← Previous lessonFree lesson 2 of 3 · lesson 2 of 11Next lesson →

Unlock all 11 lessons of Introduction to GUI based CFD using ANSYS FluentFull course ₹40,000 · paid

Price & syllabus
Free lesson · 48 min · no payment

2D Flow Over a Cylinder: Vortex Shedding, Steady vs Transient

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: “2.0 - Flow Over a cylinder-part 1”

What will you learn in this free Introduction to GUI based CFD using ANSYS Fluent lesson?

This lesson sets up 2D flow over a cylinder in ANSYS Fluent, using a custom fluid viscosity to control the Reynolds number between 20 and 100. It adds a monitor point and compares a steady run with a transient run, which captures vortex shedding.

  • Cylinder domain sized by diameter multiples
  • Custom fluid viscosity to fix Reynolds number
  • Monitor point to track velocity during a solve
  • Why vortex shedding needs a transient solver

What comes after lesson 2?

The next free lesson is lesson 3, “Ahmed Body Car Model: Enclosure, Inflation Layers and Post-Processing” (44 min). 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 and welcome to a new video. So today we will be working on a very simple but a fundamental problem, flow over a cylinder, right? So this is a problem that has been studied a lot both computationally and also through experimentation. The reason why you need to do this problem using computational fluid dynamics is because you can actually understand how different components in your CFD setup affects the end result. So in this particular case, you will be learning how to perform a two-dimensional simulation.

Now, the condition is going to be highly controlled, meaning we are going to be setting up this case for a particular Reynolds number. So you will be learning how to control the Reynolds number by creating a customized fluid, right? So we're going to create a user-defined fluid, you can say that, and we are going to control its properties so that we can precisely control the Reynolds number. You will also be learning how to control the Reynolds number by creating a run-time animation. That is, as the solution is being calculated, you can also take a look at some meaningful plots like the velocity contour and pressure contour to understand how the flow is being developed.

So in this process, you will visualize something called as the vortex shedding, which is an important phenomenon that occurs when you are simulating flow over a cylinder. And as far as the post-processing is concerned, you will be learning how to add monitor points. So these are like small sensors which can measure anything like pressure, velocity, temperature at a given particular point. So you will learn how to do that. And then we will be learning how to create animation files. So this is different from runtime animations.

So runtime animation appears when you're running the simulation, but you can always take all those data files and create a movie file with it, which you can send to a friend or a colleague. From a physics point of view, you will learn about numerical diffusion and how it actually affects your results. And we will also be looking at both the steady state approach and transient approach. And we will be doing, you know, intermediary level post-processing in this particular case. So our geometry is fairly simple. So we are having a rectangular computational domain.

And this right here is our cylinder. All right. Now, this is a 2D approximation. So you are just taking one slice of the cylinder. And hence, the cylinder is going to look like a circle. Hope that makes sense. So we are going to have an inlet velocity of one meter per second. And at the outlet, we are going to have the pressure boundary condition. We are going to say that, you know, we have one atmosphere or the gauge pressure is actually equal to zero pascals. And then the top and bottom wall, we are going to use something called as the symmetry boundary condition.

Now, with respect to the cases that we are going to be solving, or at least I will be solving at least one of these cases. And maybe I'll assign the others as an assignment. You will be modifying the Reynolds number from 20 all the way up to 100. The reason why we do this is we can actually capture what you call as vortex shedding, which occurs at Reynolds number higher than 40. So even though the flow is laminar, vortex shedding can occur. And we are interested in capturing this because this is what you call as the von Karman vortex street, which is a very popular phenomenon that occurs in the laminar flow regime.

Right. So these are the three different cases that we are going to be setting up. So that being said, let us launch ANSYS workbench and get started. Okay. So what we are going to do is we are going to select fluid flow, fluent, and create a standalone system. And we are going to call it flow over a cylinder. All right. So let's double click on the geometry to launch SpaceClaim. This is what we are going to be using to create the geometry. So once you open up SpaceClaim, go to file, click on SpaceClaim options.

And then you're going to click on units and we are going to make sure that this is set to meters. All right. And we are just going to click on OK. And we're going to click on the Y axis and then start our sketch. We're going to start with our cylinder, which is basically a circle and the diameter is going to be two meters. Okay. And then just zoom out so that you can see your circle. All right. Then we are going to be creating the computational domain.

