[RobertHB]

I'm not exactly sure, as my simulation are never consistent. From what i can figure, as long as all patches are the exact same size, have the same BC and patch name, just running the command might work. But as for all functions in OpenFoam: If you mess something up, the program will tell you. So just try.

[gu1]

Hi Robert,

I did several iterations, sorry for just answering today. The question and the problem I am having is ... WHERE IS THE TURBULENCE?

[RobertHB]

My first guess would be, that the runtime of your LES simulation is not long enough for the flow become turbulent. But santiago provided a few explanations in post #6 for why a pipe flow might not become turbulent at all. Maybe it's one of those reasons.

[Santiago]

Originally Posted by gu1

Hi Robert,

I did several iterations, sorry for just answering today. The question and the problem I am having is ... WHERE IS THE TURBULENCE?

That plot tells nothing about turbulence! I don't understand what you expect to get from just the residuals.

[gu1]

Originally Posted by Santiago

That plot tells nothing about turbulence! I don't understand what you expect to get from just the residuals.

Hi Santiago,

I just showed the residual to demonstrate the convergence and iteration time (not important at the moment).

1. Having just a high Re doesnt guarantee obtaining a turbulent field. In an error-free numerical solver, an initially laminar Poiseuille flow with Re*=1000000 will stay laminar, unless you introduce an instability.

2. Having obstacles in the flow may or may not trigger turbulence. It depends on many things. Besides, it may triggers turbulence in the wake generated by the blockage.

3. You could perfectly perturb a potential field with perturbU, if youre modelling wall bounded channels. I dont know whether extrapolating this method to any sort of flow will render useful. I remember that perturbU is an implementation of the work of Schoppa & Hussain, which provides an unstable mode for channel flows.

I'm working with Reynolds = 5300 (I believe it's low-Reynolds) and I also believe that Robert is correct about the simulation time.
At the present moment I am thinking of disturbing the fluid using the 'perturbU' tool... OR changing all my parameters to mapped (according to the tutorial: /opt/openfoam5/tutorials/incompressible/pisoFoam/LES/pitzDailyMapped), but still I'm trying to understand if this tutorial is configured as a cyclic domain, could you comment?

Incidentally, have you ever used the 'postChannel' tool? Can it be used in simulations like mine (pipe)?!

log perturbU compilation:

Making dependency list for source file perturbU.C
could not open file cyclicAMILduInterface.H for source file perturbU.C due to No such file or directory
could not open file cyclicAMIPolyPatch.H for source file perturbU.C due to No such file or directory
could not open file addLatestTimeOption.H for source file perturbU.C due to No such file or directory
g++ -std=c++11 -m64 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam5/src/finiteVolume/lnInclude -I/opt/openfoam5/src/cfdTools/general/lnInclude -IlnInclude -I. -I/opt/openfoam5/src/OpenFOAM/lnInclude -I/opt/openfoam5/src/OSspecific/POSIX/lnInclude -fPIC -c perturbU.C -o Make/linux64GccDPInt32Opt/perturbU.o
In file included from /opt/openfoam5/src/finiteVolume/lnInclude/ddtScheme.C:30:0,
from /opt/openfoam5/src/finiteVolume/lnInclude/ddtScheme.H:342,
from /opt/openfoam5/src/finiteVolume/lnInclude/fvcDdt.C:28,
from /opt/openfoam5/src/finiteVolume/lnInclude/fvcDdt.H:205,
from /opt/openfoam5/src/finiteVolume/lnInclude/fvc.H:44,
from /opt/openfoam5/src/finiteVolume/lnInclude/fvCFD.H:8,
from perturbU.C:26:
/opt/openfoam5/src/finiteVolume/lnInclude/cyclicAMIFvPatch.H:39:35: fatal error: cyclicAMILduInterface.H: Arquivo ou diretório não encontrado
compilation terminated.
/opt/openfoam5/wmake/rules/General/transform:25: recipe for target 'Make/linux64GccDPInt32Opt/perturbU.o' failed
make: *** [Make/linux64GccDPInt32Opt/perturbU.o] Error 1

[Santiago]

Originally Posted by gu1

Hi Santiago,

I just showed the residual to demonstrate the convergence and iteration time (not important at the moment).



I'm working with Reynolds = 5300 (I believe it's low-Reynolds) and I also believe that Robert is correct about the simulation time.
At the present moment I am thinking of disturbing the fluid using the 'perturbU' tool... OR changing all my parameters to mapped (according to the tutorial: /opt/openfoam5/tutorials/incompressible/pisoFoam/LES/pitzDailyMapped), but still I'm trying to understand if this tutorial is configured as a cyclic domain, could you comment?

