CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

Help need on fluxes

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   August 7, 2001, 21:39
Default Help need on fluxes
  #1
Zhu
Guest
 
Posts: n/a
hi,there, I want to simulate the fluid field around a hexagonal section using the FVM and projection method(incompressible),when I deduce the FVM difference formuation,i met a problem: in order to expedite the code,i must use MG method,so the mesh which can be formed by Phoenics is appreciated,in which grid are in Cartesian coordinates but not all mesh are orthogonal,in other word,non-orthogonal Cartesian coordinate system with unequal grid space,when i integrate the equ. over the finite volume and after applying the Green's theoren,the advective term (dE/dx,dF/dy) now become E and F ,which are the fluxes on the center of the interface of the finite volume,while the diffusion term can be integrated without any difficulty,the difficult is how can i determine the spatial values of the fluxes on the interface of the finite volume,for the accuracy and stablity,i cannot use the averaged values(central difference) and first order upwind scheme,i donot know how to deal with this problem,how the Phoenics deals with this kind of problemes,does it use hybrid scheme(Patankar)?how the bybrid scheme works on non-orthogonal Cartesian coordinate system with unequal grid space on FVM.

thanks Zhu
  Reply With Quote

Old   August 8, 2001, 03:28
Default Re: Help need on fluxes
  #2
Kang, Seok Koo
Guest
 
Posts: n/a
As you stated, if you use an arithmetic mean flux of two adjacent cell as an interfacial (convective) flux, you may face some problems related to numerical oscillations. In FVM, this problem is concerned with the classical Riemann problem. When you calculate inviscid fluxes through a cell edge, you should use an approximate or sometimes exact Riemann solver to calculate them. There are many solvers such as Roe, HLL and LF etc. Patankar's techniques will not help. In addition, to obtain second-order spatial accuarcy, you'd better adopt MUSCL-type slope limiting technique. It can be implemented on arbitrary grid. Finally, to integrate semi-discret equations various time integration techniques are employed.

Best Regards,

Seok-Koo Kang
  Reply With Quote

Old   August 8, 2001, 22:35
Default Re: Help need on fluxes
  #3
Zhu
Guest
 
Posts: n/a
Thanks,Seok-Koo Kang,before I got your information,i want to use 2nd-order upwind scheme to calculate the fluxes on the interfaces of the finite volume,because my code will deal with unsteady flow,implicit scheme must be used,but i donot know how to write the flux in a uniform(or common) formulation when the advective coff.>0 or <0,will this situation also meet in the Riemann,or something like that? while,i beg you give me some reference focusing on what you said. best regards, Zhu
  Reply With Quote

Old   August 9, 2001, 06:08
Default Re: Help need on fluxes
  #4
Kang, Seok Koo
Guest
 
Posts: n/a
It is not straightforward to use Riemann solver for solving incompressible NS equations and continuity equaiton on unstructured grids, for the PDEs are not hyperbolic due to absence of time derivative term in the continuity equation. Riemann sovlers, in general, needs information on the eigenstructures of PDEs. If you want to solve these equations by those used in compressible flows calculations, I think pseudo-compressibility methods is a good choice.

If your problem of interest is not convection-dominated, actually, Riemann solver is not necessary. You can calculate the interfacial flux by simply averaging two neighboring fluxes and multiply unit outward normal vector. In 2D, the normal flux through a cell face is ( (F_left, G_left) + (F_right, G_right) ) dot (nx, ny) = ( (F_left + F_right)Nx + (G_left + G_right)Ny )/2. The sign of the flux is determined automatically.

If the upwind scheme is used, ( (F_left, G_left) + (F_right, G_right) ) dot (nx, ny) = ( (F_left + F_right)Nx + (G_left + G_right)Ny )/2 - |(A, B) dot (Nx, Ny)| ( U_right - U_left ) / 2 (See Hirsch's book), where U is a conserved variable and A, B are the jacobian matrices. In this case, the sign changes automatically due to the absolute operator. In case you use MUSCL-type method, you should reconstruct variables for each cell, so that it is distributed linearly.

I'm not sure that these will be helpful but provide you a little references.

