Flow arround a train in a tunnel
 

Hello to everyone. I'm new in CFD and I really need your help.
I'm trying to simulate a flow arround a train in a tunnel so the train is represented by a box and the tunnel by an enclosure.so the problem is same like an elevator problem. The length of the train is 0.7m while the length of the enclosure is 7m in front the train and 7m behind the train. My scheme is: a fixed train in space while air and walls pass by at a constant speed. The walls are moving walls in translational motion relative to adjacent cell zone. The solver is "pressure-based", "k-epsilon Realizable" model with "non-equilibrium wall functions", boundary condition on "velocity inlet" and "pressure outlet", solution methods scheme is:
1) for first 100 iter: "simple" with "first order upwind" for momentum , turbulent Kinetic Energy and Turbulent dissipation rate
2)after 100 iter: "simple" with "second order upwind" for momentum , turbulent Kinetic Energy and Turbulent dissipation rate

Is it a good conditions for my case?

After 2000 iter I got these results:
1)scaled residuals reach the number 1.65e-02 oscillating between 1.6e-02 and 1.7e-02
2)velocity in x,y and z directions reach 1.36e-05, 1.06e-05 and 8.42e-06 respectively with small oscillations arround that values
3)k and epsilon reach 3.7e-05 and 1.02e-04 respectively with small oscillations arround that values.

Can I consider it as convergence?

And also the mesh have to be fixed or I must impose some condition to make it sliding and how to do it?

Hi Artur,

If you don't consider the in- and outlet of the tunnel but only the constant internal part, using a moving wall sounds fine to me.

In terms of convergence, the residual of 10^-2 is a bit high, but the residuals themselves are relative values and therefore not the best way to judge absolute convergence. What would be better is to:

- set something like volume-mean velocity, or another (integral) parameter of interest as a monitor
- see when that reaches a constant value.

This is a better monitor for convergence, if that quantity oscillates the solution is not converged, regardless the residuals.

Anyway, I guess with 10^-2 residual (for momentum I guess?) you should probably iterate a bit more. Did you try lowering the underrelaxation factors? Or refining your mesh in regions where you expect steep gradients?

Best,
Cees

I agree with Cees.
Residual is just one of the many kind of criteria for convergence. you need another parameters. If you are interested in drag, friction, mean velocity, pressure, or whatever, you should check the variation of the very parameter directly.


And, I guess residual of 10e-2 is continuity.
If it is, it may be because of the intrinsic unsteadiness of blunt body: mainly by vortex shedding behind the blunt body.
If you are interested in the flow itself near the train, you should use transient solver.


Plus, I heard that the number of iteration is also important in simulating external flow. I was advised to keep calculating, watching parameters, even though the default residual criterion is satisfied.

Thank you a lot.
Yes 10e-2 is residual continuity.
And yes I am interested in external flow arround the body.
I refined the mesh with a "box of influence" where I expect gradients and I can't refine it anymore because I got an old computer and I reach the maximum number of elements it can resolve in fluent.
Now I will try to iterate some more, lowering the underrelaxation factors.
Can you explain me what is a transient solver and how I can set it?
Thank you a lot again.

Hi Artur,

I also agree on the number of iterations - I see that clearly in stirred tank simulations, where the residuals may be satisfied but the flow did not reach the expected pattern yet.

Regarding transient simulation; you can set it under solution setup --> general --> transient.

There are a few more things to set now. Under solution methods you can choose if you want 1st or 2nd order time stepping (same as with spatial discretization, a trade-off between speed and accuracy). In the `run calculation' part you can set number of timesteps, timestep size and iterations per timestep.

The number of iterations per timestep should be somewhere between 20 and 50. (You don't need that many, because in transient the solution of t is the initialization for t+1, and the 2 should be rather close to eachother). If you need much less, take bigger timesteps. If you need more than 50, you are likely better off taking smaller timesteps.

Best,
Cees

CheesH and swtbkim thank you a lot. I will follow your advices and run another simulation.

Best regards.
Artur.

I got another question:
What kind of "viscous model" should I use? Is it ok to use "k-epsilon" or should I choose another model?

Well, k-e is based on the assumption of isotropic turbulence, which does work well in unidirectional (pipe) flows typically, but not so much in boundary layers. It depends a bit on what you want to know, and how accurate you want it to be. So my suggestion there would be to look at:

- What is the theory/assumption behind different turbulence models
- Under what conditions are they known to operate well, and under what conditions not
- what is the degree of accuracy I want

Remember, it is very likely you will get some results, but how good they are depends fully on the things you set, assume, and how well you understand them. So do make sure you know what the background of your models is.

Thank you. You helped me a lot.

Just FYI, I'm simulating a flow around a car, especially inside the wheelhouse and I decided to use sst k-w model, because it is known as well-predicting the separation of boundary layer.

I compared some papers, authors' comments about their turbulence model, and considered Fluent Theory guide Ch.4 Turbulence.

Choosing turbulence model is very difficult stuff. A lot of CFD papers consist of comparing many turbulence models and experimental values and suggesting that this model is suitable in this case.


In my very personal opinion, sst k-w model is ok in your case, too. but i'm not sure.

It will be also very good to try a few models and validate them

Thank you. Now I'm reading some papers too, about turbulence models. It's the first time I use a CFD and I'm very glad I found You. You helped me a lot!