Grid Independence with discretization schemes
I have been testing the grid independence to a particular case by verifying the results from the first order and second order discretization schemes.
The discretization scheme in CFX could be changed using the advection settings. However, I just started up with Fluent now and it is required to separately choose a discretization scheme for momentum and pressure in Fluent. So when I contacted Ansys support over this, I was told that it would be enough to just change the discretization for momentum from 1st order to 2nd order and leave the pressure discretization to a default scheme if my objective is only to test the grid independence but I don't really get this because " pressure " is also a transport variable and therefore needs to be considered in switching over the discretization. Could some one please explain this 
Well, pressure is not a transported variable in the same way that velocity is. Pressure is a source in the momentum equations and is introduced into the continuity equation, but it isn't governed by a usual advectiondiffusion type equation.
That being said, you are right, the way pressure is discretized will affect your solution. It just depends what you are trying to test. If you just want to know about the impact of advection schemes you should just leave the pressure scheme alone to isolate that one influence. 
Thank you very much for the clarification christopher I found it really helpful.

Let me guess. Total pressure is equal to static pressure + dynamic head (which is due to velocity). In boundary layer static pressure is almost constant in the normal direction, it is the velocity which changes. So with coarse grid and fine grid you will almost same pressure distribution, but it affect the velocity. So grid independent should be made with 2nd order momentum equation and not necessarily the pressure term.
In other words pressure term will change little in momentum equation with 2nd order scheme. Best method is the sensitivity analysis i.e. check both schemes and find the difference. 
On a more general note, there is more than just the accuracy of the advection scheme you are looking at when you do a mesh sensitivity study. There is the diffusion terms, the ability of the grid to resolve flow features and other issues. So to replace a grid sensitivity study with simply a comparison of advection schemes is to only check half the issue.
So I would recommend doing a full mesh sensitivity study as that is a more thorough assessment of the accuracy of your simulation. BTW: The seminal work on CFD accuracy is "Computational Fluid Dynamics" by Roache. If you are interested in CFD accuracy it is highly recommended. The JFE editorial guidelines (http://journaltool.asme.org/Template...umAccuracy.pdf) are a good summary of the key points. 
Good point Glenn. I didn't notice the words "grid independence" in the original post. Certainly just testing the advection scheme is not sufficient to claim grid independence.

Christopher, Glenn and Far  your comments are really interesting. Thanks a lot.

After several years experience and disappointments with similar issues ;) I have adopted the following procedure for the mesh independence study.
1. Take three meshes a) use 2nd order scheme (you can use 1st order scheme if you have convergence issues and after few iterations change to 2nd order) b) required Y+ c) Turbulence model check the important results. Like velocity, turbulence quantities and drag. What ever is important to you. 2. Access the convergence error on the finally selected mesh with varying the convergence criteria. 3. Access the 1st and 2nd order scheme on the finally selected mesh. 4. Access the Y+ effect on the finally selected mesh. For example with Kepsilon model with scalable wall functions, you will get the almost similar result. For the SST model you will get the similar results up to Y+ = 10 then results will start to deviate. For transition model you need Y+<1. In this case you have to refine the streamwise mesh along with grid independence study. One important point to note in following pic (one Figure is more than thousand words:rolleyes:) http://afinemesh.files.wordpress.com...el529x359.png http://afinemesh.files.wordpress.com...el529x359.png 
So in CFX does the discretization scheme chosen in the advection settings apply to the diffusion terms and source terms too.

The advection discretisation scheme only affects the advection term... obviously. I think the diffusion term cannot be changed from central differences (check this in the doco if this is important to you :) ). Note diffusion and advection have very different characteristics, so the issues you might be familiar with for advection do not necessarily apply to diffusion.

FYI... in CFX diffusion terms are based on the gradients that come from the element shape functions. There is some control over the shape functions (through expert parameters I think) but usually the defaults are used.

Could you please let me know how the source terms are treated in CFX.

We always told that diffusion term(scalar quantity) is discretized by the central differencing scheme and it is always second order accurate. I hope I am recalling correctly :rolleyes:
But CFX is finite element based finite volume solver. Confusing..... But finite element method is used for making the shape functions which are used to form the cells and integration points. Later on finite volume takes the control. Am I correct? 
Theory guide section 11.1.1.5 describes diffusion terms as being calculated from the element shape functions (the derivatives of the shape functions actually).
Discretization of source terms is not described as far as I can tell in the theory guide, but if it is just a volumetric source it will just be the value of the source in the control volume multiplied by its volume in the discrete control volume equations. 
Check out "Numerical heat transfer and fluid flow" by Suhas V Patankar. May be you will get an idea of how source terms are discretized and how non linearity of source terms are handled.

Sainath, Yes, that book is a good background, but it uses a finite volume approach with a segregated SIMPLE solver for PV coupling. CFX uses a finite elementlike approach with a coupled solver. The diffusion term is handled differently in a finite volume scheme to a finite element one (that is gradients are calculated by central differences versus shape functions).

My mistake. I forgot that discussions here are pertaining to CFX. Yes, the shape functions are used to evaluate the spatial derivatives for the diffusion terms by CDS.

Quote:
Glenn at the end finite volume solver is used to solve the equations. It will always be the central difference scheme whether it is being evaluated on the shape function or the control volumes. Then these coefficient will form the matrix, which is solved by the finite volume solver right? 
Method is based on finite volumes with finite element shape functions being used for interpolation. The mesh defines the finite elements and the mesh dual defines the finite volumes. Once the finite volume mesh is formed it is pretty similar to a finite volume method on that mesh except for the way interpolations are handled. There are some other differences of course but this is the major one.

Dear Ahmed why we should start by second order scheme?
and also which terms should at least be second order in fvSchemes so that a run can be called in second order totally? 
All times are GMT 4. The time now is 04:49. 