A Projection Method for Incompressible Viscous Flow on Moving Quadrilateral Grids, J. Comp. Phys., 166, 191-217 (2001)

A staggered control volume scheme for unstructured triangular grids,INTERNATIONAL JOURNAL FOR NUMERICAL METHODS IN FLUIDS, VOL. 25, 697-717 (1997).

A conservative finite-volume second-order-accurate projection method on hybrid unstructured grids, J. Comp. Phys., 150, 40-75 (1999)
  Reply With Quote

Old   August 9, 2001, 23:12
Default Re: Help need on fluxes
  #5
Zhu
Guest
 
Posts: n/a
hi,thanks for your guide, for the Reo scheme,i have read through it,it is difficult to implement, compared with other simple fluxes calculation method,on other hand,what i simulate is unsteady impressible viscid flow,which need a large number of time step's results,maybe the speed of my code with 2nd order Reo scheme will restrict me.

from the simulation of impressible viscid flow around a body,i finally want to calculate the force acting on a body at each time step,there are reversed flow in the domain,i am not sure if i must use 2nd-order scheme to obtain good result,how about the frist order Reo method?any suggestion will be appreciated. thanks
  Reply With Quote

Old   August 10, 2001, 17:01
Default Re: Help need on fluxes
  #6
Kang, Seok Koo
Guest
 
Posts: n/a
It is undoubtable that higher-order method gives more accurate result. If it is possible, using higher-order accurate method is more desirable, I think.

And Roe's flux function does not need excessive computation time. It may looks complicated bu you might need just a little computation time.

Because you solve 2D inviscid flow, compuation time will not take much inspite of its unstediness.

There are plenty of choices to solve your problem : pressure-velocity coupling method, FEM, pojection method, upwind-FVM/FDM with pseudo-compressibility method, etc. Each has both advantages and disadvantages.

Please read papers and make up your mind. The choice depends on you.
  Reply With Quote

Old   August 11, 2001, 21:29
Default Re: Help need on fluxes
  #7
zhu
Guest
 
Posts: n/a
dear Kang Seok KooŁ¬thanks for you help,maybe,in the thread i posted,i didnot discribed my simulation clearly,what i deal with is viscid incompressible flow,because i am familar with projection method,so FVM will used with projection method.

the trouble come from the irregular domain,the domain is fluid flowing around irregular body,the cell will be structural quadrilateral,some arenot rectangle,now i am not sure about the follwing things: 1.for impressible flow,i think the second-order upwind scheme which is derivated from Reo scheme is enough,because i willnot meet discontinutiy,so the MUSCL or something like TVD are not necessary. 2.can fluxes extropolation(evaluetion) be used implicitly?for unsteady flow,the large time step is more appreciated. 3.for arbitry quadrilateral cell with one side having an angle of 45 degree to x-direction,i am not sure how to extropolating the flux like rho*v*fai,here,rho is the density,v is the convective velocity in y-direction,and fai is the scalar,should this fluxes be extropolated in x- or y-direction ?

thanks for your time

Zhu
  Reply With Quote

Old   August 12, 2001, 10:14
Default Re: Help need on fluxes
  #8
Kang, Seok Koo
Guest
 
Posts: n/a
For an extrapolation of variables on arbitrary grids, see the papers I commented before. Two of the papers are related to projection method. I strongly recommend you to see the paper of Kobayashi et al. (J. Comp. Phys, 150, 1999). You may be able to see detailed information on what you wonder. It is a good idea to follow the procedure described there.

If the flow is not concerned with shock, you do not need to think about Riemann solver.

There are several choices for implicit method. The most stable is first-order backward Euler method. You can also you a second-order backward differentiation. Using higher than third-order implicit method is not frequent.

Best Regards.
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
CANTERA code to get pure species mass fluxes gemmafebrer Main CFD Forum 0 October 19, 2010 11:42
Viscous fluxes in a Riemann HLLC solver Bryce Sharman Main CFD Forum 5 July 8, 2009 23:29
Fluxes of scalars at wall faces K Sanjay Phoenics 10 August 15, 2005 10:45
simple turbulence fluxes for FV dominique Main CFD Forum 1 April 22, 2004 13:29
Roe upwind fluxes!! Magesh Main CFD Forum 2 July 17, 2003 11:35


All times are GMT -4. The time now is 00:59.