Lesson finished
Lesson finished
Unlock all 11 lessons of Introduction to GUI based CFD using ANSYS FluentFull course ₹40,000 · paid
Ahmed Body Car Model: Enclosure, Inflation Layers and Post-Processing
A free lesson from Skill-Lync's Introduction to GUI based CFD using ANSYS Fluent course, on Grow by Skill-Lync · Last updated 16 Nov 2026 · Session: “3.0 - Ahmed Body”
What will you learn in this free Introduction to GUI based CFD using ANSYS Fluent lesson?
The instructor introduces the Ahmed body as a validation model for CFD and builds the flow domain in SpaceClaim using the enclosure tool. He then adds inflation layers, plots vectors and velocity profiles along lines in CFD Post, and sets a grid dependence challenge.
- Why the Ahmed body validates CFD results
- SpaceClaim enclosure to create the fluid volume
- Inflation layers: first layer and total thickness
- Velocity line charts exported from CFD Post
What comes after lesson 3?
Later in Skill-Lync's Introduction to GUI based CFD using ANSYS Fluent course (paid): lesson 4, Exhaust Port Simulation; lesson 5, Rayleigh Taylor Instability; lesson 6, Dam Break Problem. The full course has 11 lessons (15 h 52 min of video); see the course overview or its price and syllabus.
Lesson transcript
Machine transcript of the lesson audio (lightly cleaned). Technical terms may contain errors; the video is the reference.
Part 1
Hey guys, hope you're all doing good. In this video, we are going to be setting up a very exciting problem, which is basically flow over an ahmad body. Ahmad body is basically a device, is a 3D model that is representative of a standard passenger car. Now, the reason why this model was developed is to help in validating CFD codes. So one of the most common questions that gets asked is, hey, I have a CFD code, how can I trust the result, right? In order for you to validate or trust your CFD code, you need to make sure that, you know, it gives you results that are comparable with, say, experimental data, and that is where the ahmad body comes in. This is a research model which was, you know, built in real life, and people actually did experimental analysis on it, and then they have a lot of rich data, and this data is available through their publication.
Now, what you can do is, say that you are developing your own CFD code, or if you are using Amsys Fluent, then what you can do is, you can set up this particular problem in Amsys Fluent, and try out different modeling strategies to see how different your results are. All right, so let's get started. I've already opened up the workbench here, and I'm just going to drag in fluid flow fluent, and I'm just going to name this ahmad body, and then I'm going to double click on geometry and launch SpaceClaim.
All right, so once SpaceClaim has opened, what you can do is, you can just drag and drop the ahmad body model that has been shared with you. All right, so now you can actually see the model. For example, if I click on any particular dimension, you know, I can basically see, you know, what's the current unit system. Looks like it's in millimeters, which I don't want. So I'm going to go to file SpaceClaim options, and then click on units, and make sure that for this document, we are going to be using meters.
And if you want to change this setting so that you don't have to change it again and again, you can basically make this into a global setting by selecting all new documents. In my case, I like to go back and change it as and when needed. So I'm just going to save this document, and let's click OK. OK, and we're just going to look at this in the front view. Now, the modeling strategy is very simple. We want the flow to be simulated outside the ahmad body, right? In other words, that is where the mesh needs to be created, and you don't want the mesh to be inside the ahmad body.
So what we are going to do is, we have to create a box that's, you know, covering or encompassing this model. You can go to sketch, create a rectangle, and do that. That's one way. It's a longer way. The easier way is to actually use the enclosure option. So you can see that I have enclosure here. So once I'm inside this enclosure, just click on the ahmad body, and SpaceClaim is going to create an enclosure. Now, on the left-hand side, under create options, you know, try to expand this so that you can see some additional options.
Here we are saying that it is symmetric dimensions. Let's just uncheck it so that we have more control. So the first thing that I'm going to do is, I'm going to type in the dimensions, and I'm just going to put in five meters. Oh, looks like the unit system has not been changed. So let me hit escape, go to file, SpaceClaim options, units, meters. I think I forgot to click OK. That's why. All right. So now let me click on the model again, and this needs to be five meters. That looks correct.
