Mesh around ship with appropriate free surface refinement
 

Hi,
I'm looking for a way to generate a mesh around a ship with the "typical" refinement of the free surface region to capture the waves.
Basically, what I intend to do is following:
- start with a base grid (from BlockMesh) with identical cells of aspect ratio approx. 1
- in SHM:
- refine near hull and appendages as usual by isotropic splitting of cells (1 -> 8)
- refine the free surface further away from ship mostly normal to the initial waterplane (anisotropically) as the waves are expected to be significantly longer than high (I don't want to waste cells, isotropic refinement of larger regions significantly pushes cell count)
- snap to hull and appendages
- create inflation layers for boundary layer

The difficulty is the anisotropic refinement of the free surface region. In Hexpress or Star-CCM+ mesher I can define either isotropic or anisotropic refinement for a region. In SHM, as far as I understand it, only isotropic refinement is possible in the Dict and the hex8 class referenced by SHM (although the refineMesh utility has anisotropic refinement).

Does anyone have a solution to this problem, either by a modification to SHM or a specific workflow?

Thanks
Hannes

Hi Hannes.

what i do is to mesh everything isotropically in sHM, snap, add the layers and than refine the freesurface using the setSet to select the freesurface area and refineMesh to refine anisotropiacally (just in the z direction).

good results so far...

Hi Vieri,

thank You for the explanation. I'll try that way as well as one described in a paper I just found: http://www.tfd.chalmers.se/~hani/kurser/OS_CFD/ChristofferJarpner/ReportInOpenFOAMbyChristofferJarpner.pdf

Nice website, by the way.

Cheers,
Hannes

Hi Hannes,

It seems that the link is not working anymore. Could you please forward me the file?


Thank you!

PM me your Email.
Hannes

Greetings to all!

For the sake of future reference, the link was sent back to the historic side (2011) of the course ;): http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2011/ChristofferJarpner/ReportInOpenFOAMbyChristofferJarpner.pdf

Best regards,
Bruno

pdf
 

Thank you very much Bruno.

Obrigado!

hi all,
i am dealing with same problem, if i refineMesh (in dirZ) before SHM, shm doesn t do layers to good, and split a lot of cells at the junction of free surface and hull. but if i do shm them refineMesh it create files in the case directory a lot of cells, loops, anchors .obj ... and the solver fail because of negative alpha1...
any subjection ?

dear Foamers,
i have made some little progress, i refine the free surface with toposet and refineMesh but when i run snappyhexmesh it's refine to much the cells around the hull selected with toposet...
do i need to make my own mysnappyHexmeh to obtain a good mesh.?
should i make two mesh and stich them?
going trought the paper of Christoffer Jarpner look very interesting but a bit hard isn't it???
thanks for helping LL

Hi laurent98,

I'm not sure how much you are familiar with sHM,
but from what you wrote two options come to my mind that could help you

* you switch the order of your process: first run sHM and then run topoSet
and refineMesh

* limit the number of cells with the keyword maxGlobalCells in the sHMD

I hope I got your question right if not let me know.

regards

Hi Colin,
thank you for reply. To answer your question, I play with openfoam during my free time, and use finemarine of numeca at work since a year... so I still have a lot to learn...
I did as you suggest shm then refinemesh, the domain set in toposetDict is like a U around a refining box.
as you can see I ve got a gap between hull and the limit of the box. Of course I will have to adjust the shmD to have the same size in Z between box and freesurface, but because of diffusion, refineMesh will always refine more cells around the box...
also refinemesh in z direction only make some strange cells around, like cube inside cube.. see the slice image cut.jpg
so, I am thinking of making two different mesh one for the freesurface, and one for a small box around the hull, is there something better ?
I will be happy with a mesh like the one
http://www.youtube.com/watch?v=_j-zT...eature=related
best regards LL

Hi LL

from the video I think I could see what kind of mesh you want
but let me summarize in my own words to see whether I grasp what
you want:

You want to have the mesh refined around the ship hull, rather dense
in order to resolve e.g the boundary layer, which you basically want to
achieve with sHM

However in the area of the free surface you want to refine the mesh
as well especially in z direction to better capture the wave elevation.

