, SOLARK simulations curvature based mesh is pretty robust at handling that at low detail. Now also if we run a dynamic analysis to compare those frequencies using this similar approach we can see that, if I run the full non linear dynamic with bolt connectors in there I get a natural frequency of 200 Hertz versus if I use this linearized technique and run this using a frequency analysis, it is a little different. It's a little stiffer using this approach, 232 Hertz as opposed to 200. So since we can't use in a frequency analysis, since we cannot use the bolt connectors and contact directly, we do need to come up with some form of simplification. Alright. So that's a little more on the linear eyes. Next, what I'd like to talk about is, solid modeling bolts. Sometimes this higher level of detail of actually modeling the physical bolt, it makes sense. So I wanna compare results of a bolt of using the Sauer simulations bolt connector to actually physically modeling the bolt. So in this example, I've got my direct bolt model. It contains several special features that I've constructed in it. Some you some may you may want to add, some you may not need. Here's an example is that that 30 degree frustrum split body. This gives me a zone about which I can apply mesh refinements by actually using the split, not just split line, but the split feature in Sourczyk to split the body using a surface. I can refine the zone and that gives me better accuracy around the bolt. I have a shrink zone on the bolt shaft. Now the way we model this shaft so that it shrinks and creates a preload is we can use temperature, thermal expansion. We create a custom thermal expansion coefficient for this region of the body and we could even make it orthotropic so that it will only expand and contract in the x direction. This is the bolt direction coordinate system, and you can see the x is the axial direction. After creating that shrink and applying a temperature pardon me. After applying that material and applying a temperature load to the bolt, we can see that we get the desired shrink effect creating our bolt preload. Another feature that we can add, if we expect the bolt to slip and that's a feature that we want to simulate is some slippage, we may want to model part of the thread so that the thread engages with the wall. Here shows an animation of what happens when the bolt slips. We see a quick jump from one position to the next when the bolt makes contact with the wall and we see this as the increase the shear load, the load is pulling this top plate to the right. As that increases the shear stress through the bolt is increasing. Here's a same animation, shown with both the compression and the shear load being applied at 2 different scales, true scale on the left and a 100 x scale on the right. You can see of course when we exaggerate by a factor of a 100, the bolt after the slip occurs, the bolt looks like it disappears off screen because it jumps to a new position. The true scale on the left shows a better representation of after that slip occurs. Also here's the same animation at 10 x and what I want you to pay attention to is there's sort of 2 slips that happen. The first slip happens between these two plates right about now. Then the second slip happens between the the head and the top plate. You see it holds on for a longer period of time up here near the head and then slip then the full slip occurs. So we sorta have 2 stages of slip, a half what I'll sort of call half slip, and then full slip. The threads were the threads were modeled here to account for the full slip, the half slip. If we if we only care about simulating up to half slip, we can bond the head of the bolt to the top member and then leave friction between these members, simplifying our study. Here's a comparison showing that as that bolt slip, what happens to different loads on the bolt. Here's the shear load on the bolt. As I increase the shear on this plate, I'm pulling remember, I'm pulling this top plate to the right, increasing that shear load from 10 to 20 to a100 to 200, and we can see the shear on the bolt is not increasing at all until we hit half at least half slip. Once the two members start slipping, then we start seeing the shear on the bolt increasing. Then when we hit a full slip, then we see the center starts experiencing shear. We have we have 2 points on shear, shear in the head, but also shear in the center. That's when that center shear starts to increase. When the threads hit the wall, we see that center shear will get added to the head shear to to enact the the overall shear on the bolt. Comparing this to using a bolt connector. If I had just used a bolt connector instead of going through the trouble modeling this bolt, I would have gotten about the same answer. You see the blue line looks very close to the red line. The blue line's our bolt connector, our simplified bolt connector model used in SOLIDWORKS simulation. The red line is the solid model. This also shows the axial force acting on the, bolt. Now careful the units the, scale can be a little misleading. I don't have this set to 0. It's set to a1000 to 1200. So the axial force does not vary by much, but if we do model the solid bolt, there is more variation to that axial load than versus if I use a bolt connector. If I use the bolt connector, it maintains that preload at 12 at close to that 1200 initial preload I have for