All right. And on the front side, we want a distance of two meters. And this one is going to be zero meters. And this one plus y, we're going to add in one meter. Right. So this is basically the dimensions, the length and height. We still need to adjust the width parameter for which I'm going to be looking at the model along y-axis. Zoom in a little bit. And then you can type in 0.5 and 0.5 here. And then click. OK. Right. So you might get a warning message.
Just ignore that. The reason why you're getting this warning message is because, you know, we're trying to cut this very closely. Now, what have we done exactly here? Well, let me show you this. So you can see that we have created two components. So the first one is the actual Ahmad body, right, which we had originally imported. Let me just hide it and then enable the enclosure. Now, what is this enclosure? It still looks like a box that contains the Ahmad body. Yes, it is. But the key difference is that SpaceClaim has automatically created a single volume by taking the larger volume and subtracting the volume of the Ahmad body.
It has done that automatically when we used the enclosure option. And this is super convenient. So let me hit escape to exit this tool. And I'm going to go to design and we're going to be clicking on the plane tool. And if I click on the origin, I'm automatically going to get three sets of plane, one that has a normal along X axis, one that has a normal along Y, and finally a plane that has a normal along the Z axis. So let's go to cut view and then let's look at this particular plane, the first one.
Oops, looks like I'm still in the plane tool. So let me hit escape. Select the plane and select the section mode. There you go. You see that? The Ahmad body has automatically been cut and this is exactly what we need for the simulation. So now what I can do is I can hit escape. And what I'm going to do is I'm just going to close this guy and we're going to go back to workbench. I'm just going to double click my mesh. All right. So the meshing interface has opened up.
Let me just adjust the size of my windows. And then what I'm going to do is I'm going to first use the face selection tool and then hit N, shortcut key, and I'm just going to call this as the inlet. The other way to do the same thing is select the face, right click, and use create named selection. Right. And this needs to be called as the outlet. All right. Now, the top face, the side faces, the bottom faces, they are going to be symmetry. So I'm just going to call them as symmetry wall.
And when these faces are selected, if you hit F8, it's going to hide the face. Right. You might not see this because visually when a face is hidden, ANSYS measure does not give you a very good indication. So we need to pay attention slowly. So for example, you can see that there is a light gray color. If I do F8, you can see that that's gone. So that's how you know that there is a face and that's how you know that we can hide it. The reason why I'm hiding all of this is so that I can use my box select tool, draw a box around my armoured body, use the shortcut key N, and I'm just going to call this as car wall.
Right. Okay. So now what we can do is click on mesh. You can see that the element size is 416. You know, always first create a basic mesh to see everything works. Okay. So it looks like the mesh has been generated and what I'm going to do is look at this from the top view, use the section plane and let's just cut this guy open. Now, when we see this, you can see that the mesh has been generated, but we are also seeing mesh inside the armoured body.
Now, this is not good because you are having mesh in a region where, you know, you don't want to simulate the flow. Right. There can be instances where you want to do this type of analysis. But in this particular case, you know, we don't want to see any type of computational mesh inside because the analysis is going to be done only outside. Or the other way of saying that is only the flow outside the armoured body matters. Right. So how do we fix this? Well, the easiest thing is to go back to SpaceClaim.
So let me just close this guy and go to geometry. And the reason why this is happening is we actually have two copies of the armoured body. Right. So, for example, you have this copy as well, and this is basically causing that issue. So what I'm going to do is I'm just going to right click and I'm just going to say, hey, suppress this for physics. We don't need that component. So let's close this guy now and let's open up meshing again. It says upstream data has been updated.
So it needs to reread it. That's perfectly fine with me. So click on yes. OK, so you can see that it says one or more objects. If the error message goes away, don't worry. If you just click on this message, you will see the warning here. Just double click on it. It says one or more parts were found to be unmodified. So smart updated. So what I'm going to do is I'm just going to look at my name selections. Look at the geometry. So you can see that the enclosure is there.
And this time, you know, just make sure that you first clear the generated data and just click on generate mesh one more time. So now if you zoom in, there you go. You can actually see the armoured body. And if you zoom in closer, you can see that everything is captured correctly. And this is exactly what you need to run the simulation. All right. So we are going to take this first, run a baseline simulation and then make changes to it. So let me close this guy.