If this is so my suggestion would be:

- create a coarse background mesh with blockMesh

- use snappyHexMesh only to mesh the surface and use refinementMode
distance and add layers

- then use topoSet with a box refinement in order to refine the free
surface

I hope I got your idea right. However the above mentioned way provides
good results for me.
If I didn't get your idea you might want to provide some sketches which
illustrate your problem and a sHMD as well.

regards
Colin

hi Colin,
you've got exactly right my ideas
i did as you said, and trying my best to match the box limit bettewen the hull refinement and the FreeSurface Z refinement.
good idea to use distance, i never used that option before...
but because i have a cell (nCellsBetweenLevels 1) in the FS refinement place, it make undesired splits cells as you see on the picture.
is there a equivalent of nCellsBetweenLevels 0 .??
thanks you again for helping LL

So you are trying to adjust the blocks directly to the refinement
which you are getting from snappyHexMesh?

Well the solution to this is simply defining a box which also includes
the ship even if there is no more mesh (inside of the ship)

If you want to have more refinement in certain areas you have to define
several boxes which are overlapping.

Did you get my idea?
So don't worry about boundaries but simply use overlapping refinement areas.

i think it is what i am doing with the 'box1' i attach some of my files if you have time to look at it, i think you will better understand , of course all advice will be very welcome!
regards LL

hello
after a week-end playing with blockmesh, createpatch, mergemesh stitchmeshes, i am nearly there... still some inside patch to get rid off . mergeOrSplitBaffles ..???

Hi,
I'm getting quite good meshes using blockMesh, sHM, topoSet and refineMesh by now (in OF2.2.x). I start with an isotropic grid for the entire domain with a split exactly on the designated waterline (approx. 10e4 cells). Then I refine isotropically around the ship and at the waterline, especially in the Kelvin angle region (sHM), followed by snapping and layer insertion. Last I split normal to the waterplane only in the region of the expected wave height.

Dear all,

I'm keenly interested in the described use of SHM and refineMesh and I've read your previous posts.
I still have trouble in refining the free surface region.

My procedure is:

1. run blockMesh
2. run SHM (setting castellated, snap, layers as true)
3. run topoSet to select a box to be refined
4. run refineMesh over the selected box and refining just in normal direction

It's not clear to me if I have to run repeatedly topoSet and refineMesh, adapting every step the box to be refined in topoSet, because the refineMesh can split just one initial cell into two (in normal direction).
Is this the only way or a smarter procedure exist?
Any suggestions (also about my workflow) is really appreciated! Thanks for youe support,

Best regards.

Andrea

try this:

1. run blockMesh
2. run SHM (setting castellated as true and snap, layers false)
3. run topoSet to select a box to be refined
4. run refineMesh over the selected box and refining just in normal direction
2. run SHM (setting castellated as false and snap, layers true)

if you need more than one anisotropic refinement you will need to rerun toposet and refinemesh more than one time.

best Regards,

V.

Hi Vieri,

thanks for your reply.
I've tried the procedure you suggested, but still troubles remain. Using the following procedure:

1. blockMesh
2. SHM (setting castellated as true, snap false, layers false)
3. topoSet
4. refineMesh
( till now checkMesh is very good !! )
5. SHM (setting castellated as false, snap true, layers true)

I was hoping this would work fine, but the following error was reported:

--> FOAM FATAL ERROR:
Number of cells in mesh:1948200 does not equal size of cellLevel:918205
This might be because of a restart with inconsistent cellLevel.

It seems that the 0/cellLevel file has not be updated after the refineMesh phase.
How did you manage this problem, if it happened to you in the past?

Thanks in advance, best regards.

Andrea

Remove the 0 directory (save all relevant field data (U, p, ...) in 0.org before)

For getting the best cell sizes for resolution of a typical wave train several refine passes in normal direction are usually required, but, if you want to limit the normal refinement to specific refinement levels (e.g. up to one below the hull refinement level) you run into challenges after the first pass due to loss of information (cellLevel).

Hannes

Hi Andrea,

to avoid the mentioned error message and to
prevent you from copying folders and so on you could also
use the -overwrite flag for some of the commands.
That works for me.

So the workflow looks like:

1. blockMesh
2. snappyHexMesh -overwrite
3. topoSet
4. refineMesh -dict -overwrite
( till now checkMesh is very good !! )
5. snappyHexMesh -overwrite


This however makes it impossible to see earlier results of your mesh.


