[SGWANG]

Hi guys,

I am struggling in the KCS hull resistance simulation for many weeks. I start with the DTCHull tutorials and the results are always about 10% bigger than the experimental data.

I tried to change the schemes and mesh following some threads and training materials of OpenFOAM workshop, the forces were always converged about 10% bigger, while many papers report some results with err less than 2%...

Attached is the mesh and force convergence line of half hull and whole hull... The hull is fixed and schemes and solutions follow the DTChull tutorial..

I compared the results with some papers and the err is mainly contributed by the viscous force component.

Does someone have an idea about this? I would appreciate it if someone could give some hints...

[Ship Designer]

Hi Shuguang,

I'm currently calculating the resistance of the KCS hull too, to validate my setup. I can tell you that your results are much closer than mine are. In my case, both the viscous and wave resistance are underestimated. My mesh is at ~2.2 mio cells. My wave pattern doesn't show diverging waves, which is unrealistic at Fr = 0.28. My model is fixed, not free to trim and sink. Bare hull with no appendages.

I have a few questions that might help me understand your case setup better:

- What tools did you use to make the mesh? blockMesh and snappyHexMesh or others?
- How many cells does your mesh have?
- At what Froude number are you calculating the resistance?
- Which model are you validating against? I'm using the MOERI case with Lpp ≈ 7.3 m.
- Are you calculating the bare hull or with appendages?
- Where did you find the experimental results? I could only find C_T plots in a graph (without exact figures) of a master thesis.

Maybe we can help eachother and find out what needs to be done to get results close to the experimental results. But more importantly understand why.

Cheers

[bennn]

Hi, here's my 2 cents input



your loads don't seem converged
mesh convergence is crucial here. Did you refine enough

y+ can be really important here. try and improve viscous layer maybe
ensure your schemes are accurate. second temporal order are required to reach a 10% accuracy (Backward)

[SGWANG]

Originally Posted by Ship Designer

Hi Shuguang,

I'm currently calculating the resistance of the KCS hull too, to validate my setup. I can tell you that your results are much closer than mine are. In my case, both the viscous and wave resistance are underestimated. My mesh is at ~2.2 mio cells. My wave pattern doesn't show diverging waves, which is unrealistic at Fr = 0.28. My model is fixed, not free to trim and sink. Bare hull with no appendages.

I have a few questions that might help me understand your case setup better:

- What tools did you use to make the mesh? blockMesh and snappyHexMesh or others?
- How many cells does your mesh have?
- At what Froude number are you calculating the resistance?
- Which model are you validating against? I'm using the MOERI case with Lpp ≈ 7.3 m.
- Are you calculating the bare hull or with appendages?
- Where did you find the experimental results? I could only find C_T plots in a graph (without exact figures) of a master thesis.

Maybe we can help eachother and find out what needs to be done to get results close to the experimental results. But more importantly understand why.

Cheers

Sorry for the late reply,

I studied the case2.1 & 2.3a in Gothenburg 2010. You could find the nice EFDs you want.

I use HEXPRESS, a very good mesh tool, to generate the mesh about 1.8M in total for the full ship (Lpp = 7.2786).

[SGWANG]

Originally Posted by bennn

Hi, here's my 2 cents input



your loads don't seem converged
mesh convergence is crucial here. Did you refine enough

y+ can be really important here. try and improve viscous layer maybe
ensure your schemes are accurate. second temporal order are required to reach a 10% accuracy (Backward)

Sorry for the late reply.

Since this is a famous case conducted by many papers and tutorials, I just follow the same mesh generation methods.

I also changed the boundary layer mesh, slightly changing the final results but still bigger.

Now I think it may be the turbulence model problem in multiphase condition. T tried to give a small initial value of k and omega. The results are better and err could be less than 4%. But still bad if compared with the CFD results in literature.

[mzzmrt]

There may be multiple paramaters to effect the accuracy of such a simulation.

It is well known that the standard RANS models have difficulties for capturing realistic (breaking or non-breaking) free surface wave phenomena by over-production of turbulence levels.

As a solution to this problem there are specially modified eddy-viscosity turbulence models which are called "stabilized" so by using a stabilized kOmegaSST model, your results may (or may not) improve.

[Ship Designer]

Hello Shuguang,

Thanks for the link. In the Gothenburg 2010 workshop you linked I can only find experimental data of the wave elevations, but not C_T or other resistance components. I'm comparing against the Tokyo 2015 workshop I now found. How do you conclude that your friction resistance is off? Have you calculated friction resistance according to ITTC '57 to compare against?

To check whether the problem is linked to the wall functions or turbulence parameters, you could try run the solution with turbulence off in turbulenceProperties and see, if that makes any difference.

