Steady Fluid Flow: Load Stepping

[Anonymous]

Hello,

I am running a steady fluid flow simulation with water running through a coldplate tube (I'll later couple this with a steady-state heat transfer simulation). I have flow entering one end of the tube with a velocity of 2.5 m/s and an outlet condition at the other end of the tube. The simulation runs without any errors however I get one warning; Warning: Converge with stagnation due to oscillation. The pressure distribution/drop look quite reasonable compared to actual results. I suspect the warning I am receiving is a result poor load-stepping parameters (I am using the default parameters with one load step).

I have attached the simulation report; it would be great if someone could suggest how to achieve a better suited Load-Step. Perhaps I shouldn’t be concerned about the warning?

Thanks,

Ian

[hupn]

Hi,

The warning could mean that oscillation pattern is detected in the fluid flow solver. This could the fact for some real simulation problems, e.g. vortex shedding. You may want to refine the mesh, also make sure that the turbulence model is on for turbulence problem.

hup

[Joey.X]

For Warning message: Converge with stagnation due to oscillation, check the reply in this previous thread

http://forums.autodesk.com/t5/Autodesk-Simulation/steady-state-flow/m-p/2763048#M532

or search the whole string "Converge with stagnation due to oscillation" in this forum for more posts and replies.

[Anonymous]

Thanks Hup/Joey. By turning turbulence ON, the warning about convergence stagnation went away. Now I have a new problem though - the resulting overall pressure drop is about 10 times higher than experimental results. I have LES turbulence model selected with the default model constraints. Any ideas?

In a previous post you (Joey) said, "(b) Check if "turbulence" is check on in Analysis parameters/local curve/Turbulence if the flow is turbulence flow (user needs to manually check the ranger of Reynolds number). Without checking on turbulence is a common mistake for simulation convergence issue."

I am wondering how to check the range of the Reynolds number (the flow is turbulent, Re~14,000).? I didn't see a field in the Analysis Parameters to enter such a quantity.

Thanks,

Ian

[Joey.X]

The verification of simulation result with experimental data is probably tricky and needs good experience depending on the nature of problem.

- How much error on your experimental data?  How did you measure the fluid pressure?

- How did you measure the pressure drop from simulation? The pressure is usually not constant in cut section, and even changes a lot.

- Mesh density and boundary layer mesh

Back to simulation side, if the flow is laminar flow, the result should be accurate enough if user sets reasonable boundary conditions. 

However, if the flow is turbulence, a couple of factors will have major impact to result accuracy, refer the details in software help.

-   Type of turbulence models

     k-epsilon model is more accurate but depends more on boundary layer mesh, model settings, and more computational expensive.

-   Boundary layer mesh (mesh density and accuracy)

     To pursue better result accuracy, mesh dependency study is needed

-   Modeling boundary conditions

    One important tip is avoiding  set pressure BC or ioBC close to the location having large pressure change)

-   Measurement of the pressure drop

Yes, user needs to check if the flow is laminar or turbulence then then turn on/off turbulence model in model settings. Put it simple here,

(a) for internal flow, the critical Reynolds number is 3200~4000

(b) for external flow, the critical Reynolds number is 5e5

Note that the reference length used in calculating Reynolds number is conceptly different in above two cases.

[Anonymous]

Thanks for the tips Joey.

The experimental results that I was referring to actually come from the manufacturers spec, therefore i cannot comment on its accuracy but i would expect it to be reasonable. The goal of my steady fluid-flow simulation is not to make a one-for-one comparison to the manufacturers specs, its more a matter of making sure i haven't missed anything by ensuring pressure results are somewhat comparable i.e. +/- 50% (i'll later be using the results from the fluid flow in a steady-state thermal simulation).

By improving the quality of the boudry layer mesh i was able to obtain a pressure drop of about 20 PSI, an improvement from ~30 PSI from using default mesh size (the manufacturers spec is 4PSI at 2 gal/min). The pressure distribution of a cross section is very consistent throughout with a variation of not more than one-thousandth of a PSI. The flow IS turbulent and i'm still using the LES model. The k-epison model is more accurate but could it account for this large variation? It seems like I might be missing something. Any suggestions?

Thanks in advance,

Ian

P.s. in the meantime i'll play around with the K-epsilon solver.

[Joey.X]

Ian, thanks for providing the reference data to diagnose the accurancy issue.

Here are more items for you to check

a) Perform mesh study to see the result's sensitivity on mesh density, you may ty multiple mesh densities.

b) Depending on your problem's nature, if the total pressure drop majorly from the pressure drop(through non-streamline like objects such as valve) or friction contribution, for later case, the turbulence model and boundary layer mesh (check y+ and refer to the turbulence model document) makes big difference. For example of the flow through an airfoil which has a good streamline profile,  the LES turbulence model may have relatively larger error in predict total pressure drop and drag force on the airfoil.

c)  Check your Reynold number in this problem, if it is close to the cretical value, the flow is in transient area, neither  of the laminar model and turbulence model can predict it accurantly.