I had for this example. And then finally, bending. The bolt experiences bending which very, which closely matches the bolt connector. Our solid bolt matches the bolt connector up until we hit that full slip. So the bolt connector assumes that it stays bonded up here the whole time. So there's never a full slip that occurs when we use the bolt connector. So we don't see a transition after that full slip, but it does mimic up to that up to that point, fairly well. Now to evaluate if you do model your bolts and you want to look at these bolt forces, we typically will use this tool called the free body force tool. Like to do a brief demonstration of this tool. It's very handy for evaluating things like shear forces and in this case, looking at a moment. So if I wanna see, the bending moment acting at the head of this bolt here, you see I've got these models as separate bodies. So that way I have a face I can select here to evaluate what is the moment, the bending moment, and the shear load, and the axial force going through this face. And I can evaluate all those loads by using our list result force tool using free body force. And there's an option here that says vertex for location of moment or reference point, and it's going to solve for the moments acting around this bending point I put up here. I select the face, and here it tells me the the sum of z, the the remember the loads going to the right, so it's gonna create a bending that goes to that goes to the right, kind of pivots around the z direction. This is my bending moment, and, it says free body moment here in pound inches. Also, I can get my sum of y. That's my force in the y. That's the axial force, and here's the shear force as well all from this one free body force tool. So the bolt connector gives you these numbers directly. If we use a solid bolt model, we'll have to create some geometry that we can probe using our free body force tool to get to those same kind of numbers. Alright. So that's talking about directly modeling your bolt, which hopefully you rarely will need to do. It does as you can imagine, it does take a lot more user input and computational effort if you have to take it to this level of detail. So hopefully that bolt connector is suitable for most of your, models or maybe even linearizing the bolts might be suitable for some of your simulations. Next what I'd like to talk about is this, this the options for a rigid bolt connector versus a distributed one. This is one of the fields that Enrique had pointed out in his presentation, distributed versus rigid when he was setting up his bolt connector, and he'd used early on in one of his examples used the rigid option. Which one should we use in our studies? Well, let's consider a case where we have a steel bolt fastening through a steel member and what this will do. If I use distributed, I get a result here on this, multiple bolt scenario of 73.3 mils of displacement under that load. If I just switch all these bolts to rigid, I get a different answer, 60.5. So which one is gonna be more accurate? If I use distributed, what that fundamentally is doing in the background, It's it's equivalent to as if I apply a uniform load on the surface where the head engages with the member. Or another way to look at it more physically is it's like I have a bolt, and there's a soft gasket between the bolt and the member. A soft gasket which will spread the load out uniformly. As a result of this, it creates a deformation pattern that looks like this. If I compare using distributed to those other equivalent models such as applying uniform load, I don't see any difference between the 2. Toggling back and forth, I see pixels moving on the screen. They're practically identical as I said. Or if I use the, get that soft gasket, very similar. K? So this this this is fundamentally what distributed is doing, in the background. Creates a uniform contact pattern. We'll compare this to using the other option in a moment, but you see that this contact surface is all one color, all yellow, very uniform. If I use rigid, rigid is like as though I'm prescribing a displacement to that same face. It's a very stiff displacement or more maybe more physically. If I'm if my bolt is made of this infinitely stiff material and I bond it to that surface, it's equivalent to that. And here as the same illustrations, if I use rigid versus I've prescribed a displacement, virtually identical, or if I use a rigid bolt and bond it to the surface, same thing. Here's that here's what that contact pattern looks like. Very stiff around the edge. A large amount of contact pressure around the outer edge. Now let me compare this finally to actually modeling, creating a solid model of the bolt and pulling on it downward. If I do that, I get a pattern that looks like this. Which which one does this look more like? Distributed or rigid? Here's what that contact pattern looks like. And if I put them all side by side, you can see it's neither an exact match to distributed nor a match to rigid. It's somewhere in between. And if I put these images next to each other, it kind of looks a little more like distributed to me. Here's distributed. Here's solid modeling the bolt. Here's rigid. Let me go back and forth a little bit between the images. Distributed and the solid model, they look very similar in their pattern, their deformation pattern. And, rigid versus the solid model, it looks