[Solved] URANS with CfdOF / transient simulation of macroscopic vortex ?

[Raedchen_im_System]

Dear Forum,

I've been trying to set up a simulation of the macrocopic vortices in the Kármán vortex street for a few weeks now. I am trying to get a result equal to this video: https://www.youtube.com/watch?v=IDeGDFZSYo8. I built a 2D-model of a pillar surrounded by a flow in a fluid:
.

Simulation Model.JPG (274.46 KiB) Viewed 5445 times

.
I selected a transient simulation (unsteady RANS-Simulation / URANS):
.

Physical Model.JPG (25.55 KiB) Viewed 5445 times

.
As a result, I don't see any macrocopic vortices:
.

Result.JPG (27.76 KiB) Viewed 5445 times

.
I tried this simulation with many variations, for example change of the mesh size, change of the velocity from 0.5 m/s up to 50 m/s and change of the fluid from air to water, but these changes showed no effect. Rick Palo states in his blog that he was successfull with his simulation. As fluid, he used air, but he didn't write anything about the dimensions or the speed of his model.

I have the following question: Is my intended simulation feasible with the PIMPLE-algorithm and the RASModel "kOmegaSST" ? If this simulation is feasible, why does my simulation show no macroscopic vortices? Must I change simulation parameter (input speed, simulation time, ...) ?

I found a similar simulation in the book "CFD-Modellierung" by Rüdiger Schwarze. In contrary to CfdOF, he uses the k-epsilon-Modell and the pisoFoam-algorithm. Is this approach more appropriate for this simulation?

Thank you very much for your answers and your help in advance !

OS: Windows 10 Version 2004
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24276 (Git)
Build type: Release
Branch: releases/FreeCAD-0-19
Hash: a88db11e0a908f6e38f92bfc5187b13ebe470438
Python version: 3.8.6+
Qt version: 5.15.1
Coin version: 4.0.1
OCC version: 7.5.0
Locale: German/Germany (de_DE)

OpenFoam version: ESI-OpenCFD, v2012

[thschrader]

Hi Raedchen,
welcome to the forum!

I ran the simulation below as steady-state and transient.
The steady state solution does not converge, the residuals "swing".
When running a transient analysis at Re=120, the opposite happens:
The flow field is perfect symmetric, the residuals are flat as runways.
(with turbulence, without)
And that is the point I do not understand.
I wonder how Rick Palo got a solution with his model. Maybe a "lucky punch".
However, interesting problem. Looks simple, but...
Done with bluecfd.
Here is the FC-file:

karman_vortex_ts.FCStd

(35.75 KiB) Downloaded 124 times

And a fast running steady-state sim for checking convergence:

naca2412.FCStd

(405.86 KiB) Downloaded 120 times

flow_around_cylinder.JPG (80.44 KiB) Viewed 5371 times

[thschrader]

maby splitting the inlet into 2 domains with minimum speed-difference
to force a movement. In reality the incoming flow at the cylinder is multidirectional,
not only in x-axis with z/y=0.

[Raedchen_im_System]

When running a transient analysis at Re=120, the opposite happens:
The flow field is perfect symmetric, the residuals are flat as runways.
(with turbulence, without)

Hi thschrader,

I ran this model as a transient simulation, and everything is fine: I see the vortices, they are build up after 10 seconds. I increased the simulation time from 10 seconds to 30 seconds:
.

Simulation Time.png (17.95 KiB) Viewed 5293 times

.
In order to save simulation time, I meshed the array with larger elements. The FreeCad-file is attached.
.
I made a Video, this Video can be seen via Youtube:

https://youtu.be/_LZG9UFk8kQ

In the original model, I worked with too high a Reynolds number. Thank you very much for your help !

Bernd

[Raedchen_im_System]

I ran this simulation also with the physics model "RANS" and "k omega SST" with a transient and steady simulation. In contrary to the simulation with the laminar turbulence model, the characteristic Karman vortex street can not be seen. It seems that the "k omega SST" approach for turbulence suppresses the oszillation.
.
The residuals in the steady simulation seems to have a convergence:
.

Residuals Turbulance Model steady sim.JPG (71.08 KiB) Viewed 5263 times

.
For the steady simulation and the transient simulation, macroscopic vortices can be seen in Paraview with the steam tracer:
.

Steam Trace Steady simulation with RANS.JPG (163.43 KiB) Viewed 5263 times

[thschrader]

...
I see the vortices, they are build up after 10 seconds. I increased the simulation time from 10 seconds to 30 seconds:
...

After i ran my sim, I had a look at several YT-videos and my suspicion came up, that the sim-time was too short.
Bernd, great job!

Some ideas:
Try different meshers (maybe gmsh is problematic in 2D-cases, because the tetrahedrons are transformed into wedges)
Develop a model, that uses ONE mesh to recreate the complete cw-curve below.
For me the interesting region is above Re=200000 (wind-loading at storm)
BTW: check the U/p dict-files after case writing.
Regards Thomas

pic1.JPG (100.05 KiB) Viewed 5195 times

pic2.JPG (67.8 KiB) Viewed 5195 times