Right. So as shown in the PPT, we are going to have a 10 times the diameter. And this distance is actually from the center of the circle and not from the circumference. So we need to make sure that from the center of the circle, the inlet is located at a distance of 10 times the diameter, which means that's going to be 20 meters. Right. So let me draw a construction line. Right. So that, you know, I can locate my inlet correctly. And similarly, if I go to the PPT, you can see that 20 times the diameter, which means 40 meters, that's the location of the outlet boundary.

So I can put in 40. Right. So that is going to be the extent of my computational domain. And what about, you know, the size of the inlet? Well, I'm going to say that it's in total, the inlet is going to be 10 times the diameter, which means from here to here, that's going to be 5 times the diameter, which is 10 meters. Correct. So I have that here. And similarly, on the other side, we are going to have 10 meters. Correct. So once we have this, we can actually use the rectangle tool to basically select this particular corner and kind of see if we can actually get this particular point.

So it looks like I can do something like this. And you can see that I have 20 meters for my inlet and 60 meters for the total length, which is perfect. All right. So that concludes the geometry creation process. And since it's 2D, it's fairly easy. So now that we have created the geometry, we need to basically convert this into a surface. So I'm going to use a pull tool. When you use the pull tool, suddenly you can see that it changes the color. Right. That means it has actually become a surface.

So now hit escape or you can rather or alternatively, you can go back to the select tool and then you should now be able to select the circle inside and just delete it. And then expand your curves and whatever construction lines that you have drawn, you can just delete them. All right. So that basically concludes the geometry creation process. Make sure that the origin is located in the center of the circle. It's very important because we will be adding a monitor point based upon this particular coordinate system.

So let me just close this guy. And now what I'm going to do is I'm going to right click on my mesh and I'm just going to click on update so that the geometry information gets updated. So then double click on the mesh to open the meshing interface. So this is going to show the computational mesh. So now if you click on mesh, you will immediately see that there is a basic quadrilateral mesh or a quad dominant mesh that gets created automatically. So a quadrilateral contains four sides, as you might know, and you can see that predominantly most elements are quadrilaterals.

You still have a triangle, one or two triangles here and there, but it's primarily quad dominant, right? And we don't want this. We want the mesh to be a bit more triangular. So what I'm going to do is I'm going to right click on my mesh and insert method. So the idea is you have a baseline mesh and then you can add several methods. And what Ansys is going to do is it's going to first create the baseline mesh and then it's going to include that method in and just keep on processing all the methods that you have added.

Then what I'm going to do is I'm going to click on this automatic method. And the first question that Ansys is asking me is, hey, what is the geometry on which this method needs to be applied? Well, it's the entire body, right? Now, in this case, I'm clicking on body, which means it's a 3D geometry, but in reality, it's not. So what you can do is you can actually use the face selection tool to select the same thing. It doesn't matter. And then in the geometry section, just click apply.

And you should immediately see that it says one body, right? If it says no selection, in other words, if you see yellow color, that means Ansys is actually missing a user defined input, right? So if you see something yellow in color, that means you are supposed to type in something there or select something there. You cannot get past that step without making sure that, you know, all the yellow inputs have been filled. Okay, hope that makes sense. So here you can see that the method by default is quad dominant.

I'm just going to select this and make it triangles. And then now if I click on mesh again, you can see that your mesh appears pink. That means that mesh is actually obsolete, which means that mesh is no longer valid. So you need to click on update or generate mesh. So we will click on generate. And immediately you can see that now the mesh is triangular, right? Which is what we want. So if you click on mesh, you can see that asks for a particular element size.

Now, what would be the element size? Well, it's very hard for you to take a guess. What you can do is in this case, the problem that you're simulating is a cylinder, which has a diameter of two meters. So what I'm going to do is I'm going to start with two meters as my element size. Now, remember, ANSYS is going to adaptively refine the mesh near the cylinder, right? So, for example, previously we had the element size to be three meters, right? Which is the case here, right?

So, for example, here you can see that the triangles are very, very large. But as we come closer to the circle, things get smaller, right? So ANSYS is doing the right thing. So I'm going to start off the element size of two meters. And ideally this changes with problem to problem. There is no single number or single formula that you can actually use. You kind of have to go case by case to figure it out. So in my case, I'm starting with two meters. And then I'm just going to...

