Hello,

For finite-volume formulation (for Euler!) on unstructured triangular meshes, there are "perhaps" mainly three different approaches.

(1)Vertex-centered (2)Cell-centered (3)Cell-vertex

Which approach is the most popular one in real-world applications?

And is there any specific reason for that? (or is it just a matter of personal preference?)

I've just finished writing my own cell-centered FV code which I found the easiest to write. And I'm curious about other approaches.

Thank you very much,

Nishikawa

Between cell based and vertex based schemes, the main difference is in the storage requirements. Typically, the number of vertices in a tetrahedral mesh is 1/6th the number of cells, so storage decreases by that much. However, the counter argument is that you have 6 times more resolution with cell centered schemes. so you can argue both ways.

I have some experience with vertex based schemes. The problem there are the viscous fluxes. Using edge data structures and vertex storage obtaining mesh transparency for viscous fluxes is ellusive. THis shows up really badly for turbulent flow calculations using two-equation models. I really have not seen any two equation model calculations using cell based schemes. if you or anybody else out thre is aware of such methods do let me know! thanks

srinivasan

Could you explain a bit more about the second part?

Vertex-based method is not good for Navier-Stokes? Two-equation models are hard to implement for cell-based method?

Thank you, Nishikawa

Finally I found someone wich have interest in work with that. Recently I made a big review about this subject. Today, there are reserchers working with both cell-centered and vertex-centered schemes, but the number of publications that use the cell-vertex schemes directly are smaller. I finish to implement the convective-difusive unsteady equation with both of those methodologies. Whit this work I could verify that the cell-centered aproach is more acurated and also with the finite element method. I sugest you read the review of Frink, N.T. (Upwind Scheme for Solving the Euler Equation on Unstructured Tetrahedral Meshes, AIAA J., vol. 30, p. 70-77, 1992). In this paper the author make a good discussion about the most popular schemes. I also found some othes articles about Euler and Navier-Stokes simulation with both of those methodologies. Thank's the opportunity.

Marcio Aredes Martins Doctoral Student Mechanical Engineering Departament UNIVERSIDADE FEDERAL DE MINAS GERAIS

Thanks for your information. I'll take a look at the Frink's paper.

So, you say that the cell-centered scheme is the most accurate one among the three and FEM. Is it mainly because of the larger number of data points as Mr. Arunajatesan said in the second message? Or are there any other explanations? (such as boundary conditions)

Thank you!

Nishikawa

Hi!

Will cell centered schemes, you get better accuracy because of the increased number of data points. Also there are other accuracy issues as well.

With cell based schemes, the data point is always at the centroid of the control volume. With vertex based schemes, depending on the triangulation, the point can be very far from the centroid of the control volume enclosed by the faces on which the fluxes are computed. (see Tim Barth's papers to better understand how this happens).

Another issue is the alignment of the normal to the control volume face to the edge. These two may not always be aligned very well. THis can happen in cell based schemes also. But, with the increased number of data points this is less crucial in cell based schemes.

with the viscous fluxes, for accuracy, these fluxes have to be computed on the cell centered ans distributed back to the nodes, directly computing the fluxes on the control volumen face is not accurate enough. with the highly non linear behaviour seen in two equation turbulence models, this becomes much more pronounced.

hope this clarifies, srinivasan

Dear Collegues

I agree with Mr. (or Dr. ?) Srinivasan Arunajatesan about the cell-centered scheme. If we considered only the first order schemes, the error analisys betwen cell-centered, vertex-centered and FEM show that the first one is more acurated. I started an analisis about the matrix builded by those methods and the most obviously conclusion is that the matrix builded by the cell-centered method is the bigger, becouse it is based in the number of mesh volumes. This fact could be an bad characteristic, becouse the "bottle neck" of the code ís the solver. But, in the frist order approach, the matrix has only four non-zero position for each line while the FEM and vertex-centerd matrixes are smaller, but they have much more non-zero position. Another very interesting comment is that the cell-centered scheme is the only of then that is the "real" mass and energy balance at the cell boundary, wich is completly coerent with the traditional finite volume method.

Marcio Aredes Martins

Doctoral Student - Mechanical Engineering Department

UNIVERSIDADE FEDERAL DE MINAS GERAIS - Brazil

[elia_l]

Could someone give me a copy of that paper?
(Upwind Scheme for Solving the Euler Equation on Unstructured Tetrahedral Meshes, AIAA J., vol. 30, p. 70-77, 1992)

[shingala]

I have never heard about the vertex centered approach, can anyone please explain?

[LuckyTran]

If you have a cube, it has 6 square bounding faces, and 8 points that defines this cube. Question is which of these features you use to anchor your solution and use as values to compute all other thingies you need. For example do you use the center of the cube to compute the fluxes on the faces? Or the other way and compute the center of the cube using the values on the faces? Using the center of the cube is cell-centered, the other ways all have their methods.

FEM and pure FD is usually not cell centered and in many fields of computation that are not CFD, vertex based approaches remain the norm and are way more popular than cell centered approaches.

[shingala]

But are there any software which solves at both or something mixed approach for any legitmate reason that I dont know?

[LuckyTran]

Typically for a single physics solver you use one or the other.

In multiphysics problems you can employ multiple simultaneously. For example, you can use FVM for flow and FEM for E&M in MHD or QED problems. Or you can be like Ansys and use FEM for solids and FVM for flow.