A question that came up to me:
How much does the mesh quality improve if you do the snappy in two
steps instead of one.

my current procedure looks like:

blockMesh
surfaceFeatureExtract -includedAngle 150 (...)
decomposePar
snappyHexMesh -overwrite (of course with mpirun etc)
reconstructParMesh
topoSet
refineMesh -dict -overwrite

then changing the set in the refineMeshDict

topoSet
refineMesh -dict -overwrite

with this procedure I get some good results.

Do you think with my approach and yours combined the results could be
even more improved?

Dear all,

thanks for all your replies. They have been very useful to me, and now my procedure works fine.

About your issue Colin: as you know the problem is related to mesh quality.
Refining the mesh in the free surface region after having completed all the three SHM phases (castellated, snap, layer) could be critical for skewness and non-orthogonality of cells.
So a good solution can be move up the refineMesh phase, just after the castellated meshing.
As Vieri suggested, this works quite fine for me.

But some issues regarding the layers insertion remain: the boundary layer appears not complete in many areas.
I think you have managed similar problem, very frequently, using SHM in the past. Which parameters in my SHMD (please see attached file) can improve my boundary layer, in your opinion?

Thanks again, regards.

Andrea

Dear Andrea,

I have also troubles with the layer settings and I
overcome it with a more or less suitable workaround:

scaling down the ship to model scale and then simply just add
only one layer, for adding more layers doesn't work.

see attached my sHMD for comparison. I hope you find the information
you need.

regards

Dear all,

I try to mesh with refinement in z direction. I use the procedure blockMesh/SHM/topoSet/refineMesh but when I run topoSet, I have the following message:

Create polyMesh for time = 0

Reading topoSetDict

Time = 0
mesh not changed.
Created cellSet refineCells
Applying source boxToCell
Adding cells with center within box (-30 0 -2) (66 -24 2)
cellSet refineCells now size 0

End

It's normal to have size 0? Where is my mistake?

I attache my blockMesh and topoSetdict.

best regards

Hi all

I found the solution. It seem I must create an box in SHM around the free surface to have a size different than 0 whit topoSetDict.

But now, when I use refineMeshDict, even if in direction part in refineMeshDict, I choose only "normal", always It refine all cells in all directions like if he don't take account of topoSetDict and refineMeshDict.

Any Idea?

Best Regard

Vince

Ok I resolve my problem with refineMesh. I just forget to indicate the file where is the refineMeshDict.

Now it's ok.

Vince

Hi Vince,

Thanks for your contribution. Do you mind post your case? I never used refine mesh before and it will be good to compare my results?


Regards,
Rafael

Hi Rafael

Sadly, I can't post this case because the CAD geometry is confidential. But I'm going to test the KCS hull and I will be happy to post this case. I hope I will have some good result to show.

Regards
Vince

It will be good to see your KCS hull results. Do you have any experimental data to compare it?

Hi Rafael

I have some experimental data from the Gothenburg 2010 workshop but if you have more data base, I'm interesting to see that.

Regards
Vince

Hi Rafael

I test the KCS with this meshing method. I join the folder, but sadly for the moment, I have a Ct=3.21.10-3 where it's expected Ct=3.711.10-3, so an error up to 13%.

I use a simple K-epsilon model for turbulence and for numerical scheme, you can see in the folder.

If anybody have an idea to increase the precision.

I must delete the CAD file to upload my case but if some people would like the CAD, I can send by mail.

Regards

Vince

Hey Vince,

have you tried the k-omega-SST turbulence model instead of the
k-epsilon model?

For me the k-omega model gives somewhat better results than
the k-epsilon.

It would be interesting to see whether you could confirm that or not.

kind regards
Colin

Hey Colin

I test yesterday the same calcul with kOmega SST model. If it's little better, I haven't a result closed to experience yet.

An another problem that if I see the forces evolutions, it's not stabillize after 100s (I work with the full scale model). I attached the Fpx, Fvx et Fpz evolution.

In your opinion, what's wrong? My mesh, maybe too coarse? Or my schemes (I modify the div(rho*phi,U), div(phi,k) and div(phi,omega) ?

You can note, I use for k, omega and nut parameter, the formula found on this page:

http://www.cfd-online.com/Wiki/Turbu...ary_conditions

Kind regards

Vince

Hi Vince

I noticed one major difference:
You use interFoam while I use LTSInterFoam.

