[AnhDL]

Hi experts,
Hi experts,

I am simulating an airflow through an object as in the picture. The simulation conditions are Re = 4.3e+5, Uin = 7m/s, Pout = 1atm. The boundary condition for turbulent quantities is turbulent intensity = 0.3 (based on Re) and turbulent length scale l =0.2 (based on the size of the object).
The simulation with the central object is okay with very good agreement with reference data. And the turbulent viscous ratio reached up to 3e+04.
However, in the simulation with additional objects on the left and right, I got a message from the solve "turbulent viscosity limited to viscosity ratio of 1.000000e+05".
I tried to increase the limiter to 2.00000e+05, but the message still appears.
Then, I increased the limiter to 5.00000e+05, the message disappeared and the tendency of the unsteady force on the object was similar to that with the result at 2.0000e+05
I did the transient simulation, and the above message appears and disappears periodically during the simulation.

Now I am trying to compare the solution with increasing the limiter to that with the default limiter value.
I wonder if the limiter will affect the physical results, Can someone help me, thank you?

[LuckyTran]

The limiter is set to unphysically, impossibly high values for the viscosity ratio. If the region where the limiter is being violated is on the dark side of the moon then it would obviously not impact the result and there is no harm to raise it for the sake of turning off the alarm. However, if the limiter is being exceeding in the region of study then all the CFD results are likely garbage.


Fix the warning, don't fix the limiter. You should never have that high of a viscosity ratio in the first place. It is equivalent to asking if it is okay to raise the maximum temperature to 1 million Kelvin.

[AnhDL]

Originally Posted by LuckyTran

The limiter is set to unphysically, impossibly high values for the viscosity ratio. If the region where the limiter is being violated is on the dark side of the moon then it would obviously not impact the result and there is no harm to raise it for the sake of turning off the alarm. However, if the limiter is being exceeding in the region of study then all the CFD results are likely garbage.


Fix the warning, don't fix the limiter. You should never have that high of a viscosity ratio in the first place. It is equivalent to asking if it is okay to raise the maximum temperature to 1 million Kelvin.

Thank you, LuckyTran,

A paper by Richards and Hoxey "Appropriate boundary conditions for computational wind engineering models using the k-E turbulence model" implied that the turbulent viscous ratio can be reached to 2.0000e+05 which is over the Fluent limiter. Also, this web http://www.eureka.im/77.html says that TVR can be up to 1e+8 or 1e+9.

Someone mentioned that the poor mesh quality may be a problem. But in my case, the high TVR occurred at the region with structured mesh. Thus, I think the quality of the mesh is good since there was no problem with the result in the case with only a square object. So, any solution to this problem?

In this simulation, I only one to get the force on the object where the TVR is smaller than the default limiter 1.000e+05. The excessive TVR occurred in the downstream region of the object. So, you mean the result is there for acceptable?

[LuckyTran]

I completely disagree that your mesh is good. Your mesh is far from perfect, there are many skewed cells.

You most likely have too high inlet turbulence intensity and too high a length scale. 30% is a ridiculous amount and not seen in any engineering device. The inlet turbulence intensity and length scale are not decided by any details in your domain. These depend on the properties of the flow upstream before your inlet.


Nonetheless I don't think any of these will impact your results. Turbulence does very little in scenarios where you can get 99% of the answer from a simple back of the napkin calculation. For example you can just as easily set the inlet BCs to anything else and still get the same results.

[AnhDL]

LuckyTran,

My mistake. Turbulent intensity at inlet was set 3% based on Re. Actually, the unstructured mesh was generated close to the object because the object will moved or rotated. So skewness cells exist. However, the high TVR occurs on the structured region far away the object, where I think the mesh is good.

[LuckyTran]

If 3% is your inlet turbulence intensity then it makes even less sense how you get more turbulence viscosity than anyone has ever measured before. If you truly believe this result to be correct, go measure it! You will be a Guinness World Record holder! Take some kid's lego blocks and put a fan in front of it, you'll be blown away one way or another

[CFDKareem]

Originally Posted by AnhDL

Thank you, LuckyTran,

A paper by Richards and Hoxey "Appropriate boundary conditions for computational wind engineering models using the k-E turbulence model" implied that the turbulent viscous ratio can be reached to 2.0000e+05 which is over the Fluent limiter. Also, this web http://www.eureka.im/77.html says that TVR can be up to 1e+8 or 1e+9.

Someone mentioned that the poor mesh quality may be a problem. But in my case, the high TVR occurred at the region with structured mesh. Thus, I think the quality of the mesh is good since there was no problem with the result in the case with only a square object. So, any solution to this problem?

In this simulation, I only one to get the force on the object where the TVR is smaller than the default limiter 1.000e+05. The excessive TVR occurred in the downstream region of the object. So, you mean the result is there for acceptable?

I'd have to agree with Lucky that the TVR seems very suspicious. Even in the link you provided they said the TVR can get up to e8-e9, but in atmospheric boundary layers, an incredibly large length scale and high energy planetary system. With only 7m/s of airflow at the inlet and the high IVR happening in the freestream, something does not add up.

[AnhDL]

Originally Posted by CFDKareem

I'd have to agree with Lucky that the TVR seems very suspicious. Even in the link you provided they said the TVR can get up to e8-e9, but in atmospheric boundary layers, an incredibly large length scale and high energy planetary system. With only 7m/s of airflow at the inlet and the high IVR happening in the freestream, something does not add up.

Hi, the square object is rotated with speed up to 23 rad/s (225 rpm). This rotation flow interacted with the flow pass the left and right rectangular objects, will this increase the turbulent quantities at the wake?

[AnhDL]

Originally Posted by LuckyTran

If 3% is your inlet turbulence intensity then it makes even less sense how you get more turbulence viscosity than anyone has ever measured before. If you truly believe this result to be correct, go measure it! You will be a Guinness World Record holder! Take some kid's lego blocks and put a fan in front of it, you'll be blown away one way or another

Thank you, now I am trying to do simulation with more refinement mesh behind the object where the high TVR occur to check. I forgot to mention in the question that the square object is rotated with speed up to 225 rpm using sliding mesh. Is this the reason for a high TVR?