Click on Generate Mesh. And you can see that the mesh looks pretty much the same. There's not a lot of difference. Now, one thing that I noticed is if I actually come in close, you can see that my circle is looking more like a polygon with maybe 12 or 13 faces. So it's not a perfect circle. And to be honest, you can never get a perfect circle unless you have infinite number of edges. However, this is too small. I can still see that, you know, there are some sharp corners here which can actually affect the flow field. So one thing you want to do in CFD is you want to make sure that the geometries on top of which you are trying to simulate the flow, they are captured perfectly. So I'm going to right click on the mesh and I'm going to insert a sizing method, right? So this option is used to precisely control the mesh. So what I'm going to do is I'm going to be selecting the edge because the edge is what I want to control.

And apply. And then what I want to do is I want to say that the number of divisions is maybe 36, right? How did I come up with that number? This is more from an experience point of view. You can use a large number here. That would basically increase the mesh count. But in general, you know, if you are having an edge for every 10 degrees, you know, because the circle is made up of 360 degrees, if you have an edge for every 10 degrees, that gives you a smooth enough representation, right?

Or in other words, I can say that it's good enough for engineering calculations. So now if I right click and generate mesh, you can see that we have a much more smoother looking circle, right? So I think this is enough, right? So this would be a very good base mesh, meaning with this, you can go ahead and run your simulation, you can get the results and you can make changes to your mesh as required. Now, one thing that I want to do is, since the flow around the cylinder is very important, I want to make sure that I take care of the region around the cylinder.

And I can do this by using something called as an inflation layer. So inflation layer helps us create what you call as a body fitted mesh. It might not be clear to you right now, if I just say what body fitted meshing is, but I can actually show it to you. So first, what I'm going to do is I'm going to select the entire face and click apply. And for boundary, I'm going to select this particular edge and click apply, right? And I'm going to say that for my inflation option, I'm going to be using the first layer thickness, and I'm going to say that my first layer is 5e-3 or 5 millimeter thick.

And let's generate the mesh, right? So if I go to inflation, you can see that I have two layers. So if I zoom in on my mesh, you can see that I have two layers, right? And this is basically refining the mesh even more. Now, what I'm going to do is I'm going to go to inflation, I'm going to type in a value of 6, right? So that I have six inflation layers, let's generate the mesh. And you can see that the mesh that we have created closely follows our geometry.

And that is what you call as a body fitted mesh, because the mesh perfectly fits your body. If you come from the world of CAD, then there's a concept called as an offset curve, right? Which basically replicates the geometry that you're trying to offset. Body fitted meshing is exactly like that. In this case, we have a sphere. So the first layer mesh is also going to look like a sphere if you basically join all the sales centers, correct? If your shape is more like square or if it's like an ellipse, then when you do body fitting, if you do it correctly, then your mesh would represent your body very well.

That's why it's called as body fitted, right? Now, in this particular case, you can see that I've added six inflation layers, all right? So let me just click here and count 1, 2, 3, 4, 5, 6. So we have six inflation layers. And you can see that from the starting cell, the size slowly increases. That happens because of this growth rate. There's a factor of 1.2, right? So about 20% growth for each and every layer. So you have the starting layer, which you have defined as five millimeters. So the second layer will be 20% more, right?

And this is continuously going to increase till the number of layers that you have input, which in this case is six. So I think this is a very good basic mesh to start with. And what I can do is I can jump to ANSYS Fluid and I can run the simulation. So let's close this guy. And we're just going to right click, update the mesh. This might take a bit of time. And then what I'm going to do is I'm going to right click my setup and I'm just going to update it as well.

All right. So now let's actually edit the setup. So you can just double click on setup and we're going to be running a parallel simulation with four processors and make sure that double precision is set and click OK. All right. So you can see that our mesh has been successfully loaded. Now, one thing that I actually forgot to do is I forgot to assign named selections. Right. So I forgot to tell ANSYS that, hey, which is the inlet and which is the outlet. Right. So what I can do is I can close this guy and just click OK and then open meshing again.

And what I'm going to do is I'm going to go to edge selection mode. I'm going to select this inlet edge and use the shortcut key N or you can right click and click on create named selection. You can see that in the bracket, the shortcut key is N. Right. So that's what I used. That's what I will be using next. So I'm going to click on this and I'm going to say that this is inlet. I'm going to click on the outlet, hit N and I'm going to call this outlet for the cylinder.

Let's click on this guy, hit N and we're just going to call this cylinder wall or you know what? Let me just call it wall. And then the top and bottom, we are going to be assigning symmetry boundary condition. So I'm just going to say symmetry. Right. So we look at the mesh again and we make sure that there is green tick marks all over, which means everything has been updated. You can just close the measure, right click, update. And then we are going to right click setup and we are going to edit it.

