[DanielBarreiro]

Good day everyone,

At the moment I'm carrying out simulations in CFX of flow over a 2D Cylinder in a rectangular domain immersed in a high reynolds flow to determine its drag coefficient.

The goal of the simulations is to obtain a Drag Coefficient vs Reynodls curve that resembles as closely as possible the graph attached in the first image, for Cd vs Re for flow over Cylinders.

I'm using an structured mesh created in ICEM as a 2D mesh and the extruded one element in the Z direction so it can be used in ICEM. This mesh is then used in CFX to run the simulations for flows in the range of 10^4 to 10^7 Reynodls number.

When I run the simulations between 10^4 and 10^6, the results I obtain for the drag force over the cylinder, using the following expression:

force_x()@CYLINDER

provide with acceptable values of the drag coefficient, almost equal in some cases to the graph I'm trying to reproduce. The formula I use to obtain the Drag Coefficient is as follows:

Cd = force_x@CYLINDER /(0.5*DENSITY*V^2*A)

The cylinder has 1 meter in diameter, and the fluid is air at 25ºC. The velocity is dependent on the Reynolds number at which I'm running the simulation.

The problem begins when I run the simulation for Reynodls numbers between 10^6 and 10^7. In this case, using the same expression to determine the drag force in the cylinder, and then the same expression to determine the drag coefficient, the values I get are around half and a third of what the actual values should be.

Mesh:
Structured mesh, with a high resolution around the cylinder wall. The first cell element thickness is determined for a y+ value of 1.
The domain size is 10 times the diameter length in the upstream direction, and 20 times in the downstream direction, to allow the flow to fully develop and avoid any backflows or undesired effects. The width is 7 diameters in each direction as well.

Turbulence model:
SST, with no transitional turbulence, as it can be seen in the second attached image.

Type of Simulation:
Steady State

Time Steps:
Local Time Factor: 30

Convergence Criteria:
1*10^-8
(The convergence criteria is reached)

All of this can be seen in the third picture attached.

It should be mentioned as well that this problem does not appear when meassuring the Lift Coefficient, as it remains close to 0 in all simulations, independently from the Reynodls number.

Can anybody provide me with any insight into why for the initial Reynodls values, until the Drag Coefficient drop in the graph, the Cd values are more than sattisfactory, but as the Reynodls increases in the range of 10^6 to 10^7, the results are completely off? Is there obvious mistake?

Has anybody attempted to do a similar simulation with succesfull results?

It's a very simple simulation and I cannot see where there migth be some errors in the setup.

Thank very much in advance for the replies.

Daniel Barreiro

[AtoHM]

Resolution of the mesh seems to be high indeed, but still: you said the layer thickness is chosen so yplus is 1. What Reynolds number did you use to determine the neccessary cell height?

If you designed it for Re 10^4, you will get a higher yplus when simulating higher Re-number with the same mesh. This will in turn influence the boundary layer resolution and might lead to changes in the drag.


Check yplus values in post and see if its getting out of range for the higher Re-number simulations.

[DanielBarreiro]

Originally Posted by AtoHM

Resolution of the mesh seems to be high indeed, but still: you said the layer thickness is chosen so yplus is 1. What Reynolds number did you use to determine the neccessary cell height?

If you designed it for Re 10^4, you will get a higher yplus when simulating higher Re-number with the same mesh. This will in turn influence the boundary layer resolution and might lead to changes in the drag.


Check yplus values in post and see if its getting out of range for the higher Re-number simulations.

The y+ value of 1 has been calculated for a Reynolds number of 10^7, so when the simulations are run with a lower Reynodls number, the y+ value I get in CFX Post is always below 1.

Still, the results keep being innacurrate for Reynolds numbers above from 10^6.

[AtoHM]

Alright, this was just the first thing coming to mind as it was missing from your besides that very clear explanation of your setup. Maybe someone else can point to a solution.

[DanielBarreiro]

Thank you very much for the reply anyways. Let's see is someone else is able to point out the problem.

[evcelica]

What are you comparing to? Red line and blue dots are what in your first graph?
Cylinders do have this dip around the Reynolds numbers like your red line shows, I think you are already aware of that though.

First off, I have found that drag force on a 2D cylinder is actually quite a difficult simulation @ any Reynolds number due to the difficulty in CFD predicting the flow separation point around the back of the cylinder. I always got a slightly lower drag coefficient than literature, and I don't know a way to correct for this. I feel CFD could better predict a more complex geometry than this simple cylinder, which turns out to be much more dificult than one would expect.