And then we are going to launch the setup. So we are going to be using double precision. We are going to run this in parallel with four processors and click on OK. OK, so sometimes this happens, right? When you open fluent, nothing happens. What happens? Why is that? Well, that's because the mesh might have not been updated. So let's just close Fluent and then let's right-click our mesh and click on Update and then let's open up Setup and then let's open Ansys Fluent again. Alright, so now you can see that we're getting more information. Now, in this case, I really did not check the mesh quality, right? Ideally, you're supposed to do that once you have completed the meshing. In fact, in your challenge, you will be asked to do it to make sure that, you know, you report what the minimum quality is.
So we are just going to run the check mesh. Looks like our mesh is okay. We are not getting any quality-related issues. So the next thing that I want to do is I want to go to, you know, setting up the physics, but in general, what I can do is I can set it up here. Now, I'm going to pick a density-based solver. Now, in this particular case, the inlet velocity is going to be 55 meters per second. Now, from a Mach number point of view, you know, it's not a lot. You know, it's basically the speed of sound is 340 meters per second.
For convenience, just assume that it's just 300 meters per second. In our case, our inlet is going to be 50 meters per second maximum. So you're looking at a value of 1 by 6, right? So basically, the Mach number in this case is, you know, 0.3, right? 0.3 or, you know, actually, it's slightly lower than that. But whenever the Mach number is 0.3 and above, it's good to use a density-based solver because you need to take into account compressibility effects. In this case, that's why we are using a density-based solver. Now, I can use both steady or transient for this particular problem.
But in this case, we are interested in, say, looking at what's the drag force acting on the car, what's the velocity distribution in the rear end of the car, how does the wake look like, you know, that type of stuff. So we are okay with, you know, doing a steady state. So let's go with that. Now, then we go to setting up physics. In this case, we need a turbulence model because the flow is definitely turbulent. In fact, you will be asked to do the Reynolds number calculation for this particular case setup that we have.
Now, I'm going to be using K epsilon, all right? So that's going to be my initial choice of turbulence model. I'll tell it right away it's not a good one for this type of a problem, but we are just going to use it. And we are just going to click on OK, all right? And in this case, I'm just going to have energy equation turned on, all right? And for materials, the default material is air, which is exactly what I want. So let's not touch it. Then let's go to boundary.
And I'm going to select my inlet. You can see that it's automatically flagged as a velocity inlet boundary. That's great. So let's click on edit. And we are going to say that the velocity magnitude normal to the boundary is going to be 50 meters per second. And for thermal conditions, you know, 298.5 or 300 is fine. So let's just click on OK. And for the other boundaries. So if I look at the symmetry wall, symmetry BC is applied. At outlet, we basically have zero gauge or one atmosphere, which is perfect.
And that's basically it. So we are ready to solve this particular problem. So let's go to solving. And let's first initialize using hybrid. Now, when you use the hybrid solver, what's happening is it's basically using a potential flow solver. What does that mean? Turns out that you can actually compute two variables called as the stream function and velocity potential, which automatically satisfy your continuity equation. Right. If you are interested in reading more about that, then pick up a graduate level fluid mechanics book like like Piyush Kundu and you can get more information.
But the idea is you can basically solve for this potential flow variables to get an estimate of the initial velocity to get an estimate for the velocity components. You cannot solve for pressure. You can only get velocity. Right. And this provides a very good initial condition or starting point. It's not accurate. It is just a very good starting point. And sometimes when the flow path is really complex, for example, in case of centrifugal pump, this might actually be very useful. Right. You you basically get a PDE that you need to solve iteratively.
And that's what happens when I initialize. Right. You can see that in 10 iterations, you know, we are getting convergence for a particular scalar. Now, this being said, what I can do is I can go to post processing and what we are going to do is we are going to create a cut plane to see how the velocity looks like. Now, this is something that we want to monitor as the simulation is running. So let's go to create and we are going to be creating a plane.
Now, before we do this, I want you to first go to graphics and kind of get a feel for where the model is. Right. So this is how the flow is going to take place. Right. So you can see that the flow is taking place along the X axis. So we want to create a plane which has normal in the direction of Z. Right. So I hope you can understand it. So let's go back to post processing and create plane. And we are going to be using point and normal.
