## Computing forces: how to setup proper simulation?

A subforum specific to the development of the OpenFoam-based workbenches ( Cfd https://github.com/qingfengxia/Cfd and CfdOF https://github.com/jaheyns/CfdOF )

Moderator: oliveroxtoby

Posts: 1394
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Computing forces: how to setup proper simulation?

OK, i have a problem with a simulation.
I want to calculate the resulting wind-force on an antenna-cluster with the steel-support.
Tried laminar, turbulent, varying the k-omega-values, using differnt turbulence calculators...
Doesnt matter what I do, I cant get the residuals falling to 10e-3. The resulting force calculated
in paraview is 18 kN (at 42 m/s inlet speed air), thats 10 times higher than in should be
Whats the best way to setup such a simulation?
Help welcome.
Thomas
AntennaClusterCFD.JPG (68.03 KiB) Viewed 1164 times
cfmesh.JPG (103.63 KiB) Viewed 1164 times
oliveroxtoby
Posts: 257
Joined: Fri Dec 23, 2016 9:43 am
Location: South Africa

### Re: Computing forces: how to setup proper simulation?

Do the residuals fall and level off, or fall at first and then increase again? If the residuals level off, it is probably nothing to worry about: sometimes there are transient features of the flow field that get picked up and then you do not get convergence to a truly steady solution. A sustained increase indicates instability.

Does the final flow field look reasonable? Pressures at the far field correct? No nasty spikes etc?

Don't forget that the "p" field written by OpenFOAM is actually 'kinematic pressure', i.e. p/rho, although that wouldn't explain a 10x discrepancy.

You could try putting an entry for a 'forces' function object in the system/controlDict for your OpenFOAM case - see https://www.openfoam.com/documentation/ ... orces.html - and check if the force has converged and whether this tallies with the paraview result you are getting.
Posts: 1394
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: Computing forces: how to setup proper simulation?

@Oliver:
Thanks for your hints. The residuals are falling and remain constant after 60 Iterations.
But I will try an other approach. Lets start with a single cylinder alone. I have some
german DIN manuals to calculate the drag-coefficient/windforce for calibrating the "windtunnel".
After that I will put the antennas into the simulation.
oliveroxtoby
Posts: 257
Joined: Fri Dec 23, 2016 9:43 am
Location: South Africa

### Re: Computing forces: how to setup proper simulation?

Sounds like a good plan. For an accurate solution it would be wise to move the outer boundaries out a bit - around 10-20 times the body diameter is the rule of thumb - although this would not make anything like a 10x difference.
Posts: 1394
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: Computing forces: how to setup proper simulation?

@Oliver:
OK, the windtunnel works.
I was completely wrong when setting the turbulence-parameters.
When using the k-omega-dicts from the millenium-falcon, the result
is fine (and I used a much larger computation-domain like you did).
For a cylinder D=220 mm, L=2200 mm, v=150 km/h I get a drag factor of 0,6,
which matches nearly perfect to my DIN-manuals. The same works with snappyhexmesh.
I could not test gmsh, the dialog does not open when clicking the icon.
regards Thomas
OS: Windows 10
Word size of OS: 64-bit
Version: 0.17.13303 (Git)
Build type: Release
Branch: master
Hash: b47e011c1cc6357fa776624d371ed434989c79b1
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.1.0
Locale: German/Germany (de_DE)
oliveroxtoby
Posts: 257
Joined: Fri Dec 23, 2016 9:43 am
Location: South Africa

### Re: Computing forces: how to setup proper simulation?

Wed Feb 21, 2018 2:39 pm
@Oliver:
OK, the windtunnel works.
I was completely wrong when setting the turbulence-parameters.
When using the k-omega-dicts from the millenium-falcon, the result
is fine (and I used a much larger computation-domain like you did).
For a cylinder D=220 mm, L=2200 mm, v=150 km/h I get a drag factor of 0,6,
which matches nearly perfect to my DIN-manuals. The same works with snappyhexmesh.
Great.
Wed Feb 21, 2018 2:39 pm
I could not test gmsh, the dialog does not open when clicking the icon.
Hopefully fixed - there was some refactoring in FEM workbench code that we use for gmsh.
HarryvL
Posts: 1010
Joined: Sat Jan 06, 2018 7:38 pm

### Re: Computing forces: how to setup proper simulation?

Thomas, did you rerun the antenna assembly? Could you describe workflow and results please? I would be interested to know what the effective drag of the assembly is. Thanks. Harry
Posts: 1394
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: Computing forces: how to setup proper simulation?