Apart from that:

• What is your value for I in the formula for k? I use 0.005
• Your value for Cmu is probably 0.09 as suggested?
• What is your turbulent length scale? I use here 5% of Lpp

Concerning the convergence:

• It is recommended that the water passes the domain 3x times for a transient calculation! Was this the case after 100s?
• with LTSInterFoam I need approx. 10.000 Iterations, and then I'm using the average over the last 2000 Iterations

fvSchemes (for comparison only, keep in mind that I use LTSInterFoam):


I can't tell what the influence of your mesh is, but a coarse mesh can also

lead to a more stable calculation for waves are dampened.


Does that help you?



regards
Colin

Hi Colin

Thanks for yours indications.

I use 0.001 for I (I'm going to test with 0.005)

Mu turbulent lenght scale is 1 Lpp (I assume it's too hight)

My Cmu is 0.09

For my fvscheme, I use a limitedLinear scheme for dive(rho*phi,U), like for div(phi,k) and div(phi,omega). With those schemes, I have better results than with basic scheme. But with those scheme, when I have 2.6M cells, with LTSInterFoam, my calcul crash, that's why I use interFoam.

Finally, if the water must passes the domain 3xtimes, 100s is not enought (U=12.34m/s and the lenght of domain is 883m).

I'm going change the turbulent lenght and I and run the calcul during 215s to see if I have a better result.

regards
Vince

Hi Collin

So I change some values (turbulente intensity, turbulente length scale...) and I use a KomegaSST like turbulente model.

I modifie my mesh, now I have 2.6M of cells.

I run the calcul on 3 froude number and compare with experience. The total force is always under estimate (between 21.9% and 11.5%). But If I decompose the forces from the experience between viscous force (I use the ITTC57 formula) and wave resistance and I compare with pressure and viscous forces from OF, I note the pressure forces are very close (1.68% for Fr=0.28). However, viscous forces are really under estimate (67.45% for Fr=0.28!).

I assume I must add a layer (for the moment I don't arrive to have a correct layer for KCS) and may be increase the number of cells.

have you any idea to improve the results?

Last question, when the calcul run during a long time, it appear some wave (I join a picture) and the forces begin to split. What's wrong? My boundary conditions (wall on side and bottom, symmetry on the other side and classical inlet/outlet on enter face/exit face).

Regards
Vince

Hi Vince,

indeed the layers are important when it comes to viscous effects.
Did you run yPlusRAS on your mesh, and if so what are the results?

Concerning the incoming waves:
If the mesh is too small this leads to non-physical waves in the domain.
So I use a rather coarse mesh at the inlet to dampen out some
irregularities
Then as approaching the ship hull I gradually make the mesh more dense
and after that when the wake field gets uninteresting again I'm using again
a coarser mesh to dampen the waves and avoid reflection.

Another question that I have is, is the distance from your bow to the inlet
really that short? If so you might want to increase this distance , for
otherwise the ship might impair the inlet.

For the rest it is difficult to give you more hints, for i dont know the rest
of the settings you have.

Another hint I have is what I found just yesterday:
http://www.openfoamworkshop2013.org/...p?Main=2&sub=1

on this page you will find a paper:
Practical Application of OpenFOAM to Prediction of Hull Resistance
of some guys from Hyundai where they also describe some settings in OF
I'm about to compare my settings with theirs and see how it effects the
results.

regards
Colin

Hi Vince,

I've good experience with 1 length ahead of the ship, 3 astern, 2 aside, 1 below, 1/2 above. Further, integrate waves2foam into your solver and use the potentialCurrent condition to stabilise in- and outlet.
Good Luck
Hannes

Hi Colin and Hannes

Thanks for yours replies. I meshing with new dimension for blockMesh with different mesh density and the problem of incoming wave was solved. Now I try to add a layer but for the moment, I don't arrive on the KCS (if you have some suggestion...).

I read with lot of interest the paper "Pratical Application of OpenFOAM to predict hull resistance" present in the link gives by Colin. I have some question about this:

-he use for alpha divscheme a mHRIC, it's the first time I meet this scheme, and you?

-with LTSInterFoam, I believe it was impossible to have degree of freedom but he use DFBI (Dynamic fluid body interaction) module, it's an in-house modul developpe by HHI or it's present with the basic version of OF?

Regards
Vince