And I'm going to say that the point is going to be in the origin. Right. And my normal is going to be along the Z axis. And we can call this cut plane, cut plane Z. Right. Z basically represents the normal direction of the cut plane. So let's just create this guy. All right. So we've created it. And then we can go to contours and then click on new. And we are going to be having a velocity contour and that's going to be on cut plane Z.
We are going to be looking at velocity. Let's click on save and display. You need to make sure that you click on field so that you can see a field contour. You can see that there is initially a velocity distribution. But like I said, this is not the real velocity distribution. Right. Because viscous effects are not taken into account. There's a bunch of assumptions that goes in potential flow theory. Right. So but this is a this is a velocity profile that you can start with. You know, there's no harm in starting with such a profile because initial conditions are always washed out of the domain.
And especially when you do steady state simulation, it really doesn't matter if your initial conditions are done using hybrid initialization or standard initialization. All right. So the next thing that I want to do is as the solution is being calculated, we want to make an animation for the velocity. So I'm just going to click on solution animation and we're going to be looking at the velocity contour. So let's just preview this guy. And we don't want this particular view. So I'm just going to look at it like this, maybe zoom in a little bit and click on use active.
And I'm just going to call this guy velocity animation and click on OK. I hope it got saved. Let's go to calculation activities, solution animation and looks like velocity animation is here. Right. So let's click on preview. And there you go. So it has been set up correctly. So to start with, I'm going to be running this for, say, 500 iterations. And let's hit calculate. You can see that the contours are starting to change and the residuals are also not behaving crazily. You know, they are not rising up and down.
They seem to be going down in general at this point. So I'm just going to wait for this to run for the 500 iterations and then I'll get back to you guys. So we'll pause the video for now and then continue later. OK, so it looks like the simulation is complete. The contours look a bit funny, but don't worry, we'll actually do a better job of post processing when we use CFD post. So this is basically your baseline setup, meaning the mesh is not accurate, but it's a case that runs very, very quickly so that you can check your setup and, you know, you can do some sanity checks and we'll be showing you how to do that in CFD post.
So now what you can do is you can close Fluent and then we are going to open up the results section. All right. So now you can see the geometry. So, for example, the car wall is right there, inlets, outlets and the symmetry wall, everything is there, right? So these are all the components. So let's just have the car wall on and to start with just double click on the car wall and then, you know, you can color it by a variable. Now you can color it by the pressure and click on apply and immediately you can see the values of pressure, right?
You can see that in the front of the car, the pressure is 1.561 e power 3. And then there are areas where the pressure is actually going negative. Why does it go negative and is there a physical significance of it? Well, that's going to be something that you are going to be working out as part of your challenge. You are going to explain to us if this makes sense or if the results are actually bad. Then what else can I do? So next, I'm just going to be inserting a plane.
So we are going to call this as cut plane Z and this is going to be very similar to what we did before. So we want this to be in the Y X plane. So it looks like we are already there. So let's just click on apply and then you can just go to color. You can color this by variable and let's look at velocity. And let's click on apply, right? So you can see that the results are definitely really coarse. So it doesn't look good at all.
And if you want, you can just go to render and click on show mesh lines and click apply, right? And then let's take a look at the model from the front view. So, you know. You know. This is a result right now. This is the wake region. You can see that the velocity is getting lower here and you should be able to make vector plots as well. So let's just click on OK and we are going to be making that only on cut plane Z and let's click on apply.
So it looks like the vectors are there. But before we do this, let's go back to our cut plane, go to render and then disable the mesh lines. Click apply. And now let's go to the vectors and let's color this guy by constant. And we are just going to make sure that this color is black so that you can see the vectors. Right. There you go. You can play with the vector operations to basically understand, you know, how it behaves. So you can see that here the vectors are really, really small, right, in the recirculation region.
That's why you don't see it. All right. OK. So what else are we interested in? In the actual experiments, what they did is they measured velocities in several vertical stations. Right. So basically, you can think of having a line after the armoured body and also before the armoured body and also top of the armoured body. And along those lines, you're actually measuring the velocity. So you get a very nice velocity profile. How do we do that? So let me disable the vector plots and I'm just going to click on insert location line.
