[myozinaung]

Hello everyone,

This is my first time posting a question on this forum.

Normally, ship resistance tests do not require an overset mesh for the dynamic mesh. Even for a planning hull, a morphing mesh approach is sufficient. DTCHullMoving tutorial from "multiphase/interFoam/RAS" uses that approach.

When I was running resistance simulations (2DOF, free pitch and heave) in shallow water, I found that there is not enough room for mesh morphing below the ship hull in certain cases where the trim and sinkage are significant. Some of the cells get squeezed until their volumes become essentially zero leading to the simulation divergence. Adjusting mesh morphing diffusivity method and morphing range (innerDistance and outterDistance) can help in some cases, but it does not solve the whole problem. Different adjustments might be needed for different ship speeds depending on the sinkage and trim history. This kind of problem is more likely to happen when a finer mesh is used.

To solve that, I wanted to test the overset mesh approach. I modified the DTCHullMoving tutorial for overset mesh by combining it with rigidBodyHull tutorial from the overInterDyMFoam. I was successfully able to run the simulation. The resistance convergence histories are attached. The total resistance values are similar for all DTCHull, DTCHullMoving and DTCHullMovingOverset (mine). But, the pressure and viscous components of Overset version is different from the those of DTCHull and DTCHullMoving.

My question is: Why are they different? Forces calculation/decomposition method in overset mesh is different from the normal one?

If you are interested in the case files, I will upload them.

[gigliagarf]

Hello myozinaung, can you post your case files so we can go over them? That might help to determine the differences.

[myozinaung]

The problem is now resolved. The resistance values are similar for both morphing and overset cases.
If you are interested in the case files, check the link below.

https://github.com/myozinaung/DTCMoving_Overset

[gigliagarf]

Happy to hear things are better for you! I found this document which outlines best practices for overset, maybe it would be of use to you if you do some larger motions. I found the tutorials for overset had different values for the fvSolution dictionary than what these guys are recommending. http://www.wolfdynamics.com/training...s_2021_OF8.pdf

[simucentral]

Hi,
If you could throw some light on how the problem got resolved, that will really be a great insight. in the snapshots you uploaded earlier, we see, even though the total resistance is similar, the pressure and viscous components are showing significant differences.
Thanks and regards.
akram

[myozinaung]

Hello,

Previously I used the solver settings (fvSolution and fvSchemes) from the rigidBodyHull tutorial because that is the overset mesh tutorial with a ship and propeller. The problem is the solver settings are not suitable for the resistance calculation. So I modified the solver settings to match the original DTCHullMoving tutorial settings which are set up for the resistance calculation.
The new results are attached for your reference.

Regards,
Myo

[simucentral]

Thank you so much for the quick reply.
I shall check that. Are you working in Openfoam.com or openfoam.org?
Thanks and regards,
akram

[myozinaung]

I used OpenFOAM v2206 (openfoam.com).

[ibe]

Hello,

I'm trying to run DTCMoving_Overset case (from git )



I running into some glitches.



The Allrun and Allclean scripts call for these scripts that aren't available..:
DTCMoving_Overset/background/restore0Dir
DTCMoving_Overset/hull/cleanCase0




Also,

I'm trying to recreate the results in the youtube tutorial

Ship resistance prediction (Luofeng Huang, UCL)

At around 36:43 of the video Dr. Huang references an .xls output file.
i've poked through a bunch of controlDict files and I can't find a useful example of how to export to an .xls file. Any suggestions ?


Thank you,

[myozinaung]

Which version of OpenFOAM are you using? Foundation or ESI?
Only ESI support the overset mesh.

restore0Dir and cleanCase0 are tutorial-run functions and they come with OpenFOAM installation (ESI version).
At the top of the Allrun scripts in "background" and "hull" folder you will see the following line:

. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions

It allows to use tutorial-run functions like restore0Dir and cleanCase0.

I think Dr. Huang converts the forces.dat file to .xls file manually.
You can find forces.dat file in the "postprocessing" folder during running simulation. It is generated by the forces function defined in the ControlDict

[ibe]

Hello,

I just installed this version
https://www.openfoam.com/news/main-n...rs-and-physics

which I believe is the ESI enabled version.



the scripts were found by correctly setting
WM_PROJECT_DIR='/opt/openfoam';
and

export PATH=$PATH:'/opt/openfoam/bin/tools';



I now have 3 different "DTC" cases:
DTCHull DTCHullMoving DTCMoving_Overset
all seem to run the Allclean + Allrun sequence
but I can't find any forces.dat file in any of these dirs..



Still poking around for clues.
Thank you,

[myozinaung]

forces.dat file should be in the dir: "DTCHullMoving\postProcessing\forces\0\forces. dat"

"postProcessing" folder will appear in the case dir when you start running the simulation and finish the first time step. It may take some time to complete the first time step.