Second, are you using incompressible air? (You stated "air @ 25C" which is incompressible). If so compressibility effects could be playing a role.
Air ideal gas may be more appropriate for starters. One step further (probably not required, but a sensitivity analysis would determine this) may be using real gas with the total energy model instead of an isothermal model.

[ghorrocks]

You are using local time scale factor. Quoting from the FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

Use Local Timescale Factor. A factor of about 5 is a good guess to start with. If this is successful you should run the final few iterations to convergence with a physical timescale (not local timescale all the way to convergence).

So you need to do the final run to convergence with physical time scale, not local time scale factor.

[DanielBarreiro]

Originally Posted by ghorrocks

You are using local time scale factor. Quoting from the FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

Use Local Timescale Factor. A factor of about 5 is a good guess to start with. If this is successful you should run the final few iterations to convergence with a physical timescale (not local timescale all the way to convergence).

So you need to do the final run to convergence with physical time scale, not local time scale factor.

I have run a few simulations with a Local Time Step of 5, as well as 10, since it's a very common value too, but I do not get consistent results, and the Cd value for Reynodls between 10^6 and 10^7 are still very far from what the actual values should be.

Any idea of what else migth be causing this problem?

[DanielBarreiro]

Originally Posted by evcelica

What are you comparing to? Red line and blue dots are what in your first graph?
Cylinders do have this dip around the Reynolds numbers like your red line shows, I think you are already aware of that though.

First off, I have found that drag force on a 2D cylinder is actually quite a difficult simulation @ any Reynolds number due to the difficulty in CFD predicting the flow separation point around the back of the cylinder. I always got a slightly lower drag coefficient than literature, and I don't know a way to correct for this. I feel CFD could better predict a more complex geometry than this simple cylinder, which turns out to be much more dificult than one would expect.

Second, are you using incompressible air? (You stated "air @ 25C" which is incompressible). If so compressibility effects could be playing a role.
Air ideal gas may be more appropriate for starters. One step further (probably not required, but a sensitivity analysis would determine this) may be using real gas with the total energy model instead of an isothermal model.

Soryy I did not make that clear enough. I'm trying to reproduce the red curve in the graph as closely as possible to validate the mesh and the turbulence model I'm using for Reynodls numbers between 10^6 and 10^7.

I'm aware of the fact that the Cd it's always a bit less compared to the actual experimental value, but in my case, the Cd values I obtain with the simulations are about half, or a third of what they should be, which is not an acceptable difference.

As you well say, the energy mode I do not think is neccesary, as it a very simple simulation that shouldn't be affected by it.

I have gone once again over my set up parameters but I do not seem to find anything unusual. Any idea of what migth be causing this problem?

[evcelica]

So the blue dots are your results?
Perhaps the transient nature of the vortex shedding is not being resolved in your steady state model. That dip in the Cd lines up pretty well with a distinct vertex shedding mode, and that dip can also change with smooth vs rough walls.

Is your entrance and exit far enough away from the cylinder?

Are you are using ideal gas or constant properties?

[DanielBarreiro]

Originally Posted by evcelica

So the blue dots are your results?
Perhaps the transient nature of the vortex shedding is not being resolved in your steady state model. That dip in the Cd lines up pretty well with a distinct vertex shedding mode, and that dip can also change with smooth vs rough walls.

Is your entrance and exit far enough away from the cylinder?

Are you are using ideal gas or constant properties?

The blue dots are my results, and the tendency is a straigth line instead of increasing once again after the dip at around 8*10^5 Reynodls number.

The domain is big enough to allow for the flow to be fully developed. Around 30 times the cylinder diameter in the downstream direction and around 10 times in the upstream direction, as well as 10 times in each width direction.

I'm using constant density for the air at 25ºC.

[evcelica]

Well I would try ideal gas first.
Then run a transient model using time steps small enough to resolve the vortex shedding.

[ghorrocks]

The dips in the CD curve are mainly due to boundary layer effects. The big drop at around 2-3E5 is due to the boundary layer becoming turbulent and staying attached longer. At Re less than this you are transitioning from Stokes flow to laminar boundary layer flow. At Re higher that 2-3E5 the separation point moves forward again so you get less pressure recovery and the CD goes up.

So if you want to model the bumps and wiggles in the CD curve the most important thing is to have a very accurate boundary layer model. If you are around the 2-3E5 point you will need a turbulence transition model to capture the turbulent boundary layer with everything else laminar. For Re above above this you will need a very good boundary layer mesh and turbulence model. For Re below this you will need to match your boundary layer mesh to the laminar boundary layer you get at that Re.

Vortex shedding is a smaller contributor to the CD curve variation. The big effect is boundary layer effects as I describe.

[evcelica]

Thanks for the info Glenn,

I am interested in this as well, and appreciate the knowledge you share.