Incidentally, have you ever used the 'postChannel' tool? Can it be used in simulations like mine (pipe)?!

log perturbU compilation:

Postchannel averages along planes of statistical homogeneity in wall channels (horizontal planes). In pipe flows you need to average radially, in principle you can use postChannel as a template.

[gu1]

Originally Posted by Santiago

1. Having just a high Re doesnt guarantee obtaining a turbulent field. In an error-free numerical solver, an initially laminar Poiseuille flow with Re*=1000000 will stay laminar, unless you introduce an instability.

2. Having obstacles in the flow may or may not trigger turbulence. It depends on many things. Besides, it may triggers turbulence in the wake generated by the blockage.

3. You could perfectly perturb a potential field with perturbU, if youre modelling wall bounded channels. I dont know whether extrapolating this method to any sort of flow will render useful. I remember that perturbU is an implementation of the work of Schoppa & Hussain, which provides an unstable mode for channel flows.

Hi Santiago, sorry to open this topic again, after a while studying I learned a lot about my case ... and subjects that I did not master at the time that I generated this topic are clearer these days.

As you mentioned in the featured post (1), one of the ways to generate turbulence is to increase the Reynolds number and let the simulation work for a long time. Below I attached the image of the mag (U) at points of the domain to a flow in Reynolds 44000. I also attached the average profile.

After that, I mapped the last time of this field to a new folder, and together I made a copy of the 'constant' and 'system' folders used in this simulation (where only the 'nu' was modified in order to put the Reynolds in 5300) . Unfortunately the fluid laminated. Could you help me understand the problem?

I tried the perturbU tool, but only the schematic div(phi,U) Gauss cubic maintains the fluctuations, any other scheme, causes it to laminarize ... (and for that reason I resorted to increasing the Reynolds). I wonder if there is another solver capable of doing something similar to 'perturbU'... exists?

[boundary93]

Hey are you still working on your LES Simulations, I have a similiar problem like you. But I created a turbulence flow with a coarse mesh and a mapped inlet. After that I recieved a turublent velocity field and I mapped it on a finer grid. But then the velocity profil is getting laminar again, if I run the simulation on the finer grid.

Is there another way to keep the flow turbulent or is the only way to use Gauss cubic?

[gu1]

Originally Posted by boundary93

Hey are you still working on your LES Simulations, I have a similiar problem like you. But I created a turbulence flow with a coarse mesh and a mapped inlet. After that I recieved a turublent velocity field and I mapped it on a finer grid. But then the velocity profil is getting laminar again, if I run the simulation on the finer grid.

Is there another way to keep the flow turbulent or is the only way to use Gauss cubic?

Use Gauss Linear.
What I ended up doing in the end was picking up a turbulent field that I had on ANSYS. But something that I tested and worked out was to raise the Reynolds number (44000) and let the turbulence develop by itself... then I would lower Reynolds a bit, leave the process again and so on until get to the Reynolds that I wanted (5300).

[Santiago]

One way of "triggering" turbulence in a field is by adding a 'random force' in the predictor step. Like this you insure mass conservation and keep the solution in L2 space. Think of it as a "false" bouyancy term.

Running a high-Re solution and then going back to a lower Reynolds might give you a "wrong" energy spectra. PISOFOAM tends to be overdissipative, that means that for eddy viscosity models it may give you a lower-than-normal SGS fluxes. Meaning that the dissipative range is partly modelled as isotropic (the model) and other important chunk is not (PISO error). The latter does not depend on Reynolds, but on the time frequency. Thus, higher the Reynolds, Higher the frequency and higher the anisotropic error.
Check the higher statistical moments and the energy spectra.

[boundary93]

I have a Re of 2500 an I get really good results when i use a coarse grid first and then Gauss cubic wiht a finer grid (I mapped the results from the coarse grid as start for the fine grid). With Gauss linear I get a laminar Profil again.



I tryed to start wiht higher Reynoldsnumber some weeks ago, but the results where not that good.

[gu1]

Originally Posted by boundary93

...With Gauss linear I get a laminar Profil again.

I also had this problem, when it came out of Gauss cubic it laminarized. It means that it is still not good... and for LES the recommended one is 'Gauss Linear'.

In fact, I think Santiago understands more about this subject than I do. I went to a field that I had developed in ANSYS.

I saw it once, and you could try something like that... was to use the boxTurb tool that OpenFOAM makes available. However, it does not work for pipe, so you would have to create the geometry of a channel that fits within your domain and import the disturbed field.