very different. So to me, it looks like distributed is the best option. So since distributed seems better, why should I ever use rigid? Well, consider this case. If I have a steel fastener and then a softer material for the member, in this case aluminum which is about 1 third the stiffness of steel. In this case, if I use the distributed option, I model the solid bolt, or I use rigid. It's a little closer. It looks like it's almost right in between the 2 now. Before it's clearly distributed seemed like the better option, but now it's a little fuzzier. I'm not so sure. We're kind of in between. I'm tempted to model the bolts. If this is an important detail in my study, I may wanna model this bolt. Now, what about this scenario? If I have a steel bolt but then the component I'm fastening, the members I'm fastening are made of plastic. They're much softer than the bolt. You you guessed it. What's gonna be the best here? It's gonna be the rigid option. This is where we're leaning really close into that rigid. Here's the solid modeling the bolt versus using rigid. They're very similar now. Right. So in summary, rigid versus distributed. If the bolt head if the bolt material is a lot stiffer than the surrounding material, then we'll lean towards rigid. If they're similar in stiffness, distributed often is the better choice. Next I'd like to talk about is this, tensile stress area concept. So to get into this, when we are entering in a diameter for our shank diameter for our bolt, SOLIDWORKS Simulation is asking you for the nominal diameter. Seems like a silly question, but should I actually enter in the nominal diameter of my bolt here into this field? Here is a comparison between if I model the thread versus if I if I use a nominal diameter and I put them both in bending, I bend both of these bolts. You can see that the threaded bolt bends a lot more, more than 2 times more. And here is an example where I enter in the threaded diameter into that nominal diameter field. I enter in this sort of threaded diameter, so approximation of it versus I use the nominal diameter. It can make a big difference to my stiffness of my structure. See the displacements jumping back and forth quite a bit? So what should we use? What should our threaded diameter be to get a more accurate prediction as to things like the bolt stiffness and the joint stiffnesses? Here's some suggestions. Here I have a a bolt, and you can see the outermost diameter, we call that the nominal or the major diameter. The innermost diameter of the thread, we call this the root diameter. And then there's these diameters that are sort of in between. ISO recommends a diameter right about here, which is the average between the pitch and this projected root we have here, and ANSI is pretty similar. You see the difference between ISO and ANSI? Pretty small. And you can barely see the difference in this image unless I blow the image up a little bit. You can see ISO is a little bigger than what ANSI recommends for this this bolt diameter accounting for the threads. So here is a comparison of the different options if we actually model the thread versus using the nominal diameter option way off versus using ISO or ANSI, which are really close. The displacements are both close and the stresses. And finally, if I use the root diameter, this will give me the most conservative results, the lowest stiffness, the highest stresses. Now SOLARK simulation uses the ISO for its bolt strength calculations. So when we when we calculate safety factors and based on the thread, number of threads per inch or number of threads per millimeter, it's using the ISO option. But if we wanna use these other options such as, ANSI or the root, we can use a custom spreadsheet that we have that mimics what sour examination does, but, but uses some of these other diameters. So for example, if I pull up this, spreadsheet here. Here, instead of using ISO, you can see if I do a quarter inch by 20, quarter by 20, the actual calculated diameter instead of a quarter inch diameter, it's it's using a diameter that's smaller than a quarter inch for the actual calculations. Point 203, almost 20% less than the nominal diameter because of those threads. If I switch to ANSI, it's a little lower, and you can see that my what does it do to my safety factors? K. It's a little more conservative. ISO, I get a safety factor 745. ANSI, 743. Very similar. If I use root, which will be the most conservative, 7349. Alright. So in short then, instead of keying in, the nominal diameter into your into the fields for your bolts, you may consider keying in one of these modified diameters. Maybe the ISO standards tensile stress diameter, and that should give you a more accurate representation of that bolt stiffness. If you do that though, one point of caution, if you do enter in that smaller diameter, Just wanna go to one of these, bolts here. Like I've done here, here's that modified, using the ISO. This is supposed to be a quarter inch nominal diameter, but I've entered in 0.20309. If you enter that in, if you still want to do the strength data calculation, as long as you key in basically a large number for the threads per inch, it won't modify that tensile stress area. So some large number here or if you just key in the tensile stress area directly, it'll still perform the safety factor calculation accurately. Because otherwise, you'll be if you if you type in a