Right. And let's just call this as line number one. And we are going to say that this line is going to be created three meters along the x-axis and three meters along the x-axis. And we are going to be using the cut option. And the first point is going to be in three zero zero. Right. So that can be somewhere here. I'm just assuming. And the second point, you know, we are basically going to say that it's going to be in three two zero. Right. So along the y-axis, you go up two meters. That's where you have the two points.
And from those two points, you can create a line. Now, when you do a cut, what's going to happen is this line is going to actually cut the domain and get data. Now, if you use samples, then what's going to happen is it's going to try and get 10 samples within that line. Ideally, you need to use cuts. But sometimes your mesh is really coarse. When you cut it, the results might not look that great. But anyway, let's click apply. And you can see that the line has appeared. Now, what you can do is you can obviously go back and make this to make this to as well and bring the line closer.
Right. What can you do after you have a line? Well, I can actually go to insert and I can insert a chart and let's just call this as chart one. And this is going to be a X, Y line chart. And for data series, what we're going to do is we are going to add it from this location and which is line one. And for X axis, the variable is chart count. But we want this to be the Y coordinate and for Y axis. We want this to be the velocity U, right, the U component of velocity.
And if you click on apply, there you go. You get the velocity profile in that line. Now, the cool thing about this is you can actually right click and you can just duplicate this guy. Now, let's call this as line two. And in line two, I'm just going to change the coordinates to three. Right. The X coordinate to be three. If I click apply and if I go to 3D viewer, you can see that now I have two sets of lines. And then I can go back to my chart. I can go to data series. I can click on new data series.
And this is going to be line two. And if I click on apply, boom, I get two curves in one single plot. And the nice feature is now I can click on export and I'm just going to go to documents and type in data from CFD post and click save. And then if I go to documents and if I double click that and open it in Excel, we have the Y value and the velocity U component of velocity for that particular Y in an Excel sheet.
Right. And you have it for all the different line probes. Now, this is great because now we can run a bunch of experiments. We can make the mesh finer and you can actually compare how the velocity profile is getting affected for each and every change that you make. In fact, that is going to be part of your challenge. And this challenge is going to be like a project because you are going to be running a lot of different studies. All right. With that, I would like to conclude this particular video.
In the next video, we will be refining our setup so that, you know, we get a much more better looking mesh so that, you know, the data can be useful for us. All right. I'll see you guys in the next video. Bye.
Part 2
Hey guys, hope you're all doing good and welcome to a new video. In the last class, we finished setting up the flow over the armoured body. Now, the computational mesh that we used for that particular case was, you know, really coarse and it's in general not acceptable at all, especially for engineering results. So what I'm going to do is I'm going to basically show you what are some of the things that you can do to improve the mesh quality. So I have my original setup here, so which is called as the armoured body baseline.
So what I'm going to do is I'm just going to click this and I'm going to duplicate this setup. And then I'm just going to call this as armoured body, you know, refined setup. All right. So now what I'm going to do is I'm going to double click on the geometry. All right. And the first thing that I'm going to do is make sure that I add a region of refinement right in front of the armoured body and also, you know, in the wake region. Right.
So when we did the baseline simulation, we saw that the floor near the armoured body was highly unresolved, meaning there were not a lot of mesh points. So what I'm going to do is I'm going to draw a box and I'm just going to refine the mesh a bit more finer inside the box instead of meshing the complete domain. This is what you call as local refinement. And the way you can do this is you can use the enclosure. Right. So what I'm going to do is I'm just going to select this guy and I'm going to prepare and I'm going to select enclosure.
So when we do this, you can see that the box appears. Our unit system is in millimetres. So let's go back to units and change it to meters. OK, and then just type in the dimensions that I'm going to provide. Now, basically, what I'm doing is I've calculated these dimensions based upon the wake region size that was seen in the baseline setup. Right. Now, when you run this particular simulation, the wake might actually come outside the box, which is bad. Now, the way I calculated these dimensions is based upon the baseline setup.
