Hi. Since my calculations (a simple adiabatic steady state air flow) have great problems of convergence with SIMPLE, I'm going to try with PISO algorithm. Anybody can tell me something about the use of it in steady state? One problem I have, for example, is that when I try to set the values in the window of solution method ,the "Maximum Number of corrector Stages" is fixed to a value very near to zero; is it normal? Why?

Thanks for your answers.Andrea.

If it's a simple air flow simulation, STAR should not encounter convergence problem. Maybe you can provide a bit more detail? As for the PISO scheme, the default max. no. of corrector stages is 20.

I'm studying a flow of air in the pipe that leads to a close coupled converter of a car; the geometry of this pipe is a little bit complex(it has an elbow, the section varies, and it hasn't symmetry planes),but not so much.I 've used PROAM to mesh the CAD, so there are some trimmed cell. I' ve used the porous model for the converter, and inlet-pressure as boundaries; I've already tried to lower underrelaxation factors, but the residuals remain on values of 10e-1,10e-2.I don't really know what else to do, and I don' think the mesh is too coarse. If you have some ideas....

Thank you a lot. Andrea PS: Other informations on PISO for steady state?

Thank you again.

It is a little bug for the wrong number of correcter stage of PISO. It only happened in the windows version. YOu can define it typing. Furhter, for the unconvergence of your problem. It might be the mesh qulity is too poor. You can get convergence with further low under-relaxtion factor, especially for the pressure in SIMPLE. For the PISO, it might take longer time to get convergence than SIMPLE. You must define carefully the location of reference pressure in PISO when you have the pressure boundary involved. Otherwise, it might divergence.

Reference pressure isn't of any real consequence for incompressible calculations, PISO or SIMPLE. Setting a 'wrong' value of pressure certainly shouldn't cause the solution to diverge.

If you have a pressure boundary in the solution then the pressure field is tied down to that and the reference pressure only influences post processing.

I don't think PISO is ever a good alternative to simple for steady state calculations. It is usually slower to converge and takes much longer per timestep. I think you'd be much better concentrating on finding out WHY the original solution didn't work and sticking with SIMPLE.

B.

Hallo Andrea!

Having a poor convercency, I wouldn't use piso. May be you can check following points:

1. Do you have recirculation at the pressure boundary? If so, you should extend your calculation domain.

2. What's the magnitude of the ALPHA and BETA values of the porous media? The difference between the biggest and smallest value shouldn't be more then 3 orders of magnitude.

3. Try reducing the value of the maximum residuum for the pressure equation.

Thank you for your help; I just can't understand what do you mean with "reducing the value of the maximum residuum for the pressure equation".About the other suggestions,I've reduced today the maximum values of alfa and beta, but nothing has changed with residuals.What is strange in my calculation is that, with high values for TE and ED underrelaxation factors(0.6),TE and ED residuals fall down, but there is no way to make go down u,v,w,p res.,both with small and high underrelaxation factors. If you've got other ideas.. Thank you a lot again.Andrea.

Thank you a lot for you answer.I've tried with PISO but residuals are always the same;I've passed back to SIMPLE modifying the values of underrelaxation factors hoping that this experimental method (monitoring step by step their influence on calculation and restarting it with new values when it doesn't go well)will take me to a convergence.Thanks again.Andrea.

Andrea,

If your residuals converge only partly but your monitoring values are essentially steady or periodic with a steady mean, you may in reality have a transient flow that you are trying to solve using steady state methods. Check you monitoring values carefully if you haven't already done so. Another option is to take post dumpings from different iterations and compare the solutions. If you for instance have diffuser-like area expansions, this is a place to look for unsteadyness. The ultimate check is to restart from your "steady" solution and perform a transient run. This will for sure reveal if the problem is unsteady flow.

If the problem lies in the mesh quality you could use cran,news,pran... to collect cells with spurious solution values in a cell set and look for bad cells in that set. Enabling the error estimation option gives you the opportunity to study the error estimate directly in this way. You might of course also want to check the mesh directly for bad cells using the available tools for this if you haven't already done so.

Good luck!

Lars Ola

Hallo Lars! If you don't mind, I would like to make you a pair of questions, since you seem to know a lot of things more than I know:1)how is it possible that the flow I study remains transient forever, if the boundaries are costant in time?: there will be a time in wich the values in each cell become costant after the transient, or I'm wrong?2)You talk about error estimation:I've already tried to use the tool to do this in the StarGuide but I couldn't:can you teach me how to do? Thank you for your previous help;sorry for my repeared questions, but I've got to take my degree in a month and I have still a lot of problems. Thank you again,Andrea.

Andrea,

Just like laminar flow becomes unsteady and results in turbulent fluid motion, flows can be unstable on a "macro" level too. One very frequently quoted example is the vortex shedding behind a cylinder in a cross flow. This is an unsteady, but nevertheless nicely periodic flow where the boundary conditions are steady. Another example might be a diffuser. If it has a too large opening angle, the flow will separate due to the strong adverse pressure gradient. If the opening angle is very large (or if you have a sudden expansion) you may have a steady jet flow, but if the angle is smaller, the flow may still attach to one of the sides of the diffuser. This doesn't have to be a steady situation, however. The flow may repeatedly detach from one side and reattach on the other, and this phenomenon can even be chaotic without a distinguishable periodicity. Even a seamingly steady flow may have sligh oscillations in real life, and I suppose the randomness of the turbulence is to blame in that instance. Anyhow, the thing is that if you have area expansions or sharp turns that might provoke separation, there is reason to consider this possibility if you see your CFD solution converge only partly. And as I said in my previous post, steady or oscillating monitoring values (about a steady mean) are in such a situation a strong indicator that the steady state assumption does not hold in spite of steady BC's.

You only need to toggle on the error estimation in the StarGUIde (analysis controls/output controls/monitor numeric behaviour) in order to make STAR dump the error estimates to the file casename.err. This file has the structure of a transient post file, so you'll have to open it like you would open a casename.pstt file. Then, loading in velocity will give you the velocity error in m/s and so on. You might want to normalise these values somehow. In that case you should study the opportunities offered by the operate command, which is a very nice feature in my personal opinion.

Best whishes,

Lars Ola

Hallo Andrea,

my suggestion was to reduce the residual tolerance, mainly for the pressure equation.

You can do this with the comand

resi 0.05 0.05 0.05 0.01 (defaults: 0.1 0.1 0.1 0.05)

or in the panel:

Analysis Controls->Sol. Controls -> Eq. Behavior -> Primary Variables.

May be you need to encrease the number of (pressure) sweeps, but usually not.

This could help to reach a lower value of the final resuduals also in the case your're computing a kind of average solution of a flow which in reality is transient (s. Lars's message).

The real improvement in the solution is not big. If you've the kind of problem cited by Lars, you should check the convergence monitoring the macroscopic values you're interested in (for example mass flows or averadge pressure at given sections).

It's up to you to judge if the neglected transient effects are relevant for your problem.

Marco