[tschultz]

I am running a simulation on steady 3D laminar air flow (v=100 m/s)across a sphere and looking to calculate the coefficient of drag. I set the monitor to report and plot the coefficient of drag but the numbers converge down to Cd's around 0.001.

Is it too ambitious to expect CFD results to match experimental results? I do not understand why these results are reporting so low. Any help would be appreciated.

Thank you.

[`e`]

Have you ensured your reference values are correct? Fluent uses these reference values for calculating coefficients; including the drag and lift coefficients.

[Darius]

Did you set your residual on 0.001 or it converged by itself on that? What are the imbalances? It should be less than 1%

To be honest I've got the same problem but mine converges on 0.000001 and everything looks Ok except the results compare to the wind tunnel test data

[tschultz]

Originally Posted by Darius

Did you set your residual on 0.001 or it converged by itself on that? What are the imbalances? It should be less than 1%

To be honest I've got the same problem but mine converges on 0.000001 and everything looks Ok except the results compare to the wind tunnel test data

Darius, I must admit I am new to FLUENT and am fumbling around quite a bit. Can you clarify on how to check/set residuals and imbalances?

Thanks again

[Darius]

In the fluent setting list on the left side...you set the iterations which 200 should be perfect for the laminar flow, the other one is the Timescale factor which in your case 10 would be fine and the last one is the Residual Target that should be set to 0.000001 which defines the limit of your convergence (it means the fluent will solve the Navier stoke equations till the residuals reach as low as 0.000001).... just click on the tabs and you'll find them.

[tschultz]

I went to Monitors> Residuals > Edit > and set all the residuals' absolute criteria to 1e-6. I ran the simulation again after than and here is what my residual plot looks like

[tschultz]

Also, my Cd plot:

[Darius]

Your model is a sphere and you should setup a transient simulation of a transient vortex shedding which is different than a laminar flow over an airfoil... that's why you get these weird results....
Search in google for fluent vortex shedding tutorial and you get lots of infos

[`e`]

Originally Posted by `e`

Have you ensured your reference values are correct? Fluent uses these reference values for calculating coefficients; including the drag and lift coefficients.

Have you read my suggestion yet? Also, Darius is correct, there is most likely vortex shedding in your setup which would require an unsteady simulation.

[Darius]

The iterations should be set to 2000 and your timesteps to 0.01 and also total time or timescale on 20

[Darius]

You also have to change the analysis type to transient

[tschultz]

e- Yes I checked the reference values and they check out ok.

I will start researching the vortex shedding tutorial now. Thank you both.

Darius, you mentioned that you have a simulation that correlates well to experimental data. Is there any way that I can see your particular setup?

I appreciate your help. I am doing a project where we kind of got thrown into the deep end so im really scrounging for help at this point.

[Darius]

I'm running my simulation in CFX not fluent and it's on an airfoil not a sphere .. I also have problem with the results I get from CFX and doesn't correlates with the wind tunnel test I made before... I don't think it would be useful for you but if you want I can upload it on google drive and share it with you if you give me ur email

[Darius]

There're the pictures... the one I rotated with solidworks give better results

[tschultz]

I changed my parameters to unsteady to iterate over a few time steps and the residuals set to 1e-6. Then I set it for 1000 iterations per time step and it converged reasonably well. However, it never met the criteria and cycled at the 1000 iteration limit. The results came back looking somewhat reasonable, but still not quite there.

I read on another source that the computer platform can significantly affect the convergence. It was interesting because I following a tutorial on flow past a 2D cylinder and my setup was identical to the tutorial... while his met the criteria within 50 iterations, mine was not so lucky.

Do you think the differences in computing power can affect the rate of convergence? That seems a little odd, but it appears that we had exact setups so im not sure what the problem could really be.

[flotus1]

Originally Posted by tschultz

mine was not so lucky.

Fortunately for you, luck can be eliminated from CFD results by providing reasonable setup parameters. Let me take a few guesses:

Time step size too large.
No transient simulation takes 1000 Iterations per time step to converge with a properly estimated time step size.
We had this topic here and there for example.