smaller diameter here, it's gonna make that diameter even smaller when you key in some coarse threads down here. Alright. Now one more comment is, the the difference in stiffness may not be as extreme in some cases. Here ex here is an example where I have a a a usual preload, a normal preload on this where, the EXO preload dominates the, the results. If I use that threaded, let's say the ISO threaded diameter, I get a result here of 60.5 versus if I use the nominal, it's a bit stiffer, but it's not as big of a difference as when I did the comparison earlier where I had a lower preload. So if I have a pretty normal preload, difference is still present but not as much. Alright. So that's a little bit on tensile stress area. And finally, to wrap, I wanna show you some, some images around an advanced simulation tool. There's a tool that we have called 3dx, 3 d experience, but 3 d x for short. And this simulation tool allows you to use the abacus solver and gives you, access to a wider array of element types and allows you to do very advanced level simulation. Using this 3 d x tool, you're able to run up to a 192 cores over the cloud to really solve some of those big bolt connector problems. In this case, if I wanted to directly model things like a bolt, the actual threads. Here I've modeled a bolt with the threads and to you turned on contact inside of Abacus and inside of this 3 d x tool, and it's a the explicit dynamic solver is able to handle this without any trouble. Takes a while to run, but here I'm showing as I increase the torque on this wrench, this is the preload that it's creating. Now we have a spreadsheet as well to calculate to estimate a friction factor, which in this presentation we assumed a friction factor of 0.2. But using abacus, I can calculate what that friction factor would be based on friction coefficients. So here I'm comparing the abacus solve to a computed friction factor based on the thread, details such as things such as lead angle and coefficients of friction and so on. And I can see that they match pretty closely. We can, of course, see some of those dynamic effects when I'm tightening that wrench down, little bit of little bit of a kind of a stick slip sort of a scenario going on. But overall, the axial preload that Abaqus is predicting based on the torque I'm applying is matching with our equation pretty closely. Here it shows the interaction with the direct interaction with the threads with some yielding. You can see the amount of stretching on these threads when I really crank that torque up and also the contact surface shown on the threads as well. And you can see again some of that local yielding when we really crank that torque up. Alright. So with that, what we covered in this presentation, we went through a little bit of fundamentals talking about bolts as springs. Some of the different simulation tools we used today were the static analysis and nonlinear dynamic. We also talked about linearizing bolts and and got into running things like vibration, linear dynamic, and frequency analyses on top of these. We walked through a story where we started with a hand calculation. Enrique showed you a static study on the same bolts and then the nonlinear dynamic and we compared some of the results we got. And then finally, we walked through a variety of additional topics, such as the difference between distributed and rigid using tensile stress area and so on. For further training on, SOLIDWORKS Simulation, we do offer, several different training classes. The bolt connector covered in some degree of detail as well in our 3 day simulation class as well as a lot of the surrounding topics to get you more comfortable with the structural analysis tools. And then from there, you can branch off into a variety of different disciplines. So with that, we'll conclude. If you have any, further questions, feel free to ask them in the chat. Or if you think of something later on, shoot us an email, first initial, last name@goengineer.com. So thank you all for coming. Thank you very much. And, Sean, looks like we do have a question, from David, David Sheller. It looks like, SolRx uses ISO for strength. This is for the the nominal bolt, diameter the shank diameter input. If if SolRx uses ISO for strength, why don't they use it for everything? Let's see. Like, everything everything else, like, I'm trying to figure out what the context there. Sourx uses ISO for the bolt strength. Oh, why don't they use it for, like, the, the factor of safety or The nominal diameter, I think, is probably what what he's Oh, what he's oh, I see. Why don't we just why do we have to like override it there? So the nominal diameter, so sometimes you might have a bolt that's not entirely threaded. Right? So, the bolt the bolt shank might have a nominal diameter that's that's not threaded, a non threaded portion. And you want, to use the nominal on it. You wanna just key in the nominal diameter in the field for that case. But if you do have a bolt that's entirely threaded, that's where we we're gonna have to get a little more creative and and modify that quote unquote nominal field. And to make it more accurate, key in something like the ISO tensile stress diameter. Is that your is that your question, David? Am I answering that? Of course, should versus all thread. Okay. Yeah. If there's anything else I can expand on that, you know, and and feel free oh, shoulder.