You can see that we are getting a message saying that the upstream mesh has been changed. Do you want to load the new mesh? Yes, absolutely. So let's click on yes and make sure that you are using parallel four processors. Now, if your license does not allow you to do this or if your computer does not allow you to do this, you can use serial. You can use serial, but that's going to take a lot of time because we're just going to be using one processor.

So we are just going to click on OK and we're just going to wait for Ansys Fluent to open. And when I said it's going to take a lot of time, it's going to take a lot of time in a relative sense, meaning when you run it with more processor, obviously it's going to run much faster. I hope that makes sense. OK, so one thing that you can immediately check is go to setting up physics and click on boundaries to make sure that you see all the boundaries.

So that way you can be sure that everything has been loaded. In addition to this, you can also go to console and. You know, you can just make sure that all the parts have arrived so we can click on check mesh and you can see that there are no machine problems, which means everything is good. So we are going to be setting up physics first. So we are going to be performing a steady state analysis, pressure based solver, and we can click on discuss and I'm going to say that the viscous model is laminar, meaning there is no turbulence model. The reason why we are doing this is because of a Reynolds number is extremely small.

The maximum Reynolds number of my simulation is going to be 100, which is which is completely laminar, right, which is in the laminar regime. So let's click on OK. And the way I'm going to control the Reynolds number is by modifying the dynamic viscosity. So let me click on materials first. And then what I'm going to do is I'm going to open up flow and database and I'm going to select if you start typing AIR, you will end up with AIR and just click copy. And I'm just going to call this as user material, right, because I'm defining it and it's a customized, right.

So let's click on OK and close this. And here you can see that there are two other materials. Let us select the unwanted materials and then just delete it, right. And AIR, I think you should be able to delete it, but it looks like it's it's automatically assigned. So this is one of the things that Fluent does. In order to make your life easy, it kind of tries to predict what you want and sometimes it might be wrong. So in this case, what happened was for our volume, Fluent assumed that it is made up of AIR.

So you need to first delete or you need to first tell Fluent that, hey, don't use AIR as the standard material. Use the custom material that I've created. So to do that, go to Cell Zone, click on FFF underscore surface. This represents your volume. You can see that it's of type Fluent. Click on Edit and then change this guy to user material and click OK. So now that you are told ANSYS Fluent that your material is not AIR, you can go back to materials. You can select AIR and you can delete it.

So now you can see that only user material is there. OK, and then what I'm going to do is I'm going to say that the density is one and I'm going to say that my viscosity is equal to 0.05 kg per meter second. Now at this point, now the reason why I'm picking up this, this cause MATLAB is because in this condition, it has been documented that you start seeing vortex shedding even in laminar flow cases. And this is what you call as the Von Karman Vortex Street. So we are going to try and capture that, right?

So we are going to click on Change here. Make sure that you do it and click on Close. And one thing that I always like to do is I like to check if my material properties are set correctly. So I open up materials again and I can make sure that it is 0.05, right? If it's not, then most likely what happened is you did not click on Change and Create and you just clicked on Close, right? Since it's blue in color, sometimes you just click that directly without even seeing it.

It has happened to me a bunch of times. So then we are going to go and set our boundary conditions. So you can see that from inlet, it has automatically assigned velocity inlet boundary condition. That's awesome. And I'm going to say that my inlet velocity is 2 meter per second, right? That's the one. Oh, sorry. Actually, it should be 1 meter per second. My bad. And that's the only thing that I care about. For outlet, you can see that the pressure is 0 Pascals. But remember, this is gauge pressure, right?

Which means this is actually 1 atmosphere, right? I hope that makes sense. So click OK. And then for wall, click on Edit. And here we are just going to make sure that for our cylinder, we use a no-slip boundary condition, meaning the velocity on the first cell that's attached to our cylinder as a velocity of 0, right? So we can click on OK. And for symmetry, you can see that the type is symmetry. So that's perfectly fine. The next thing that we need to be doing is we need to look at, you know, different flow quantities while the solution is being generated.

So for that, I'm going to be using definitions. So let me click on definitions. And I'm going to be using a new surface report. And I'm going to be selecting something called as vertex average. So let me select this guy. And I'm just going to call this as monitor point. And then what you need to do is you need to select a monitor point, right? Now, in this case, you can see that we have not created any monitor point. So this is not going to work out, right?

