[FCKW36]

Thank you for your answer. this is my first CFD Analysis, that's why I have so many questions...

I did a finer mesh now, as you can see in the Picture below. I have now 7 prism layers, first layer has a thinkness of 0.13 mm with a growth factor of 1.2. The target cell size of the tetrahedral mesh is now 1 mm with a max size of 6 mm and a grow rate of 1.1.

I used free slip wall for the closure (the Body which is restrictimg the flow system) because it's not there in reality and I don't want it to affect the simulation. The Support strut itsself is a real Body. That's why I defined it as no slip wall. See at the Picture "system boundarys" what I mean.

So you mean using RANS leads to the small Variation of total pressure in front of my Body and this is a normal effect?

I reached a convergence solution, residual target is 1x10^-6.

You can see the total pressure plot with the finer mesh. The jagged and abrupt transitions are not that present anymore. What do you think?

[FMDenaro]

Originally Posted by FCKW36

Thank you for your answer. this is my first CFD Analysis, that's why I have so many questions...

I did a finer mesh now, as you can see in the Picture below. I have now 7 prism layers, first layer has a thinkness of 0.13 mm with a growth factor of 1.2. The target cell size of the tetrahedral mesh is now 1 mm with a max size of 6 mm and a grow rate of 1.1.

I used free slip wall for the closure (the Body which is restrictimg the flow system) because it's not there in reality and I don't want it to affect the simulation. The Support strut itsself is a real Body. That's why I defined it as no slip wall. See at the Picture "system boundarys" what I mean.

So you mean using RANS leads to the small Variation of total pressure in front of my Body and this is a normal effect?

I reached a convergence solution, residual target is 1x10^-6.

You can see the total pressure plot with the finer mesh. The jagged and abrupt transitions are not that present anymore. What do you think?

Ok, the "wall" is just the top and bottom of the domain, yes you can let the flow be tangent to it.
However, a RANS solution produces a smooth solution as it represents a statistically averaged field. From your plot the field seems not so regular. What is more is the fact you must have a (statistically) steady solution and the flow is specular if you do a cut along the half-body. Conversely, that seems not appearing in your solution...

[FCKW36]

Hi,

I think I know, what you mean. But I tested my Simulation with different turbulence models and different meshes. I always get results which are looking nearly, if not exactly the same.

When I Google for Pictures, i find the same thing, where the flow is not specular on both sides of the Body. For example:

https://www.google.de/search?biw=192...=1560352826023

What could be the reason? Numerical error? Is it a big problem? From what I can say, the results are looking at least reasonable. Is the thickness of the first prism layer to thin or to thick with 0.13 mm?

[FMDenaro]

Originally Posted by FCKW36

Hi,

I think I know, what you mean. But I tested my Simulation with different turbulence models and different meshes. I always get results which are looking nearly, if not exactly the same.

When I Google for Pictures, i find the same thing, where the flow is not specular on both sides of the Body. For example:

https://www.google.de/search?biw=192...=1560352826023

What could be the reason? Numerical error? Is it a big problem? From what I can say, the results are looking at least reasonable. Is the thickness of the first prism layer to thin or to thick with 0.13 mm?

Two possible issues: 1) the grid is not exactly specular and introduces difference in the errors 2) false convergence in the solution, it could require a smaller threshold for the stopping criteria.


If the physical geometry is perfectly specular, if the BCs. are specular, the steady RANS solution must be specular. Ideed, in such cases people perform the simulation on half-body to reduce the computational cost.

[FCKW36]

Originally Posted by FMDenaro

Two possible issues: 1) the grid is not exactly specular and introduces difference in the errors 2) false convergence in the solution, it could require a smaller threshold for the stopping criteria.


If the physical geometry is perfectly specular, if the BCs. are specular, the steady RANS solution must be specular. Ideed, in such cases people perform the simulation on half-body to reduce the computational cost.

When I plot the static pressure, it looks perfectly specular, the difference can only be seen in the plot of total pressure. I attached a picture below.

1) When I look at the grid it doesn't look specular to me. So this could be a reason in my opinion.

2) What do you mean? How can i check/change this?

Best regards

[FMDenaro]

Originally Posted by FCKW36

When I plot the static pressure, it looks perfectly specular, the difference can only be seen in the plot of total pressure. I attached a picture below.

1) When I look at the grid it doesn't look specular to me. So this could be a reason in my opinion.

2) What do you mean? How can i check/change this?

Best regards

- Clearly you should check the dynamic pressure.
- Try to decrease the values for convergence in the mass, momentum and energy equations by a factor of 10^-2. Are you also working using double precision?

[FCKW36]

Thank you very much for your answer, I will try this out.

What do you think about the thickness of my first prism layer with a thickness of 0,13 mm?

[FMDenaro]

Originally Posted by FCKW36

Thank you very much for your answer, I will try this out.

What do you think about the thickness of my first prism layer with a thickness of 0,13 mm?

If you want to get such a fine resolution to describe the boundary layer, the dimension in mm does not say clearly what is your grid resolution.
Compute the distance from the body in terms of the y+ function