[mr.adili]

Hi everybody,


I'm performing steady state FLUENT simulations for a room with mechanical ventilation.


In order to calculate the draught risk i use the Fanger's equation as described in ISO 7730 as a custom field function. The local air temperature, the local mean air velocity and the local turbulence intensity are needed for this equation to estimate the Draught.


According to the literatures for a room with mixing ventilation the turbulence intensity is around 40%. For my room with mixing ventilation i get a room averaged turbulence intensity of less than 10%.


Does anybody have experiences with similar cases? Am i doing something wong or FLUENT simply underestimates the turbulence intensity. Whats the solution in this case?


Thank you in advance und Regards
Reza

[LuckyTran]

It would help if there is a rough sketch of the domain and boundary condition types.

Originally Posted by mr.adili

According to the literatures for a room with mixing ventilation the turbulence intensity is around 40%. For my room with mixing ventilation i get a room averaged turbulence intensity of less than 10%.

This literature is probably experimental data? There's quite a difference between how turbulence intensity is estimated practically and how it is predicted numerically. Honestly I believe the 10% more than I believe the 40%. 40% turbulence intensity is a lot.

Probably, your length scales at your inlets are too low and it decays too quickly.

[mr.adili]

Hi LuckyTran,


thanks for your reply. You are absolutely right. The turbulence intensity values for room air flow in literature are based on mesaurements. By the experiments we usually measure the velocity fluctuations with an anemometer at measuring points and then extract the Tu Intensity. The question is, wether as by CFD simulations our grid is not enough fine to capture these fluctioations in a point are the Tu intensity values correct?


Regarding lenght scales, youre are right. Actually i have Tu intensity and hydraulic diameter at the inlets as boundary conditions. I used the recommended values of 5% for the Tu intensity for this reason which might be too low.

[blackmask]

According to your description, the turbulence intensity in the measurement is given by , where are the local turbulent kinetic energy and velocity magnitude, respectively. However, in fluent the turbulence intensity is given by , where is the reference velocity specified in the reference values task page. Make sure that your comparison are on the same basis.

I think that you do not have to recalculate, you can normalize the turbulent kinetic energy (or turbulence intensity) by dividing their value at the inlet and compare them with experiment result. While CFD might give reasonable flow patterns compared to experiments, personally I am suspicious that CFD should give reliable results for specific location.

[mr.adili]

Hi blackmask,


thanks. Thats really interesting.

[LuckyTran]

Originally Posted by blackmask

According to your description, the turbulence intensity in the measurement is given by , where are the local turbulent kinetic energy and velocity magnitude, respectively. However, in fluent the turbulence intensity is given by , where is the reference velocity specified in the reference values task page. Make sure that your comparison are on the same basis.

That is how Star-CCM does it, I am not aware that Fluent does it this way. Reference values should never be used in any Fluent calculation. If it does, then it is a bug and should be reported and fixed. Fluent should use the local mean flow velocity (or just velocity since we are talking RANS).


If in doubt, then directly specify k and epsilon or k and omega instead of intensity & length scale.


The 5% and hydraulic diameter is for fully developed duct flows. The 5% is the TI at the center of the duct (it's much higher near the wall). In ventilation ducts there are often turns and fans where the length scale is much larger. That's why I ask what your domain looks like.



In CFD you model the transport of k which is like modeling what the turbulence intensity looks like. You do need the right grid to capture shear layers and what not that would influence the production term in k. Absent of any of these flow structures that would generate any turbulence, I wouldn't expect to see anything above 5% turbulence intensity (because you specified 5% at the inlet). When these flow structures are present, the turbulence in the domain is less sensitive to inlet boundary conditions. So I am not sure that the inlet BC's are even the problem.



If you measure at specific points, I would compare it also to TI at the same location in CFD. It doesn't make sense to compare a pointwise measurement of TI (with an anemometer in the shear layer perhaps) to a room average. For example the turbulence intensity near the walls of a duct easily reaches levels of 20-50%, but it's only 5% in the core of the duct. And if you were to average it over the cross-section, well you'd get a number like 7-10%. I say this because I have no idea where the anemometer was placed. Maybe the anemometer was put in the center of the room and is measuring the quiet part (but that suggests the turbulence intensity somewhere else might have been 1000%).

[blackmask]

Originally Posted by LuckyTran

If you measure at specific points, I would compare it also to TI at the same location in CFD. It doesn't make sense to compare a pointwise measurement of TI (with an anemometer in the shear layer perhaps) to a room average. For example the turbulence intensity near the walls of a duct easily reaches levels of 20-50%, but it's only 5% in the core of the duct. And if you were to average it over the cross-section, well you'd get a number like 7-10%. I say this because I have no idea where the anemometer was placed. Maybe the anemometer was put in the center of the room and is measuring the quiet part (but that suggests the turbulence intensity somewhere else might have been 1000%).

You are absolutely right that the comparison should be based on the data extracted in the same manner from experiments and CFD. However I am suspicious that the point-to-point comparison should work. For example, say the dominant flow structure is a recirculation zone and the CFD under-predict the dimension a bit, then the point-to-point comparison could be a disaster if the probe is placed near the edge of the recirculation zone. However, if the comparison is based on the relative position of the recirculation zone, it would be much more satisfying. I just do not have much faith in a single point data. If would be much better is there is an array of probes placed in line (or in other regular manner), and the comparison is also done line-to-line rather than point-to-point.

[mr.adili]

I have attached a picture of my domain. I hope you can see it. Just the room has been modeled. It means air is entering and leaving the romm through simple openings as surfaces. The velocity profile is normal to the inlets and uniformly distributed over the surface. The dusitng and fans up/downstream the inlets are not considered.