[Manideep304]

Hi all, I have a question regarding XiFoam solver in Combustion. I am using XiFoam for conducting an experiment. I have seen some pdfs regarding XiFoam solver. Though the velocity is initially 0, the turbulent kinetic energy is 1.5 and turbulent KE dissipation rate is 375 as initial conditions. I would like to know how these values are calculated as I understand that if velocity is 0, the kinetic energy and dissipation rate should be 0.
And my 2nd question is I have given noSlip condition near the walls for velocity and fixed value for temperature. As i can observe in paraview that on the walls, the temp. is showing fixed value,but the velocity seems to variate though I have given noSlip condition on the walls. I do not understand that. If anyone could help me with this, i would really appreciate it and thank you in advance

[Gerry Kan]

Dear Manideep:

The inlet values for TKE and epsilon are usually estimates based on turbulent intensity and turbulent length scale.

Turbulent intensity is simply the ratio between the magnitude of turbulent fluctuation and some representative mean velocity. If you assume 10% intensity (fairly standard) over, say, a mean flow of 1 m/s, this will work out to (3/2)(0.1^2) = 0.015 (m/s)^2.

The turbulent length scale depends on the flow geometry. This usually represents the largest turbulent eddy the flow domain can accommodate. As a rule of thumb, the turbulent length scale should be half of the largest dimension. In pipe flows, for example, it would be the radius.

Once you know k (from turbulent intensity) and the length scale, you can calculate epsilon using the relation:

[turb length scale] = [C mu] [k^3/2] / [epsilon]

In most engineering relevant flows, the final flow field and reaction rate will be fairly insensitive to the inlet turbulent settings, as long as they are reasonable.

To your second question. Paraview plots your cell center velocity values, which are not zero.

Hope that helps, Gerry.

[Manideep304]

Hello Gerry. Thank you for your reply. It is really helpful information though i have a few questions.

1. How can I give the input of turbulent intensity and turbulent length scale values (radius of pipe) to my simulation.

2. As paraview plots cell centre values, shouldn't my temperature also not be constant. My temperature is observed to be constant where as the velocity seems to be fluctuating for the same cell size.

Would really appreciate it if you could share your ideas. Thank you in advance.

[Gerry Kan]

Originally Posted by Manideep304

1. How can I give the input of turbulent intensity and turbulent length scale values (radius of pipe) to my simulation.

2. As paraview plots cell centre values, shouldn't my temperature also not be constant. My temperature is observed to be constant where as the velocity seems to be fluctuating for the same cell size.

Hello Manideep:

To answer your questions quickly:

1) In OpenFOAM, you will need to calculate the inlet TKE and epsilson based on the corresponding turbulent intensity and length scale. The calculation is relatively straightforward. I am sure there are other more clever ways of incorporating these quantities directly, but I suspect all involve some kind of code change.

2) It is probably because temperature is relatively slow changing. If it is important to show the no-slip, you can also load the boundary along with the domain your boundaries will appear correctly.

Sincerely, Gerry.