Good luck

[SGWANG]

Originally Posted by mzzmrt

There may be multiple paramaters to effect the accuracy of such a simulation.

It is well known that the standard RANS models have difficulties for capturing realistic (breaking or non-breaking) free surface wave phenomena by over-production of turbulence levels.

As a solution to this problem there are specially modified eddy-viscosity turbulence models which are called "stabilized" so by using a stabilized kOmegaSST model, your results may (or may not) improve.

Thank you for your reply. I'll try and post if the results could be better!

[SGWANG]

Originally Posted by Ship Designer

Hello Shuguang,

Thanks for the link. In the Gothenburg 2010 workshop you linked I can only find experimental data of the wave elevations, but not C_T or other resistance components. I'm comparing against the Tokyo 2015 workshop I now found. How do you conclude that your friction resistance is off? Have you calculated friction resistance according to ITTC '57 to compare against?

To check whether the problem is linked to the wall functions or turbulence parameters, you could try run the solution with turbulence off in turbulenceProperties and see, if that makes any difference.

Good luck

Hello, Claudio.
Thank you for your suggestions and I'll try.
Since this is a benchmark case, you could find lots of good related papers including [1]. [2] [3] and so on.
Also, you could find the resistance results from some training and tutorials like [4]
I compared the results of different force component with the nice results they have shown...
Hope these would be helpful for you.

[Ship Designer]

Hello Shuguang,

thank you for the links you provided! After changing to a different type of mesh the wave making resistance of my KCS case got much closer to the experimental results. I use a graded mesh now made with blockMesh, with the smallest cell size at the bow, stern and the free surface. It looks more like yours now. It is inefficient though because it imposes small cell sizes where they are not needed and very high aspect ratio cells. But it has the advantage of not introducing the typical "hard spots" introduced by snappyHexMesh at the refinement level transisitions that disturb the correct formation of the waves (which are also present in the DTC Hull tutorial).

Using turbulence off has yielded excellent results for Fr = 0.28 but viscous resistance is largely overestimated for Fr = 0.22 with the same mesh. Good result might be just a coincidence then. I tried to add a boundary layer with snappyHexMesh but it is added only in some parts of the hull and it introduces again distortions even far from the hull and "hard" transitions near the free surface. I'll try to solve this, otherwise I'll have to abandon OpenFOAM's built-in meshing tools, since they appear to be not suitable for this type of application.

What I've noticed that might influence viscous resistance, is that at cells of the hull surface which are not hexahedrons, the values of k and omega are different than in the vicinity, i.e. their values are heterogenous over the hull surface, see "stripes" in images. I wonder whether this is due to the different cell shape that calculates cell values differently or whether it is misrepresented in ParaView. Does this happen to you as well? Is this normal?

I'm afraid I have no other suggestions for you at this moment.

Cheers

[SGWANG]

Originally Posted by Ship Designer

Hello Shuguang,

thank you for the links you provided! After changing to a different type of mesh the wave making resistance of my KCS case got much closer to the experimental results. I use a graded mesh now made with blockMesh, with the smallest cell size at the bow, stern and the free surface. It looks more like yours now. It is inefficient though because it imposes small cell sizes where they are not needed and very high aspect ratio cells. But it has the advantage of not introducing the typical "hard spots" introduced by snappyHexMesh at the refinement level transisitions that disturb the correct formation of the waves (which are also present in the DTC Hull tutorial).

Using turbulence off has yielded excellent results for Fr = 0.28 but viscous resistance is largely overestimated for Fr = 0.22 with the same mesh. Good result might be just a coincidence then. I tried to add a boundary layer with snappyHexMesh but it is added only in some parts of the hull and it introduces again distortions even far from the hull and "hard" transitions near the free surface. I'll try to solve this, otherwise I'll have to abandon OpenFOAM's built-in meshing tools, since they appear to be not suitable for this type of application.

What I've noticed that might influence viscous resistance, is that at cells of the hull surface which are not hexahedrons, the values of k and omega are different than in the vicinity, i.e. their values are heterogenous over the hull surface, see "stripes" in images. I wonder whether this is due to the different cell shape that calculates cell values differently or whether it is misrepresented in ParaView. Does this happen to you as well? Is this normal?

I'm afraid I have no other suggestions for you at this moment.

Cheers

Hello, Claudio

I have no idea about the "stripes" behaviour of k and omega. Mine is different as shown in the figure.

I think the reason for the over-predicted resistance may be due to the usage of nutkRoughWallFuction for nut in the OpenFOAM tutorial DTCHull. This would account for roughness effects. I changed to nutkWallFunction like the OpenFOAM workshop training materials. Results are better now.

