Hi all, I am developing a finite volume code for solving non-isothermal and non-Newtonian fluid(GNF)flow. Under the Newtonian case, i found this code can give a pretty good convergence based on SIMPLE coupling algorithm. However, for the highly nonlinear case such as n<0.1 for power law, the convergence was slowed down considerably, indicating the poor coupling ability of SIMPLE. Any cure for this ? Maybe i should use multigrid ? or try other coupling schemes (PISO, SIMPLEC..)? Hope the experienced one can give me the suggestions. Thanks in advance

i know the CMOLD software for simulating flows of thermoplastics which are definitely non newtonian uses a pressure based method. i don't know which one though. perhaps you can contact them and ask. that might help you

What kind of grid and geometry are you using? 2D or 3D? CMOLD only has 2.5D product for non-Newtonian polymer.

CMOLD is a generalized hele-shaw approach, that is ,only a pressure possion equation is sovled. My problems was encountered during solving primitive variables Navier Stokes equation by FVM(or more correctly by SIMPLE) on either 2D or 3D grid in the simulation of highly nonlinear GNF flow.

(1). Looks like that "SIMPLE" is not always very simple. (2). If what you are doing is somethin new, that is, you are not following any published paper or approach, then you are on you own. (3). Convergence rate depends on many parameters, so, it is not easy to pin point the source of the slow convergence rate. (4). Since you are satisfied with your Newtonian model, I would suggest that, you focus on the effect of the Non-Newtonian model effect first. That is, first simply the problem and then try to identify the sources affecting the convergence rate. (5). So, you are free to use any available methods to speed up the convergence of your Non-Newtonian model. At the same time, you can try to do journal paper search to see whether you can find the similar cases. It is always helpful to mention the paper or the article you are following, so that the reader can dig it up if it is easily available.

Hi.

I have been doing computer simulation of Non-Newtonian fluid flow. It is good to know that somebody is doing similar thing like what I do. Actually, I am using FEM instead.

You problem is very well known in Non-Newtonian flow simulation and it also has been bothering me a lot.

Basically, there is no sophicated cure for that. However, there are some laborous ways that I found from literature survey and also from trial and error.

(1) use increment techniques start with Newtonian case or Non-Newtian case(n>0.6) and gradually decrease power index down to number you want.

(2) use Picard type solver Due to strong nonlinearity in viscous flux as n is close to zero, your initial condition(starting point) is very reasonable to get solutions. However, it is not that easy as you know. Therefore, at first of a few iterations(about 10) you need to move your intermediate solutions sufficiently close to real solutions using Picard type method which is less efficient but has larger radius of convergence. And then, switch to standard linear matrix solver imbedded in SIMPLE (I think it is TDMA). It is strongly true for my case in which I use Newton-Raphson method for non-linear FEM equations and then use GMRES matrix solver.

(3) use relaxation factor I think SIMPLE uses some level of relaxation factor during iteration. You may need stronger relaxation like 0.2 if you move your power index close to 0.

Unfortunately none of the methods above does not promise guarantee convergence.

In FEM case Non-Newton fluid flow simluations started in early 80's with power law fluid model, but there was not satisfactory improvement for lower power index case. It is very difficult to get solutions when n < 0.2, people usually do when n > 0.25. In my cases, I usually do when n > 0.4 because below 0.4 I still have convergence problem.

JK.

Hi, JK

I am a beginner for CFD. I am trying to write some codes for steady incompressible N-S equations. I tried many ways to solve the following simplest example: given a cavity, 2 sides are wall (u=v=0), 2 sides are provided by pressure p0 and p. And also Newtonian fluid is assumed, convective term is omitted.

All the standard algorithm: FDM, CVM, FEM will give singularity concerning continuity equation.

Delta . v = 0

I just want to know what tricks have you made when you developed your FEM code. Do you use SUPG and PSPG FEM algorithm? Or add bubble function for velocity?

I appreciate your response.

yangang bao

Hi..

If you do that, there will be indeterminecy in your incompressibility contraint. If you assign pressure, you need to assign velocity(any type, zero or non-zero). I am not quite sure about your configuration. It sounds like a lid driven cavity. If it is, I think you just need to put one contant pressure value at one of corner nodes in the cavity. For incompressible flow pressure is only appeared as gradient term like dp/dx, any value is possible.

I am using SUPG and also pressure Poisson equation.

JK