Hi !

I am trying at thebbeginning of my problem, to simulate a flow induced by natural convection in an open chemney with heated walls. I cannot reach convergence even the residuals are very stable but high (0.001 for energy, 0.1 for continuity) I I lower Under relaxation factors to 0.001, it converges immediatly. I hear that in theory we can take URF very low, but this seems kind of weird. Do you have any advice on that ?

Thank you so much for your help !

Marie Anne

New Value = Old Value + Omega * Correction Where Omega (The under relaxation parameter) can take any value from 0 -> 1 So the value you used looks small but it takes the solver to the right path of convergence. As the solution proceeds you can increase these parameters Cheers

Thank you for this precision Ahmed. The thing is that if I take back up the URF again, the residuals go up again... I guess it is that in fact they go low with low URF because the correction is around 1. Does it mean my problem converges ?

Thank you !

Shouldn't the correction get smaller as you approach convergence?

Yes it should. That s why I don t know if I am approaching convergence. It is just the residuals which are going down...

1- Are you using a commercial programme ? 2- What is the quality of your mesh ? 3- Are you using corrct Boundary Conditions ? If you are happy with all the factors that affect convergence, then initialize your domain with zero values for all variables , use small under relaxation parameters and go for a coffee break. Good Luck

A taylor series expansion will tell you that the errors are functions of delta x, so you might need to remesh you domain

Thanks for that. I use Fluent and run today my problem in transient mode. It converges then very easely. Do you have a good explanation for that ?

Thank you

Hi Marie,

yes you have hit on something that we often see. One can show that an under-relaxation factor and using a physical time step for under-relaxation are similar. In fact one can show that a fixed under-relaxation factor is equivalent to using a different time step in each volume. See section 8.8 of Versteeg and Malalasekera.

Basically if the problem is easy to solve you will not see much difference in the two approaches above. However if the problem must "evolve in a physically reasonable sequence" to remain solvable then the constant physical time step usually has advantages. Natural convection is certainly one of these where letting each equation in each cell wander off to different physical times at each step....probably leads to a mess!

I personally think it is a better approach in many cases. There are, however problems which have a wide disparity of time scales the under-relaxation approach can be better as pseudo-transient time marching will be limited to a small time step that captures the fastest process.

Very interesting topic.......

Tell me how did you choose your time step?

Regards,

Bak_Flow

Thank you so much for your response and reference to Versteeg and Malalasekera. This book is clear, great, useful...:a treasure. I hadn't really chosen the time step based on previous URF since these didn't work well. having a major drop in residuals with a major drop in URF was I think indeed due to the fact that not much difference could exist between two iteration since not a big variation was allowed by such small URF. I will try to compare URF at wich I get a start of convergence(stability of the mass flow rate)and the time step. I will let you know of the results if you are interested.

Thanks again,

Marie Anne

First my apologies for not being able to answer your question earlier. Before trying to answer your question I would like you to clarify the following:

1- What is the Rayleigh number in your domain?

2- Do you get the message "solution converged" at the end of each time step of your unsteady simulation or does the solver completes the specified number of iterations per time step and starts another time step

3- Could you post your mesh somewhere on the web, I would like to check the quality of your mesh

Cheers and Good luck.

[bitak]

Hi.
I work on project about subsonic ejector like you.
My solve is :air - couple - axisymetric - k-e rng - pressure inlet and outlet ideal gas - my presure inlet are 150 ,250 ,350 ,450 Kpa and out let is atmosphere.
unfortunately my solve is divergence!!!!!!!!!
really I need to your help.
I change k-e to k-omega and pressure inlet to mass flow but devegence again.I know i have a shoke and so reverse flow in fluent.