I also tried the stabilized turbulence model, the results could be more stable and better but it's not the critical reason for this problem I think. I cannot show the results using the modified model because it's developed by others.

[Ship Designer]

Hello Shuguang,

it looks like your results are very close to where they should be, well done! Thanks for the picture you've posted. I see there are no such stripes, I presume your mesh quality is better than mine. I'll try making the mesh with cfMesh now and see if it brings an improvement.

Cheers

[Richal Sun]

Originally Posted by Ship Designer

Hi Shuguang,

I'm currently calculating the resistance of the KCS hull too, to validate my setup. I can tell you that your results are much closer than mine are. In my case, both the viscous and wave resistance are underestimated. My mesh is at ~2.2 mio cells. My wave pattern doesn't show diverging waves, which is unrealistic at Fr = 0.28. My model is fixed, not free to trim and sink. Bare hull with no appendages.

I have a few questions that might help me understand your case setup better:

- What tools did you use to make the mesh? blockMesh and snappyHexMesh or others?
- How many cells does your mesh have?
- At what Froude number are you calculating the resistance?
- Which model are you validating against? I'm using the MOERI case with Lpp ≈ 7.3 m.
- Are you calculating the bare hull or with appendages?
- Where did you find the experimental results? I could only find C_T plots in a graph (without exact figures) of a master thesis.

Maybe we can help eachother and find out what needs to be done to get results close to the experimental results. But more importantly understand why.

Cheers

Hi Claudio,
I've been stuck on this question for two weeks.I'm in the same situation as you.The viscous component is seriously underestimated. I refer to the results of simulation employed star CCM+ by my colleagues and find that the viscosity component is underestimated by 25%.On the basis of blockmesh, the mesh is encrypted many times by refinemesh. Bow, stern and moonpool area i concerned about are locally refined.The boundary layer is generated by absolute size of snappyHexmesh. The height of the first boundary layer cell is about 1.3mm.The coverage of boundary layer is more than 90%.By the way, the turbulence model is k-omega SST. However, the viscous component is still seriously underestimated.I don't know what else to adjust,Any suggestions？
Looking forward to your reply.

[isulovsky]

Dear foamers,

Regarding the KCS resistance case, I have been dealing with it a last month or so. My main problem is also overpredicted resistance but by a much larger scale. Values of force in X direction are always somewhere in beetween 250-300N which is not even close to experimental data (around 40N). I am well aware that my mesh is not perfect, free surface is not anisotropicaly refined in the whole domain and the boundary layers are also not perfect. I doubt that the mesh is that bad that will produce so bad results so I need a second opinion from you guys. Every boundary condition, turbulence model is the same as in DTChull tutorial only the velocity is set to 2.169 m/s. I am also noticing high intial residuals for p_rgh which I presume can be a hint for badly setup simulation but I cannot figure out what to change. Photos are in the attachment , Thank You in advance.

Ivan

[Ship Designer]

Hi Jayiu, please accept my apologies for my late response as I've been very busy with work recently. How did you manage to get viscous layers via absolute size with snappyHexMesh? I never managed to accomplish that… Could you please provide close-up pictures of the viscous layers? I'm curious how they look like in your mesh.

One thing you could do is to check the y+ values of the hull patch by using the yplus function object. That should show whether your viscous layers are resolved enough for the wall functions to work properly.

Cheers, Claudio

[Ship Designer]

Hi Ivan, on first sight I believe your mesh might be the cause. Having a fine mesh resolution of the free surface — especially in the vertical direction — is essential for the waves to be calculated properly. I recommend at least 16 cells above the still water line to the highest wave crest and at least 8 from still water line to the deepest trough. Transition above and below should be gradual with cell height growth of max. 1.2. Try to keep the mesh below the surface reasonably fine because that's where the pressure gradients of the waves are substantial. If the pressure field beneath the waves is not well resolved, the pressure forces will be wrong as well.

Using the DTC hull tutorial as a starting point is okay, however I caution you that the mesh it uses is not a good one in my opinion. It's very coarse and with abrupt cell size transitions. It works well for the viscous resistance though, because the cell size around the hull patch is constant and that's why snappyHexMesh is able to create reasonably good viscous layers. The tutorial calculates resistance for the highest Froude number published in the original DTC paper and the results match virtually exactly. However, if you pick a lower Froude number, you'll find that the wave resistance component gets way off. The mesh is too coarse to capture the wave pattern well, especially at lower Froude numbers where the waves get shorter and the pressure gradients less deep.