[ibe]

your time on this is most appreciated.

Any suggestions are welcome...







Here's the log from the Allrun

and below that is the controldict

nothing seems out of place...

using the unix command

>> find -name 'force*' yields nothing

and there is no postprocessing folder or obvious warnings or errors.





(base) ie@ie-OptiPlex-9020:~/S/CODE/OPENFOAM22/DTCHullMoving$ ./Allclean
Cleaning case /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
(base) ie@ie-OptiPlex-9020:~/S/CODE/OPENFOAM22/DTCHullMoving$ ./Allrun
Running surfaceFeatureExtract on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running blockMesh on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running topoSet on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running refineMesh on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running topoSet on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running refineMesh on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running topoSet on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running refineMesh on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running topoSet on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running refineMesh on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running topoSet on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running refineMesh on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running topoSet on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running refineMesh on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running snappyHexMesh on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Restore 0/ from 0.orig/
Running setFields on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running decomposePar on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running renumberMesh (8 processes) on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running interFoam (8 processes) on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
Running reconstructPar on /home/ie/S/CODE/OPENFOAM22/DTCHullMoving
(base) ie@ie-OptiPlex-9020:~/S/CODE/OPENFOAM22/DTCHullMoving$





========== controldict ==========
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2206 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application interFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 35;

deltaT 0.0001;

writeControl adjustable;

writeInterval 1;

purgeWrite 0;

writeFormat binary;

writePrecision 6;

writeCompression off;

timeFormat general;

timePrecision 6;

runTimeModifiable yes;

adjustTimeStep yes;

maxCo 25;

maxAlphaCo 15;

maxDeltaT 0.05;

functions
{
forces
{
type forces;
libs (forces);
patches (hull);
rhoInf 998.8;
log on;
writeControl timeStep;
writeInterval 1;
CofR (2.929541 0 0.2);
}
}


// ************************************************** *********************** //

[myozinaung]

Please check the log.interFoam file and see the simulation ran successfully.
It should be inside the "/home/ie/S/CODE/OPENFOAM22/DTCHullMoving".

If there are errors inside the log.interFoam, you should check the other log files above. such as log.decomposePar, log.setField, etc.

Those log file should be in your case dir if you run the Allrun without any modification. Tutorial run function "runApplication" will generate those log files.

[ibe]

that was a very helpful suggestion.



quoting from log.interfoam . .



so I need to learn how to change the call to interfoam.



The other log files didn't have errors that I could see.



Thank you,







======== log.interfoam =====

--------------------------------------------------------------------------
There are not enough slots available in the system to satisfy the 8
slots that were requested by the application:

interFoam

Either request fewer slots for your application, or make more slots
available for use.

A "slot" is the Open MPI term for an allocatable unit where we can
launch a process. The number of slots available are defined by the
environment in which Open MPI processes are run:

1. Hostfile, via "slots=N" clauses (N defaults to number of
processor cores if not provided)
2. The --host command line parameter, via a ":N" suffix on the
hostname (N defaults to 1 if not provided)
3. Resource manager (e.g., SLURM, PBS/Torque, LSF, etc.)
4. If none of a hostfile, the --host command line parameter, or an
RM is present, Open MPI defaults to the number of processor cores

In all the above cases, if you want Open MPI to default to the number
of hardware threads instead of the number of processor cores, use the
--use-hwthread-cpus option.

Alternatively, you can use the --oversubscribe option to ignore the
number of available slots when deciding the number of processes to
launch.
--------------------------------------------------------------------------

[myozinaung]

In the decomposeParDict, the no. of subdomain is 8. You need 8 cores/threads to run interFoam. If you don't have enough cores/threads on your system, use a lower number for subdomain.

[ibe]

My system has four cores.
https://www.dicytrends.com/optiplex-...pecifications/


Assuming that translates to supporting four subdomains,

I first tried

numberOfSubdomains 4;
and

then

numberOfSubdomains 1;
in decomposeParDict


I've attached the corresponding log.interfoam files,

and will poke through the forums in search of solutions.

Any suggestions or references which sacrifice parallelism or speed i.o.t. run more reliably would be most appreciated.

[ibe]

Here's another thread that addresses some of the problems I'm seeing.


https://www.cfd-online.com/Forums/op...ubdomains-not-
equals-number-processors.html

[Yann]

Did you run decomposePar again after modifying decomposeParDict?

decomposePar -force

Yann

[ibe]

Hi,



I'm just rerunning the Allrun script which has this excerpt


# runApplication decomposePar
runParallel -s decompose redistributePar -decompose


I precede that call with Allclean - which wipes out all the intermediate result dirs so I believe that accomplishes the -force intent.




That other thread gave me the info on the subdomains necessary (it seems) to make runs and start looking at force output.

progress!



thanks