I'm trying to make sure that the wake region is also refined. All right. So this has to be done iteratively and it changes from problem to problem. And that's why we need to run a baseline setup. So before start typing in values, make sure that you uncheck symmetric dimensions. All right. And we are going to have a one meter long refinement on the front side, on the back side. And then half a meter refinement on the front side. You know, the bottom is going to be zero.
So that it coincides with the bottom of the armoured body. And this is going to be 0.5 meters. And that's basically it. So when you click OK, you are going to get an error. Now, if you take this geometry right now, in this particular case, your outer box and you have an inner box. If you take this and if you mesh it, it might not work out. So to prove that, what I'm going to do is I'm just going to close this guy. Now, let's open the meshing interface.
But before we do this, we need to actually reset the meshing. Why is that? So let me actually open meshing right now. It says that the upstream data needs to be reread. So let's click on yes. And then you can see that the geometry has been loaded. But only the internal faces or internal surfaces are available. I'm not able to select the outside box. Right. You can see that the named selections are there. I can see my inlets and outlets. But if I try using the face selection method, I can no longer select my inlet.
Similarly, if you select the symmetry wall, you can see that, you know, the bottom face is missing. Right. Now, this brings me to an excellent point. So you need to duplicate your case setups only if you're not changing your geometry a lot. Meaning, say that you're changing the diameter of a particular feature or the length of a particular feature, then you can still duplicate and kind of save a lot of time. But in this case, we are actually introducing a new component, which kind of breaks, you know, previous components.
Right. So because of that, the meshing interface is not playing well. You can try to fix this one by one by deleting all the name selections. You know, you can work backwards. But the best thing to do in this type of scenario is just right click and first clear generated data and then right click and then just hit reset. So this is just going to delete everything, which we are perfectly fine with. And then we are going to edit the meshing again. All right. So now you can see that both of our bodies are available.
Right. So this is exactly what we wanted. So before doing anything, I'm just going to first generate the mesh to show you how the baseline mesh is going to look like. So it seems like the mesh has been created. So let's create a section plane and take a look at the internal geometry. All right. So this is what I was talking about. Right. So you can see that, you know, you don't have a mesh inside the arm of the body, which is good. But then you kind of have this, you know, mesh overlap here.
Right. So the mesh from the bigger box and the mesh from the smaller box are not getting attached perfectly. In fact, they are overlapping and this is bad. So in order to fix this, what we need to do is we need to close meshing. We need to go back to geometry and then first understand what's going on. So the easiest way to visualize what's going on is to create some planes. So I'm going to select the plane tool and I'm going to point it towards the origin.
So when I do that, you can see that it's showing three planes and that's exactly what I want. So if I click on the origin, I'm going to automatically create three planes. Right. So now make sure that you hit escape to exit the plane tool and carefully select, you know, the side plane or whatever the plane is. Right. And then hit the cross section mode. Now, when you do this, you should be able to see what the issue is. Right. Now, each section has a particular hatch pattern.
Right. So you can see that this guy, I mean, the hatch inside our smaller box basically contains hatches from both sides. This means this is actually an overlapping region and we don't want that. And if you go to prepare and if you run the interference check, you can see that SpaceClaim is able to say that, hey, there is a huge interference here. So what we are going to do is we are going to click OK. And it's basically solved the problem. So now you can see that there is no overlap.
So what did we do here? First, let's exit out the section mode and go to 3D mode and let's hide all of our planes. And I'm just going to show you each of these enclosure. Right. So we'll first take a look at this guy. Right. So you can see that this particular enclosure, if you cut it by, you know, this plane, you can see that the inner box has been cut out automatically, which is very, very important. And if we hide this guy and show this guy, you can see that this guy contains the inner box.
But this time the arm of body has been cut out. Right. And when these two boxes are joined together, that forms our flow domain. Now, in order for all of this to work, you need to make sure that share topology is set to share. Only then these two individual blocks are going to exchange information. Right. In other words, the meshing is going to be uniform. So now let's close this. And if we right click and edit, it says the upstream data needs to be re-read, which is perfect.