So what you have to do is you have to unfortunately come to post-processing, which is actually after the solving tab. Now, this kind of breaks the flow, right? But the reason why I showed that is to actually tell you that sometimes you might have to actually switch your workflow a little bit, depending on what is it that you want to achieve. Now, in this case, what I want to do is I want to create a point at a distance of four times diameter to the right side of my cylinder, right?

I want to see how the velocity changes. So I'm going to create a point there. And what I'm going to do is I'm going to basically go to the graphics tool. And you can immediately see that the location of the monitor point is being shown. It kind of looks really big, which is not nice, but that's fine. I'm going to say that this is actually at a distance of four times the diameter, right? Which means that should be eight meters along my x-axis and the y-coordinate should be zero, right?

And the value that was before is as good as zero. But I'm just going to make sure that it is exactly zero. And I'm just going to call this as my monitor point and I'm going to create it, right? So when you created it, you don't get a prompt and I don't think you get any message in the console as well. So let's just close this guy and now go back to solving. Go to definitions, new, surface report, vertex average. Now, since we have just one monitor point, the average value is basically going to be equal to the velocity value itself, right?

So now I'm just going to call this as monitor point velocity. When you type in a space, fluent is automatically going to replace that with a hyphen. That is very, very handy. You don't have to type hyphen on your own. And I'm just going to be looking at the velocity. So make sure that the field variable is velocity. And in particular, we are looking at velocity magnitude. Now, you can also look at the x component of velocity specifically. But in my case, I'm interested in seeing how the velocity core magnitude fluctuates.

And from that fluctuation, I might be able to calculate a frequency, right? And that is why I'm choosing velocity magnitude. You should be able to do that with looking at the x component of velocity as well. But it's just a personal preference. I like looking at velocity magnitude. And I'm going to be looking at the vertex average in the location of the monitor point. So make sure that the monitor point is selected. Click on report file and report plot. The frequency is 1, meaning each and every iteration, we are going to be looking at this.

So let's just click OK. All right. Now, in addition to this, what I want to do is I want to create velocity plots and pressure plots, right? Contour plots. So to do that, I'm going to first use hybrid initialization. So make sure that hybrid is selected and click on t equal to 0. And that's going to initialize your domain. So now your domain would contain some, you know, initial values of velocities with which I can set up my contour plots, right? So go to post-processing and click on contours and click on new.

The first contour is going to be velocity. And I'm going to be using something called as a field option. And we're just going to select everything. And we're just going to click on. Oops. Before I click on save and display, I'm just going to make sure that I actually look at velocity. So let's click on save and display. Compute. And if you go to graphics, you can actually see the initial velocity that was obtained by the hybrid initialization. This is not the final solution. So let me close this guy.

And then we're going to click on contours again. Click on new. And this time we're going to be looking at pressure. So make sure that you select pressure. It is very easy to miss selecting the contours that you're actually interested in. Sometimes I just change the name here and I actually don't change the variable, right? It has happened to me a lot of times. So then make sure that you click on filled. You know, you can use a banded color map or smooth color map. It really doesn't matter.

And I'm just going to select all of my components. And I'm just going to click on save and display. And just click on compute. So here you can see that the pressure is actually all zeros, which is perfectly fine. Don't worry about it. This is just the initial condition. So now we actually have to go back to solving, right? And this is where I said the workflow is kind of non-intuitive, but you will get used to it once you set up, you know, two or three simulation.

For the solution method, we are going to be sticking with the simple method. And, you know, we are going to be looking at the residuals for continuity, x-velocity, y-velocity. X-velocity and y-velocity basically represent the residuals from your x-momentum and y-momentum equation. Now I'm going to uncheck these convergence criteria, right? And I'm just going to click on OK. Why did I do that? I want to make sure that I see the solution till the number of iterations that I input. Sometimes what you might have noticed is you might put in a large number of iterations, but the solution would stop much before that.

And sometimes that's actually not very good because it could be that the physics in your particular problem takes a little bit of time to evolve. And in the initial phases, nothing is happening. So things might actually converge very, very quickly and fluent might think that you have a converse solution. So I don't like that. So that's why I like to provide, you know, my own number of iterations. Sometimes this also doesn't work. It's always important to make sure that your solutions have actually converged. And when I say solution, I'm not talking only about the residuals.

I'm talking about some type of a physical parameter, which is important for you. So in our case, that could be the velocity in the monitor point location.