HarryvL wrote:
Sat Mar 24, 2018 1:16 pm
Thomas, did you rerun the antenna assembly? Could you describe workflow and results please? I would be interested to know what the effective drag of the assembly is. Thanks. Harry
model-scale 1:1, antenna-lenghts 2,0 m, type Kathrein K80010865, according to

mesher: cfmesh, 350000 cells, meshing time 290 sec.
solver: simpleFoam, steady, incompressible, turbulence-model k-omega SST. runtime 3,5 hours.
fluid: air, density 1,25 kg/m^3.
inlet-speed 42 m/s (=150 km/h, according to Kathrein datasheets).
After 700 Iterations the residuals remain stable and the results dont change any more.
In paraview you can calculate the drag-force by using several filters.
The drag_x on the whole cluster is 1707 N. When doing a calculation "by hand" with an approach I
normally uses in my statics-calculation (1x frontal loading on antenna, 2x rear under 45 deg + tubes)
I get 1663 N. The error is below 3%. From a scientific point of view the simulation can be done better
(much finer mesh, more boundary-layers, mesh-refinement in downstream region, bigger computing domain and...)
but I must find a compromise due to my not so sophisticated computer.
turbulence-parameters: I found out that I get the "best" results when using the default parameters
in the input dialogs.
To be done: simulating the effect of cable-packages / ladders on the antenna structure.
cfmesh.JPG (182.56 KiB) Viewed 613 times
model.JPG (45.4 KiB) Viewed 613 times
paraview.JPG (147.49 KiB) Viewed 613 times
smath.JPG (25.03 KiB) Viewed 613 times
Posts: 1394
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: Computing forces: how to setup proper simulation?

and here is the FC-file.
cluster.FCStd
Done with
OS: Windows 10
Word size of OS: 64-bit
Version: 0.17.13433 (Git)
Build type: Release
Branch: master
Hash: b45bc4889d390eb50022a49a58c6af80f4a328f5
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.1.0
Locale: German/Germany (de_DE)
Posts: 1394
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: Computing forces: how to setup proper simulation?

This is a calculation with a cable-package mounted at the mast. Such packages
are normally used to feed the cell-phone antennas. Tube diameter 200 mm, each cable 25 mm (=1"),
Length 1 m. Inlet speed 42 m/s (=150 km/h and q=1,10 kN/m^2). Number of cells 1400000 (yep, my first simulation
with more than 1 million cells...). Runtime 5 hours (I expected much more), stable residuals after
400 Iterations.
Results:
computed overall drag-force 226 N, which gives a drag-factor of 0,91. A check-back according
to DIN 4131 "Antenna-systems" gives 236 N. The factor 0,65 behind the bracketts is a
slenderness-reduction-factor, the terms inside the bracketts are only valid for an infinite long system.
I am wondering why the k-values (k=turbulent kinetic energy) are the highest behind the tube?
I would expect the maximum between the cables. Mmmh...modelling error?
To be continued...
(BTW: to all the folks who are ranting on FC: show me a free software, which can do this!)
force.JPG (20.59 KiB) Viewed 537 times
model.JPG (72.27 KiB) Viewed 537 times
meshRefinement.JPG (152.58 KiB) Viewed 537 times
pressure.JPG (105.57 KiB) Viewed 537 times
turbulent_kinetic_energy.JPG (23.12 KiB) Viewed 537 times