[MrCaplin]

Hi,

it's been a while since I posted a thread about a meshing issue:
http://www.cfd-online.com/Forums/ans...ted-plate.html

I really need some advice as time is passing by and there's no one around me who could help me in any way. So I'd really appreciate any help and/or tipps!
I will try to keep it short.

First of all, this is not for commercial purposes or an in depth analysis and thus does not demand the "highest precision" (there are several issues; hardware limitations, no). The general idea is to get an overall picture of the internal flows inside our geometry(/-ies).


The problem:

An internal gas flow
The geometry is basically a tube with 6 inlets and one outlet.
The tube also contains a mixing volume and several perforations.


There are 3 modifications/models (pictures below):
1: A perforated plate
2: A normal plate forcing the airstream to the side
3: An "open" tube



Current settings:
FLUENT 14.0

I did not succeed in getting a structured mesh/or a steady state solution.
So I opted for a completely unstructured mesh. Note that the geometry involving the perforated plate was meshed without an inflation layer as this was not possible due to hardware limitations (without inflation I get aroung 9e6 cells). FWIW the PC I'm working with has only 8 gb of RAM.

Steady-state; I know that this problem "screams" transient (based on my understanding) since it has a turbulent mixing zone and several recirculation zones but as I said the goal is to get an idea of the general flow behaviour.

Incompressible; First results yielded a max velocity of about 105 m/s which puts me around a Mach number of 0.3. From what I learned this is the compr./incompr. threshold. Since those velocities are only measured in rather "small" zones and to save computational time I opted for incompr.

Turbulence: Realizable k-e; Turbulences/recirculations not necessarily wall bounded/easier to converge

Boundary conditions:
Inlets: Mass flow
Outlet: Pressure Outlet
Turbulence: Hydraulic diameter + Intensity

If you need more information, please let me know!

First results:

Convergene criteria:
1. I switched off the default criteria.
2. Monitor scaled residuals and let simulate until they reach plateau
3. Check mass balance/difference between inlets and outlet
4. Started monitoring volume averaged velocity

Residuals:


Results:
Perforated plate:


Plate:


My questions:

1. Is it possible to do these simulations in 2D or use symmetry planes/cyclic symmetries?
This would help me to save time and also to get a finer mesh with the perforated plate but I'm unsure about using it since the first results showed recirculating zones/turbulent zones that would probably cross the borders.

2. There are still asymmetries in the profiles. I guess this means that the simulations are not fully converged? Can I take write an interpolation-file based on those results and simulate them on a finer mesh to enhance my results?

3. Max. velocities calculated during the normal plate and perforated plate differ by a factor of 2 (55 to 105 m/s)!? Is this caused by mesh differences? BCs are the same for all simulations.

4. The funny thing is that the supposedly easiest geometry is giving me the hardest time! I just don't get any results. The residuals started dropping for about 3000 iterations and suddenly started diverging what could be the cause?
Can anyone give me any advice for the "open geometry". It's also not that mesh intensive as the other two geometries.


Anyway, I would really appreciate some advice and sorry for the lengthy post!

Regards,
Luis

[LuckyTran]

I don't agree that the problem screams transient. I always start with a steady solver until I run into instabilities that requires a transient simulation, it also helps to determine whether your instability is numerically driven or is a physical hydrodynamic instability. Any numerical instabilities that you encounter in a steady solution is also a hint that your setup is not high quality.

Originally Posted by MrCaplin

1. Is it possible to do these simulations in 2D or use symmetry planes/cyclic symmetries?
This would help me to save time and also to get a finer mesh with the perforated plate but I'm unsure about using it since the first results showed recirculating zones/turbulent zones that would probably cross the borders.

2. There are still asymmetries in the profiles. I guess this means that the simulations are not fully converged? Can I take write an interpolation-file based on those results and simulate them on a finer mesh to enhance my results?

3. Max. velocities calculated during the normal plate and perforated plate differ by a factor of 2 (55 to 105 m/s)!? Is this caused by mesh differences? BCs are the same for all simulations.

4. The funny thing is that the supposedly easiest geometry is giving me the hardest time! I just don't get any results. The residuals started dropping for about 3000 iterations and suddenly started diverging what could be the cause?
Can anyone give me any advice for the "open geometry". It's also not that mesh intensive as the other two geometries.