Part 2

All right. So now I'm just going to hit calculate. And when I do that, you can see that my scaled residuals are there and my monitor point velocity is also appearing. So you can see that the velocity is fairly flat. We are about 200, 225, 250 iterations, 350 iterations and nothing is happening. Right. And our velocity. And let's take a look at the velocity plot. So we are just going to click on display. Okay. And we are just going to display pressure as well. You know, you really can't say anything. One thing that I can say for sure is that there is no wattage shedding because my velocity line velocity at the monitor point location was not at all fluctuating. So that's bad. One thing that I want to make sure is since the solution is going to change as a function of iteration, it might be a good idea to add some animations. So I'm going to go to activities. I'm going to click on create.

And I'm going to click on solution animations. And they're going to be looking only at the velocity animation. Let us say that we store the values after every 10 iteration or, you know, if you're doing a transient simulation, then you might see time step there. Right. So let's type in a value of 10. Make sure that you select velocity and then click on OK. OK, so that since we have already named a contour plot with velocity, I don't think it's allowing me to add a velocity object.

So let me try that again. Go to solution commands and I'm going to call this velocity animation and type in 10 here. Click on velocity again and click OK. All right. Looks like that worked. So if you click on edit, you can see that velocity animation is there, but there's no data. Right. That's because we ran the simulation first and then we tried to set up the animation. Right. So it doesn't work that way. So unfortunately, what you have to do is you have to initialize your solution again, which I like to do.

And then rerun the calculation from the start. So now if we go to graphics, you can see that this window is actually updating. Right. So that means after each 10 iterations, we are actually looking at the velocity, but the flow has actually reached a steady state. And that's why you don't see any variation. OK, so looks like the solution is complete. And if you look at our residuals, it's kind of behaving funny. It has dropped below one E minus three. So you can call it converged, but it's not continuously dropping.

And if you look at the monitor point velocity, this is what I said. It comes down straight and doesn't change at all. So let's click on solution animation playback. And as you're going to play it, you can see that the solution becomes steady quite easily. Right. So there you go. So the solution no longer changes. Now, this is kind of bad. Why? We did update a solution, but it did not simulate the physics that we were looking for. Now, we know for sure that when your Reynolds number is close to 40, you're supposed to see one common vortices.

So I'm just going to go to setting up physics, make sure that my viscosity is correct. And it is. So it looks like I've set up everything correctly. So the one parameter that I can try changing is my computational mesh. So what I'm going to do is I'm just going to close this guy, click OK, and then I'm going to click on computational mesh. So now what I'm going to do is under the mesh parameter from two meters, I'm just going to modify this to one meter.

Right. We'll see if that actually helps out. If it doesn't, we have to come back and refine it further. So now we have a one meter base mesh. We still have our inflation layers and all that stuff. So this is good. So let's close this guy and make sure that you right click and update your mesh block. And then we are going to right click our setup and update that as well. All right. So it looks like the update is complete. So let me click on Amsys Fluent and make sure the double precision and parallel option have been selected.

Click on OK. All right. So I'm going to directly go to solve right now. And I'm just going to click on T equal to zero and I'm going to delete my previous solution because I don't want it. And then let's try running the case again. Right. So the only thing that we have done is we have modified our mesh and we're going to be looking at the computational mesh right now. So you can see that the behavior still seems to be the same. There is really no difference.

OK. And just for completeness, I'm just going to be looking at the animation as well. To see if I can see some kind of minimal vortex shedding. Right. And there's nothing here. That's bad. So let's go back, close this and refine our computational mesh one more time. So let me click on my mesh and make sure that this time the element size is 0.5 meters. And right click, generate mesh. OK. So the mesh is definitely much finer. We are going to close this guy. Right click, update the mesh.

And this time I'm directly going to open up Asys Fluent. And when I click on OK, it's going to say, hey, the mesh upstream has been updated. Do you want to use it? Yeah, absolutely. Click on yes. So right. It's two ways to do the same thing. And then click OK here as well. And one thing you always need to do is you need to make sure that the mesh has loaded. So always make sure that the most recent change is shown here. Right. So the mesh seems updated.

Let me actually go back to the material properties and make sure that it looks correct. So yes, it does look correct. So let me close this guy, go to solving, initialize the domain one more time, 350 iterations and let's hit calculate. So we're kind of starting to see the same pattern. The velocity is dropping. 160, 160 iterations. Okay, so this time I think I saw a very small blip right there, but it doesn't mean anything. Right. So I'm pretty sure if I look at the animations right now, it's not going to show me any type of vortex shading.