The residuals you're seeing might be high or low, but that depends also on your solver settings, how many correctors you use etc. In my experience, the residuals alone don't tell much about the progress of the computation, also bearing in mind that this type of free surface simulation is transient. Approx. 80% of the solution time is spent creating and eventually stabilize the wave pattern, during which the residuals may go up and down. I find it more insightful to use the fieldMinMax function Object and output e.g. every 10 time steps all relevant field values. As long as they are within typical values for the case at hand, the computation should converge without problems. You can keep an eye on U knowing the hull velocity you chose for your case and p_rgh by calculating the stagnation pressure based on initial U. The max. value of p_rgh should be close to that figure at the bulbous bow but not higher, whereas the min. value is often around -0.5 times the max. value. If you see the order of magnitude for p_rgh changing for several time steps, that's usually an indicator of divergence which might not necessarily be reflected by the residuals.

If I find time over the holidays I can set up a case for the KCS with the mesh I'm using and share it here. It would be an interesting validation exercise I believe. Can you tell me please which experimental results you're using? I haven't found a publication with the experimental results for the fixed hull without rudder.

Cheers, Claudio

[Richal Sun]

Originally Posted by Ship Designer

Hi Jayiu, please accept my apologies for my late response as I've been very busy with work recently. How did you manage to get viscous layers via absolute size with snappyHexMesh? I never managed to accomplish that… Could you please provide close-up pictures of the viscous layers? I'm curious how they look like in your mesh.

One thing you could do is to check the y+ values of the hull patch by using the yplus function object. That should show whether your viscous layers are resolved enough for the wall functions to work properly.

Cheers, Claudio

Hi Claudio,
Thank you for your suggestions, due to the wall function implement in the vicinity of hull surface, y+ can be ensured in the scope of 30-300 in most areas of hull surface.But viscous component is still underestimated. Eventually，i changed nutkWallFunction to nutkRoughWallFunction and it does work.The first boundary layer height can be controlled by addLayersControls in SnappyHexMeshDict, just set relativeSize false and firstLayerThickness as value you expected and it can be obtained.The partial Fig is attached.
Best regards.
Jiayu

[isulovsky]

Originally Posted by Ship Designer

Hi Ivan, on first sight I believe your mesh might be the cause. Having a fine mesh resolution of the free surface — especially in the vertical direction — is essential for the waves to be calculated properly. I recommend at least 16 cells above the still water line to the highest wave crest and at least 8 from still water line to the deepest trough. Transition above and below should be gradual with cell height growth of max. 1.2. Try to keep the mesh below the surface reasonably fine because that's where the pressure gradients of the waves are substantial. If the pressure field beneath the waves is not well resolved, the pressure forces will be wrong as well.

Using the DTC hull tutorial as a starting point is okay, however I caution you that the mesh it uses is not a good one in my opinion. It's very coarse and with abrupt cell size transitions. It works well for the viscous resistance though, because the cell size around the hull patch is constant and that's why snappyHexMesh is able to create reasonably good viscous layers. The tutorial calculates resistance for the highest Froude number published in the original DTC paper and the results match virtually exactly. However, if you pick a lower Froude number, you'll find that the wave resistance component gets way off. The mesh is too coarse to capture the wave pattern well, especially at lower Froude numbers where the waves get shorter and the pressure gradients less deep.

The residuals you're seeing might be high or low, but that depends also on your solver settings, how many correctors you use etc. In my experience, the residuals alone don't tell much about the progress of the computation, also bearing in mind that this type of free surface simulation is transient. Approx. 80% of the solution time is spent creating and eventually stabilize the wave pattern, during which the residuals may go up and down. I find it more insightful to use the fieldMinMax function Object and output e.g. every 10 time steps all relevant field values. As long as they are within typical values for the case at hand, the computation should converge without problems. You can keep an eye on U knowing the hull velocity you chose for your case and p_rgh by calculating the stagnation pressure based on initial U. The max. value of p_rgh should be close to that figure at the bulbous bow but not higher, whereas the min. value is often around -0.5 times the max. value. If you see the order of magnitude for p_rgh changing for several time steps, that's usually an indicator of divergence which might not necessarily be reflected by the residuals.

If I find time over the holidays I can set up a case for the KCS with the mesh I'm using and share it here. It would be an interesting validation exercise I believe. Can you tell me please which experimental results you're using? I haven't found a publication with the experimental results for the fixed hull without rudder.

Cheers, Claudio

Claudio,

Sorry for the delay of my response. I have solved this problem and the main thing was the anisotropic refinement of the free surface, just as You have said. Using interFoam solver for this type of analysis it is crucial to refine it so the alpha can converge. Regarding experimental data here is the link:
https://t2015.nmri.go.jp/Instruction...ction_KCS.html

My results now have around 2% deviation from the EFD, except for the highest speed where the error is around 6%.

Regards,

Ivan