1. In 2D you would not be able to simulate the individual perforations. If you don't need high-fidelity, you may be able to just model the inlet as a uniform mass-flow.
2. Asymmetries are hard to get rid of especially on an unstructured grid. To achieve perfectly symmetric results needs a uniformly, high quality grid. The problem is cells in one region are slightly more skewed than others and this leads biasing. A finer mesh does not necessarily solve this problem, it has more to do with grid quality than grid resolution.
3. If you are only comparing the maximum, it occurs at a single location and can be located anywhere in the domain. Very easy to achieve wildly different results especially if the geometry is not even similar. Just like 2), the disparity between the two grids can cause this. Mean or bulk quantities are a better comparison.
4. If you have already played with URFs and such then again, check the grid quality. I had similar issues before in a straight circular pipe that had 4 slightly skewed cells that showed the same behavior. When you re-meshed to reduce the skewness the problems went away.

[MrCaplin]

Originally Posted by LuckyTran

I don't agree that the problem screams transient. I always start with a steady solver until I run into instabilities that requires a transient simulation, it also helps to determine whether your instability is numerically driven or is a physical hydrodynamic instability. Any numerical instabilities that you encounter in a steady solution is also a hint that your setup is not high quality.



1. In 2D you would not be able to simulate the individual perforations. If you don't need high-fidelity, you may be able to just model the inlet as a uniform mass-flow.
2. Asymmetries are hard to get rid of especially on an unstructured grid. To achieve perfectly symmetric results needs a uniformly, high quality grid. The problem is cells in one region are slightly more skewed than others and this leads biasing. A finer mesh does not necessarily solve this problem, it has more to do with grid quality than grid resolution.
3. If you are only comparing the maximum, it occurs at a single location and can be located anywhere in the domain. Very easy to achieve wildly different results especially if the geometry is not even similar. Just like 2), the disparity between the two grids can cause this. Mean or bulk quantities are a better comparison.
4. If you have already played with URFs and such then again, check the grid quality. I had similar issues before in a straight circular pipe that had 4 slightly skewed cells that showed the same behavior. When you re-meshed to reduce the skewness the problems went away.

Thank you very much for your reply! I really appreciate it since there's no one at my institute who could help me out!!

By numerical instabilities do you mean diverging residuals (last picture) or fluctuations (2nd picture of residuals)? Or both?

2. I've continued both simulations and I'm waiting for the averaged velocity to reach a plateau. Let's see how the solution changes.

4. I was not able to create a completely structured mesh. I've also read that hexa cells are recommended for zones where the cells are flow aligned. So I sliced my geometry into areas where I expect recirculation zones (tetra mesh) etc. and where the flow simply follows the geometry (multizone mesh).

This is the result so far:

I have also used the multizone method for the first half of the two inner inlets.

The problem now is that as soon as I use an inflation layer I get highly skewed cells at certain edges (see pictures). The max value is around 99.4. is there any way to reduce the skewness in these areas?




Thanks in advance!



EDIT:
I figured out the problem concerning the different max velocities.
For whatever reason I chose the wrong model simulations including the non-perforated plate.
The model had twice the number of perforations in that area and thus yielded lower velocities.

[LuckyTran]

Originally Posted by MrCaplin

By numerical instabilities do you mean diverging residuals (last picture) or fluctuations (2nd picture of residuals)? Or both?

4. I was not able to create a completely structured mesh. I've also read that hexa cells are recommended for zones where the cells are flow aligned. So I sliced my geometry into areas where I expect recirculation zones (tetra mesh) etc. and where the flow simply follows the geometry (multizone mesh).

It is always preferable to have cells aligned with the flow direction to reduce numerical errors. When the flow is not aligned with your geometry, faces of hex cells have a higher probability of being not aligned with the flow. In those cases it's better to have tets (which have slightly random orientation). It's more about cell faces than hex vs tets.

I am referring to instabilities that persist even when the problem is not diverging (but the simulation refuses to converge to a stationary solution). These variations can have very large periods (require tens of thousands of iterations to observe). They are associated with separation bubbles or vortices, etc. that move around in the domain (over many iterations) rather than staying in one place. They can appear as asymmetries in a problem that should be symmetric. Sometimes these instabilities are real hydrodynamic instabilities, sometimes they are just caused by a poor grid preventing the solution from converging. If you only run transient simulations you'll always be inclined to interpret these as physical flow phenomenon.

But, in the absence of hydrodynamic instabilities and with stationary boundary conditions, the flow solution should be stationary (because nothing is driving any unsteady behavior). Results where URANS is used, in which these instabilities are not explained or appear out of nowhere, are extremely questionable. They are an indicator that something is wrong.