Right. So I'm going to try refining my mesh one more time. Right. And this is something that you need to do. This process that we are trying to follow is what you would call as a consistency check or even a grid dependence test. But I don't want to call it a grid dependence test because we still haven't captured, you know, the fundamental physics that we are looking for, which is seeing the vortex shedding in action. Right. So I'm just going to minimize this guy or actually close it and then go back to the computational mesh.

Click on our computational mesh and go to 0.25. I know that this is a lot, but let us see. Let's click on generate mesh. Okay. You can see that that mesh is super fine. Right. And I want to just go to the statistics and look at the number of elements. So you can see that we have about 40,000 elements, which you should still be able to simulate even with an academic license. So let's close this guy. And right click update our mesh. And then let's double click, click the setup and make sure that the mesh is updated.

Click OK. You can see that the mesh has definitely been updated because it's super fine. Let's go to solving directly, initialize everything so that we get rid of all the animations that we have created. And I'm just going to check my material property one more time. I like to do this because a couple of times, for some reason, the material property got back to the original value, which I'm pretty sure I have done something wrong because it has not happened before. But now it does look correct.

So let's actually go back to solving and hit calculate. So one thing that you need to understand that is when you refine the mesh, you need to run the simulation for a much more longer time. So what we're going to do is in this particular case, if it doesn't seem to be forming any vortices for, you know, 350 iterations, we might have to run it a bit longer because it still hasn't reached kind of that steady state value that we have been seeing so far. All right. So it looks like the solution is complete. So I'm going to run it for another additional 150 iterations and click on calculate.

And I'm going to say that, hey, use the settings only for the current calculation. Right. So let's click on OK. Go to the console and we're just going to be running it for a little bit more time. So now before deciding if I have to run this a little bit more or not, what I'm going to do is I'm going to go to the solution playback and play the animation because the information has still not passed through the outlet, meaning we might have not run the simulation long enough.

And that's what I was telling earlier. When you are coarsening, when you are making the mesh finer, you always need to run it for a longer time. So I'm going to go ahead and run it for 300 more iterations. Right. So in total, we have already run 500 iterations and running for 300 more. And just make sure that you click on the first option. And so that it continues to solve from there. So you can see that at this point, we can pretty much conclude that the vortex shedding is not happening.

So what could be the reason? Right. So I mentioned last time that, you know, at the Reynolds number 40 is when the flow becomes flow starts to become critical. So what we're going to do is we're going to slightly increase the Reynolds number to see if we're able to capture the vortex shedding. So I'm just going to set this to 0.045 and click on change and close. Right. So we are. So we change it only a little bit so that it goes above the critical Reynolds number value.

Right. And let's go to solve. Make sure that we initialize everything. And we'll just clear all the objects that we have created and set this up to 350 and click on calculate. So now let's take a look at the monitor point velocity. It is dropping as usual. And this is when I think it's going to start and hit that steady value. But if the flow has to become not unstable, but if the vortices have to start to shed, then it has to happen sometime right now.

So we're just going to run this a little bit longer, maybe up to 600 iterations. So that clearly did not help as well. So what I'm going to do is next, I'm just going to push my Reynolds number to a value where I know for sure that there's going to be a lot of vortex shedding. And that is our last case, which is Reynolds number of 100. So what we're going to do is we're going to go back to setting up, sorry, setting up physics, go back to the material properties and set this guy to 0.0 tool.

So that's a really small number. Click on change. Click on close. Go to solving. Re-initialize everything. And set this to 350, which was our original value and hit calculate. So let's look at the monitor point velocity. So it looks like you can see now that at 160, things are starting to oscillate, right? You can see that your velocity is starting to oscillate. And if I go to my velocity plot, there you see it, right? Now, I know that I kind of took you guys over this, you know, complex process, right, of obtaining a solution.

So there's a reason why I did that. So in this particular case, I know that this is the condition in which the vortex would get formed. But that's not the typical process that you follow when you set up a simulation, right? You start by making guesses. And initially, you don't know a lot, right? You don't know what the results are going to look like. So you need to make sure that you change properties one at a time till you get the desired result, right? And when you change a property, for example, in our case, we modified the grid.