So let's click on yes. All right. So now let's just right click mesh and then generate the mesh to see how a baseline mesh looks like. And now if you zoom in, you know, now you can see that this perfect connectivity and there's no mesh overlap. And this is exactly the setup that you need to follow for any external flow simulation that you do with ANSYS Fluid. The only thing that's going to change is your geometry and maybe the size of your wind tunnel is going to change.
But that depends on your computational power and the flow conditions. But this is exactly the standard practice that you need to follow. You know, in industry, they also follow something very similar to this. Right. So now let's work on the meshing part. So the first thing that I want to do is, you know, outside. So outside the inner region. Right. You have a perfect structure. What do I mean by perfect structure? You know, it's made up of straight lines. Right. So there's no complex shape. So, for example, if you are following my mouse, you know, this particular shape is just made up of straight lines.
In 3D, it's just made up of boxes. In general, whenever you have a scenario like that, it's better to use hexahedral meshes. Now, hexahedral meshes have the highest quality of all mesh types. And whenever possible, you need to use that. So to do this, right click on your mesh, insert. And we are going to select method. Right. So method is used to basically select a particular meshing method. And what I'm going to do is I'm going to use body selection. And I'm just going to select the outermost body.
Hide the section plane so that you can understand what is being selected. And here, just click apply. So we know that, you know, we are basically modifying the meshing method for that particular body. And for method, what I'm going to do is I'm going to use multi-zone. All right. And when you use multi-zones, it's basically going to try and create hexahedral meshes wherever possible. And in other regions where different mesh types are being used, it's going to connect it perfectly. Now, as far as our fundamental mesh is concerned, we are going to do some modifications.
I'm going to say that the element size is 100 millimeters. And if you expand sizing, there is an option called as the maximum size. Let's say that the maximum size is also 100. So this way we are making sure that we get evenly sized meshes in the outer region. So let's right click and generate mesh to see what happens. All right, perfect. That looks really beautiful. So let's take a look at inside. All right, so you can see that you have this nice hexa mesh outside.
And, you know, it's interfacing with your inner tetrahedral mesh, which is perfect. Now, the other thing that we want to do is, you know, right click, insert, sizing. So what we are going to do is, we are going to make sure that the mesh is inside, right? So if I hide the section pane, you know what I'm selecting. We are going to make sure that here the sizing is slightly more refined. So maybe something like 50 millimeters, right? And again, depending upon the computational capacity and depending upon your licensing restrictions, you can, you know, make this number either higher or lower.
So I'm just going to hit generate. All right, and now you can see that the mesh has been refined further inside. Now, what else can I do? If I actually rotate the model and if I inspect the features, you can see that, you know, the cylindrical faces or cylindrical pillars that basically support the ahamud body have been approximated as polygons. Now, this is bad. That's because you can see that the element size here is actually quite big. Now, you can see that you have this bar, right?
So this distance is 17.50 millimeters, which means that this distance is also roughly 17.5 millimeters. So what I'm going to do is, I'm going to select my mesh and then I'm going to insert sizing. And this time what I'm going to do is, I'm going to select my entire ahamud body. So let's uncheck the section plane. Now, you cannot directly select the ahamud body because it's inside. So let's go to the face selection tool and select one face and hit F8. This is the shortcut key to hide faces.
So I'm going to hide all the faces, right, except for the ahamud body. All right. So you can see that the faces are getting hidden. All right. Perfect. So now we have only the ahamud body. Go to the box select tool, draw a box around the ahamud body and make sure that you are still in sizing and for geometry, just click apply. It's going to say that you have selected 15 faces and the method is now called as face sizing. Now, let's put in a value of, say, 10 mm and generate the mesh and see what happens.
Okay. So it looks like the mesh has been refined. You can see that this is still not perfectly round. What you can actually do is you can select only this particular face. So in other words, what I can do is I can just come here and maybe for these guys, go back to the single select tool and you can just try selecting these guys alone. And if you click apply, you're now selecting only these four faces and you can put in a value of maybe five millimeters and then now generate the mesh.
All right. So now you can see that this is much better than before and your total cell count might not have gone up a lot. So let's actually go to statistics and see how we are doing for cell count. You know, we are about one point, like point, point one eight million cells. I believe you can go up to point five million cells in academic license. So we are still within, you know, the range. So let's actually look at the section plane. Look at the geometry.