Inappropriate turbulence modeling.
Estimate the Reynolds number of the flow and tell us about it.
Use at least a standard K-epsilon model if the flow is turbulent instead of performing an under-resolved DNS.

As already stated: wrong reference values.
Or wrong direction for the drag force in the Cd monitor. Feel free to post the values you used.

A few other things: Extent of the computational domain, boundary conditions at outer boundaries, mesh quality...

[tschultz]

Here is my setup as I have it:

General:
Pressure-Based, Transient, Absolute, Planar
Model:
K-Epsilon (standard with standard wall treatment). I left the values at default.
Material: air
Boundary Conditions:
Inlet- Velocity (1 m/s)
wall- wall type with 0 shear condition
cylinder (object of interest)- no slip wall
Reference Values:
Everything is air properties.

Solution Method: coupled with everything default except 2nd order transient formulation.
Flow courant number: default at 200 (This I am not so sure of its affect, any thoughts?). Everything in the Solutions controls was left default.
Monitors: My drag monitor is printing and plotting for the cylinder wall zone. Force Vector in the X=1.
Initialization: Hybrid Initialization

I am running the calculation at 0.01 second time steps (10 steps total) and I set the Iterations/time step to 100.


As you can see from the pictures. It is pretty crazy. Anybody see anything that I may be doing wrong?

Note the first two iterations went well (actually converged within 60 iterations)

Thanks again everybody

[flotus1]

Once again, read this thread carefully and follow the procedure outlined there to estimate a suitable time step size and total simulation time.

wall- wall type with 0 shear condition

Use symmetry boundary conditions instead.
Zero shear walls and symmetry boundary conditions are not the same when a turbulence model is activated.

Reference Values:
Everything is air properties.

The drag coefficient is calculated from this formula:



Make sure to set reference density, velocity and area to suitable values.

General:
Pressure-Based, Transient, Absolute, Planar

Planar 2D basically means you are simulating a cylinder, not a sphere.

Solution Method: coupled with everything default except 2nd order transient formulation.

Use SIMPLE pressure velocity coupling unless you have a very good reason not to do so.


Apart from these issues, we need to see a closeup of the mesh around the "cylinder" wall.

[tschultz]

Here is a picture of the meshing near the cylinder. I used the inflation feature to increase the density of the mesh near the surface.

I changed the time step to 1.875s modeled after the thread you were involved with. I am trying to run 10 time steps with 75 iterations per time step.

Changed the Method to SIMPLE with second order transient. Turbulence model is still default K-epsilon. And lastly, I changed the boundary condition at the wall to symmetry.

I calculated the Reynolds value based on the reference values and I am looking at something around 7000 (expecting a Cd of between 0.5 and 1.0).

After running the simulation with this setup, I get similarly volatile residual convergence. (see attached) and the Cd convergence plot blew up.

I am doing just the 10 iterations to get a sneak peak at the results. Would you expect a simulation to have unreasonable results in the first few iterations and then settle in over time? Or is this still unprecedented?

For the Inlet, I have the turbulence set: Turbulent intensity= 0.5% and Turbulent Viscosity Ratio = 10. Is this significant?

Thoughts? Thanks again

[flotus1]

The mesh near the cylinder looks weird to say the least.
Since your Reynolds number is rather low, you do not need such a high mesh density near the wall. Reduce the number of cells in the boundary layer untill you can at least see the individual mesh lines in the closeup picture and then post picture here.
Additionally, check maximum skewness value of the cells in the meshing application and post the text message fluent gives you when you click on "mesh" -> "check"

The overall mesh density is rather high especially in regions far away from the cylinder. You can increase the overall mesh size to get faster convergence.

I dont know how you estimated a time step size of 1.875s.
What is the diameter of the cylinder?

It is normal that the results after 10 iterations have nothing to do with the final results of the converged solution. Dont worry about that.