So those are steps in the right direction. Similarly, we increased the Reynolds number because we were not able to see the vortex shedding at a Reynolds number of 40 and Reynolds number slightly higher than 40, right? Now, it has been documented that when Reynolds number is around 40, your vortex shedding should take place. Now, why did we not see that? Well, it could be because of multiple reasons. And one reason which I think this is happening is because of the type of simulation that we are running.

Now, here's the thing, right? So you can see that this looks pretty realistic, right? You can see that what is this R shedding? This looks like a real realistic flow over a cylinder case that you might have seen. However, there is a lot of things going on here, right? So, for example, if I look at the monitor point, you can see that the solution has still not reached a steady state. So which means we have to run this longer. And also, you can see that there is a particular frequency to this oscillation.

If I measure peak to peak and if I know the time, then I can calculate a vortex shedding frequency from which I can calculate a straw hall number. But I think this is where the problem is. We are using a steady state simulation and steady state simulations are typically performed to get your final answers. So any intermediary solution that you get is not time accurate, meaning at 250 iteration, you know, I get a particular value for velocity, right? This does not correlate to a particular time.

And I think this is why we were not able to get an accurate result. And anyways, now that we do see vortex shedding, we will not be able to calculate the frequency parameter, the vortex frequency. In other words, you know, how many times a second does the velocity actually flip like this? I won't be able to calculate this because there is no time parameter. And that is why we need to run what you call as a transient simulations, right? In a transient simulation, what you do is you solve equations with respect to time.

So each and every time or each and every time step, you solve equations accurately, meaning you can actually trust that result. And I think and my guess is because of that, we were unable to see the vortex shedding at a Reynolds number of 40. So what we are going to do now is we are going to set, we are going to use the same mesh. So let's go to setting up domain, actually setting up physics. We are going to be using a transient simulation, all right?

And we are going to be using pressure based method, right? There's no changing that. And we are going to go to solving. And we are going to use a time step size of 0.1 second, right? And we are going to be, say, running this for 500 time steps. And let me go to setting up physics, change my material property to 0.05, which is the original value that we had. And then what we are going to do is I'm going to click on manage and I'm just going to save.

So now what we are going to do is we are going to run this guy. Now 500 time steps is a lot. We are going to make sure that we use the settings for the future calculations as well. And we are going to click on OK. Now this process, oops, I'm just going to click on stop at the end of the time step. Click OK. I'm going to reinitialize everything so that, you know, we get rid of our steady state simulation results. And I'm going to run the simulation from first.

So we are just going to wait for this to run and check back later. So it took a lot of time to solve, but it did solve. And the exciting thing is we were able to actually see the vortex shooting. Whereas when we did the steady state simulation, we were not able to see it. And that is exactly my point. Then the problem is transient in nature. In other words, when you are looking for a quantity that's changing as a function of time, and if you want to accurately capture it, then you better use a transient simulation.

And on top of that, your mesh needs to be refined. All right. Now, based upon the things that you learned in this particular video, I know that we kind of, you know, did things in a chaotic order, but all of that was actually planned. I know that this is the right answer. But the reason why I actually took you down that path, because that is the way in which you would actually think about a problem. Right. So based upon the concepts that we have discussed, I have a series of challenges that I have provided for you guys.

Take a look at it and try to solve it and let us know if you have any questions. Thanks. Bye.

Want the rest of Introduction to GUI based CFD using ANSYS Fluent?

Get the full course syllabus and fees.

The full course is paid (₹40,000). We'll send the syllabus and call you back within one working day.

Talk to a career counsellor

Free 20-minute call. We'll map the right course to where you want to work.

By submitting you agree to our Terms and Privacy Policy.

Full course · paid

Unlock the full Introduction to GUI based CFD using ANSYS Fluent course

The remaining 8 lessons, mentor-reviewed projects and a certificate come with the paid course (₹40,000). Leave your details: we'll send the syllabus and fees and call you back.

Get the syllabus and fees

A counsellor calls you back within one working day.

By submitting you agree to our Terms and Privacy Policy.

Grow by Skill-Lync · free lesson

Start watching

Free, no payment. Leave your details once and every free lesson on Grow plays straight away. A Skill-Lync counsellor may call you about the full Introduction to GUI based CFD using ANSYS Fluent course.

By submitting you agree to our Terms and Privacy Policy.

Talk to a career counsellor

Talk to a career counsellor

Free 20-minute call. We'll map the right course to where you want to work.

By submitting you agree to our Terms and Privacy Policy.