I am simulating a transient supersonic flow in CD nozzle. After the flow has evolved, the solution is reaching steady-state. What might be the reason the reason for it? It seems that with each time step the transient character of the flow is damping till it reaches steady state.
First of all, are you sure that your flow problem must show an unsteady solution?
Then, if the physical solution is unsteady, the fact that your numerical solution converges to a steady state can depend on several factors, the numerical viscosity, the grid resolution, not physical inflow conditions, etc.
You should provide more details
Filippo Maria Denaro I am sure that the flow i am interested in is unsteady in nature. To capture the shock oscillations I have chosen a very fine mesh with cell edge length of 0.9 mm. So, initially I am able to capture the shock oscillations but after about half cycle the amplitude of the oscillation reduces and finally it dies out with only small fluctuations in the solution.
Even the time step I have taken is of the order of 10^-7 s.
If there is artificial viscosity that can strongly dump the unsteady feature of the flow. The shock thickenss is O(10^-6) m therefore the grid size is far from a resolution of the shock
@Filipino Yes it is true that the shock thickness is or the order of e-6 but my objective is to capture its oscillations which are of the order of about 10mm, for that the mesh resolution of 1mm seems fine to me. Moreover I am getting oscillations initially that should also not have come if the fineness of the mesh was a problem. Isn't it??
You cannot think to describe the movement of the shock correctly if the grid size is at least 1000 times greater than the shock thickness. To capture the shock it is likely you are using some dissipative scheme. They can capture a steady shock but if you have to describe the movement of o shock wave in an interval of 10 mm you need of a finer grid and a very accurate scheme.
OK thanks. So are you suggesting to further reduce mesh size to about e-7 in the domain where the oscillations are happening?
If yes, can you suggest some way to reduce the total number of nodes?
Earlier it was about 6 million nodes approx.
What you are tryng to do is more similar to a DNS/LES approach where you want to describe physical oscillation on a small lenght scale. That will have a computational cost. You can try to refine the zone of 10 mm with a mesh size of 10^-2 mm and relax the grid outside. That depends on the structured or unstructured grid, on the use of multiblock, etc. I suggest first to search in literature for a similar problem and follow the same techique.
Sourabh Bhardwaj , Filippo Maria Denaro : This should not come as a surprise to many, who analyze numerical schemes. This is pure and simple, due to the so-called stable algorithm! Numerical diffusion takes care of any unsteadiness. And also, the shock thickness actually being of the order of mean free path, do not think of even resolving shock!!! You are working with continuum model. Readers may like to go back to the basics of computing shocks with continuum model. What is badly needed is an honest analysis of the scheme used. Does anyone know the numerical dispersion relation? We have in the past very effectively shown transonic shock oscillation with dispersion relation preserving (DRP) schemes. Also another nice problem is dynamic stall of aerofoil, which has been captured by us.
Unfortunately, he is using Fluent and the best he can do is standard second order discretization. The only parameter he can control is the grid size and time step. Hoping that can reduce the numerical diffusion introduced by Fluent. Of course I assume that all the BCs setting are correct, some further check could be useful
sir Filippo Maria Denaro , what is better software than FLUENT to remove this convergence issue?? assuming similar discretization sscheme..
regards
Often, if you have to analyse one specific flow problem, the best sowftware is a own-made code. In this case, a high order method in time and space should be used such as WENO.
As sir Tapan K. Sengupta mentioned, you wont meet your objective by using a commercial tool. Often not only mesh that is important for solving a problem, also the schemes which we use for solving the problem is very important. So better idea is to write your own code using DRP (dispersion relation preserving) schemes.
Filippo Maria Denaro The BCs have been set properly as I have got some solutions which were in close agreement with the documented data. You are correct that I only have the freedom to resolve the mesh further or reduce the time step which already is so low.
I read it somewhere that to capture the unsteadiness of pressure waves we need to opt for explicit time formulation, but that too doesn't help much.
Atchyut Gullapalli , Atchyut Gullapalli, Tapan K. Sengupta Even I feel for that I may have to switch to a non-commercial codes to solve the problem accurately with a very high spatial and temporal resolution.
Sourabh Bhardwaj
Your flow problem is quite challenging, could you show more details?
How about the present setting you are using?
Filippo Maria Denaro I am using a Density based solver with k-omega SST turbulence model, Explicit formulation and Roe-FDS flux formulation and maintaining a CFL of 0.6.
Well, I think that this RANS formulation is not suitable to describe an unsteady flow problem as the yours. Try setting LES formulation and low diffusion Roe flux-difference splitting. However, I am quite sure you cannot solve accurately this problem using Fluent.
Filippo Maria Denaro I will try doing similar simulations later on using LES. Thanks for all your help. Appreciate it.
- Badges
- Science topic