Learning Forum

[Benjamin Walz]

Hi,

 

I have a problem with the convergence of my simulation. It takes about 15.000 Iterations for the mass- and heatbalance to add up.

The case models airflow inside a room. The air enters through the velocity inlet with a temperature of 55 °C and 0.4 m/s and leaves the room through the pressure outlet. One of the walls contains a heat sink so that mean air temperature in the room results in ~20°C. The mesh has 4.5 mio cells.

I am using the pressure-based solver. For air properties that are temperatur dependent I use a polynoma (named expression).

How can I accelerate the convergence?

Every help is greatly appreciated. Cheers.

[NickFL]

To what end? You seem to have a solution (or are coming close to one) already.

1. Use a better initial condition. What did you use as your IC for this run? Using a previous solution with minor changes in boundary conditions or small geometric changes will tend to converge faster.
2. If you are simply trying to drive the residuals lower, try moving to the coupled solver. Once you have a semi-converged solution transitioning to the coupled solver may help drive residuals down faster. The down side here is the time per iteration will be longer, but the number of iterations necessary to get to the same level of convergence is often less.
3. There is always the choice to increase the relaxation factors. The down side here is if you increase them too much the solution can diverge on you. The support here will probably tell you to avoid this one.

The number of iterations is not important. What we typically care about is the wall-clock time. Are you running in parallel and matching the number of cores to the processes used by Fluent?

 

[Rob]

You may also want to review the solution, and especially the velocity field. Buoyant flows are rarely steady state, so text book convergence may take a while, or may not occur. 

[Benjamin Walz]

Thank you both for your answers.

 

I want to accelerate the convergence because I want to simulate different geometrical variations with similar boundary conditions. The time consumption with this setup is very high.

1. For this run I patched the temperature for the room air zone to 20°C and the air in the inlettube to 55°C. I will try to patch previous solutions to the new cases.
2. I am using the coupled-solver. At first I tried using SIMPLE, but it didnt converged at all. The residuals for the continuity-equation are not going down (~0.1), I guess this is due to the turbulent nature of parts of the flow. Thats why I track my mass-balance instead to check convergence.
3. I am running in parallel-mode. Average wall clock-time per iteration is 9.5 s. What do you mean matching the number of processes used by Fluent? Currently I am using as many cores as possible.

@Rob: Yes i noticed that buoyancy in my solution is not accurate in the velocity field. Do you think t´a Steady-State simulation is the wrong approach?

 

[Rob]

I tend to run these steady but also use monitor points rather than residuals to judge convergence. I'd also review whether you need to include the entire inlet/outlet pipe. However, I'd expect things to settle down within 2-4k iterations unless the initial condition was really poor. What are you using for the gas density? 

By cores, are you using all of the cores on a single cpu? How many cores are you using?

[Benjamin Walz]

Thank you again for answering.

I need to include the pipes because I am "calibrating" the model with measurements in a lab.

For the density (and thermal conductivity and viscosity) I am using a polynoma (5th degree) in dependance of the StaticTemperature integrated via an expression.

 

I am using 30 out of 32 cores on my machine.

[Rob]

Ah. Can you plot the polynomials using the exact values in Fluent? Use the plot function in Fluent in the materials panel. 

 

[Benjamin Walz]

I created my own Polynoma fitting literature data:

I use this as a "named expression".

[NickFL]

I look at that data and I think a 6th order polynomial is a bit of an overkill. How many data points did you use to fit the data?  Have you tried to simplfiy it? It won't speed up the computation much, but it can't hurt. Also, is there a reason you are not using the built-in polynomial fit in the materials tab?

[Rob]

OK. I'm always very wary when seeing coefficients like that: how confident are you that Excel is accurate to give a sensible answer to 2.8e-12 x T^6? 

[Benjamin Walz]

I see your point.

I used around 60 datapoints (between 273 K and 333 K). I tried a 4th order polynomial but the accuracy of the material properties gets worse.

As far as I know Matlab is calculating 16 digits accuratly. The accuracy of the fit is very good compared to the datapoints.

I started a new run with the built-in polynomials material panel and slightly improved inicial conditions. Lets see if the convergence has improved.

[Rob]

Matlab might, as will Fluent. But.... Four significant figures at e-12 with something raised to the power 6 is potentially going to give some interesting results. I've seen a few "smooth" polynomials like that which looked more like a saw than a curve.