Now, the other thing that people do for external flow simulations is create something called as a boundary layer mesh. Now, remember, right, at each and every boundary, there is a boundary condition applied. Now, if you see this particular cell, you know, this particular cell, if you enable the prism mode, you can actually see how the cell shape is actually right in three dimensions. So let me maybe hide it so that I can explain what's going on here. So each cell is going to have its cell center in different locations, right, which is not ideal for applying your wall boundary conditions.
So what we want is we want to create a set of cells that actually follow the shape of, you know, the surface quite closely. These are called as inflation layers. It's much easier to actually visualize this. So let's go ahead and do that. So I'm going to mesh and there's something called as inflation here, and we are just going to say that we are going to inflate all faces in chosen named selection, and we are going to be selecting, oh, looks like there are no named selections.
Oh, that's bad. Yeah, that's because we reset everything so we don't have any named selection. So we need to unfortunately go back to geometry and kind of redo everything. So let's hide this particular face, make sure that the section plane is no longer there. Lucky that we just have the armored body, so we should be able to select it, and I'm just going to call this as car wall. We still need to name other faces, but we can get back to that later. So let's go to mesh, and under inflation, this time we should be able to select the car wall.
Now I'm going to select the first layer thickness. Now this first layer thickness needs to be calculated based upon your Reynolds number. There's something called as Y plus, based on which you can actually calculate your first cell thickness. But for now, I'm going to put in a value of, you know, 5 millimeters. Now this might be very, very large, especially for the Reynolds number that we are dealing with. 5 mm is pretty large, but unfortunately, you know, you cannot go lower than that. In my case, maybe I can go to 1 millimeter or even smaller, maybe like 0.1 millimeters as well, I have the computational power in your case, even if you have the computational power and if you have the academic license, you cannot have more than 0.5 million cells, right?
And this is going to definitely take you over that range. All right. So for now, we are just putting in 5 millimeters to understand what inflation layer means. So let's click on generate mesh. Now, if you do this correctly, the process should take a bit longer. If that happens, you know that things are working correctly. So let's look at section plane. All right. So this is what you call as an inflation layer. Now, the inflation layer, you can see that it starts small and it keeps on growing, right?
Now, that's the setting that is being provided here, right? So the growth rate is 1.2. So there's 20% growth from layer to layer. So in this particular case, you can see that the boundary layer doesn't look correct, right? The first layer thickness looks right, but after that, you know, it kind of looks messed up. This happens when you give the first layer thickness. So instead of giving the first layer thickness, if you provide the total thickness, then you are constraining the problem much more, right? So how do we do that?
Well, if your first layer thickness is 5, the second layer is going to be 5 times 1.2. The third layer is 5 times 1.2 times 1.2, right? So you can actually do this. So if you just type in 5 times 1.2, if you want 6 layers, then, you know, you need to basically say 6 minus 1, right? And that's going to be 30 millimeters. I think I have the math correct. Oops. Actually, this should be power 5. So this should be maybe power 5. I'll just put it like this.
So that says 12.44 millimeters. So what we are going to do is we are going to come here and for total thickness, we are going to put in 12.5, right? 12.5 millimeters. Let's generate the mesh again. All right. So now you can see that the mesh looks much better. It looks much regular, right? And that's because we are providing total thickness, which is going to constrain the mesh in the right direction. All right. So what I want you to do is I want you to apply these particular techniques.
Now, in this case, if we look at the total cell count, you know, we can definitely go two more times, you know, two times the total number of elements that we have here. And you can do that by, you know, maybe decreasing the mesh size in the XR region or also, or you can make this box a bit bigger, right? So anyway, I think you have everything that you need to run a decent Ahmad body flow simulation and post-process the results. Now, as part of the challenge, you will be comparing the results for different grids.
Now, I'm going to give you some flexibility in the number of grid points. Now, I'm going to be giving you some flexibility because I know that some of you have license restrictions. So the challenge would be to not target a particular element size, but it would be to run a grid dependence test from the baseline case, which should run on your machine all the way up to the maximum cell count that you can run. And then, you know, explain the differences. All right. I hope this makes sense.
And I'll see you guys in the next video. Bye.