[musahossein]

Can anyone tell me what the difference between sloshingTank3D and sloshingTank3D3DoF is? Does the "3DoF" mean movement in the principal x,y and z directions? If that is the case, the what does sloshingTank3D do?

Thankyou

Musa

[musahossein]

Bruno:
I have question. To your knowledge, what is the difference between solshingTank3D and solshingTank3D3DoF? Both are in the interDyMFOAM solver. I cannot find documentation for either one. I would suspect that sloshingTank3D permits you to model a tank in 3 dimension, but has 2 degrees of freedom - much like sloshingTank2D. On the other hand, sloshingTank3D3DoF permits one to model a 3D tank and computes displacement along 3 principal axes. Is that a correct assumption?
I look forward to your response. Thanks
Musa

[wyldckat]

Greetings Musaddeque,

I've moved your first post to here to the OpenFOAM forum and the second post from this thread: http://www.cfd-online.com/Forums/ope...ntroldict.html

AFAIK, there is no detailed documentation about these tutorials. But they should be self-explanatory.

You can easily compare the tutorial cases by running:

cd $FOAM_TUTORIALS/multiphase/interDyMFoam/ras
diff -Nur sloshingTank2D sloshingTank2D3DoF

diff -Nur sloshingTank2D sloshingTank3D

diff -Nur sloshingTank3D sloshingTank3D3DoF

diff -Nur sloshingTank3D3DoF sloshingTank3D6DoF

Running them and then seeing them in ParaView will also show you the differences.

• 3DoF stands for 3 Degrees of Freedom.
• 6DoF stands for 6 Degrees of Freedom.

As far as I can see, the main difference between sloshingTank3D vs sloshingTank3D3DoF is that the sloshing intensity is different between the two simulations, which also leads to the need to change the "deltaT" in "controlDict".

As for the cases 3DoF vs 6DoF, the main difference between the two is the use of "SDA" vs "tabulated6DoFMotion". The curious detail is that the 6DoF used in the past the "SKA" which was replaced by "tabulated6DoFMotion" in OpenFOAM 2.0: http://www.openfoam.org/mantisbt/view.php?id=325

Best regards,
Bruno

[musahossein]

Originally Posted by wyldckat

Greetings Musaddeque,

I've moved your first post to here to the OpenFOAM forum and the second post from this thread: http://www.cfd-online.com/Forums/ope...ntroldict.html

AFAIK, there is no detailed documentation about these tutorials. But they should be self-explanatory.

You can easily compare the tutorial cases by running:

cd $FOAM_TUTORIALS/multiphase/interDyMFoam/ras
diff -Nur sloshingTank2D sloshingTank2D3DoF

diff -Nur sloshingTank2D sloshingTank3D

diff -Nur sloshingTank3D sloshingTank3D3DoF

diff -Nur sloshingTank3D3DoF sloshingTank3D6DoF

Running them and then seeing them in ParaView will also show you the differences.

• 3DoF stands for 3 Degrees of Freedom.
• 6DoF stands for 6 Degrees of Freedom.

As far as I can see, the main difference between sloshingTank3D vs sloshingTank3D3DoF is that the sloshing intensity is different between the two simulations, which also leads to the need to change the "deltaT" in "controlDict".

As for the cases 3DoF vs 6DoF, the main difference between the two is the use of "SDA" vs "tabulated6DoFMotion". The curious detail is that the 6DoF used in the past the "SKA" which was replaced by "tabulated6DoFMotion" in OpenFOAM 2.0: http://www.openfoam.org/mantisbt/view.php?id=325

Best regards,
Bruno

Thankyou very much for your response. My confusion is however, that if 3DoF is for three degree of freedom, then is sloshingTank3D a case of a 3D tank thank that has only 2 degree of freedom, since there is no "3DoF" appended to the "3D"? In my case I dont need 3 degree of freedom. Motion in 2 degrees (x, y or y, z which ever way you define the axis), I need to be able to define a tank in 3 dimensions. Please let me know and as always thanks for your help!!
Musa

[wyldckat]

I wrote this:

Originally Posted by wyldckat

As far as I can see, the main difference between sloshingTank3D vs sloshingTank3D3DoF is that the sloshing intensity is different between the two simulations, which also leads to the need to change the "deltaT" in "controlDict".

Here are the differences:

diff -Nur sloshingTank3D/constant/dynamicMeshDict sloshingTank3D3DoF/constant/dynamicMeshDict
--- sloshingTank3D/constant/dynamicMeshDict     2014-08-14 16:43:10.573409120 +0100
+++ sloshingTank3D3DoF/constant/dynamicMeshDict 2014-08-14 16:43:10.673409123 +0100
@@ -24,14 +24,14 @@
     {
         CofG            ( 0 0 0 );
         lamda           50;
-        rollAmax        0.22654;
-        rollAmin        0.10472;
-        heaveA          3.79;
-        swayA           2.34;
+        rollAmax        0.2;
+        rollAmin        0.1;
+        heaveA          4;
+        swayA           2.4;
         Q               2;
-        Tp              13.93;
-        Tpn             11.93;
-        dTi             0.059;
+        Tp              14;
+        Tpn             12;
+        dTi             0.06;
         dTp             -0.001;
     }
 }

The values of the parameters for the SDA are slightly different. As far as I can see, the motions are greater in one case than the other.

diff -Nur sloshingTank3D/system/controlDict sloshingTank3D3DoF/system/controlDict
--- sloshingTank3D/system/controlDict   2014-08-14 16:43:10.565409119 +0100
+++ sloshingTank3D3DoF/system/controlDict       2014-08-14 16:43:10.665409123 +0100
@@ -25,7 +25,7 @@
 
 endTime         40;
 
-deltaT          0.05;
+deltaT          0.01;
 
 writeControl    adjustableRunTime;

The 3DoF case requires a finer time step, at least at the start. This would imply that the sloshing is more intense in this case.

The sloshingTank3D is also a 3DoF case.
I believe your difficulty here is that you have not yet studied what SDA is exactly: https://github.com/OpenFOAM/OpenFOAM...ions/SDA/SDA.H

    Ship design analysis (SDA) 3DoF motion function.

    Comprising sinusoidal roll (rotation about x), heave (z-translation)
    and sway (y-translation) motions with changing amplitude and phase.

The 6DoF is a general implementation that allows for any degrees of freedom, including restraining 5 of those degrees if necessary!

[musahossein]

Bruno:

Thanks again for your response. I did study SDA as well as the SKA codes that seems to be a part of the 3D3dof and 6d6dof cases. Out of curiosity I put the equations in a spreadsheet to see what the SDA actually does. However, I am not going to use SDA, but give discrete displacement to the tank in 3D which I have done with success in the 2D case, in the form of back and forth horizontal motion, where the total motion will be at the most 10 cm. I ran both the cases, but could not tell whether both these cases sloshingtank3d and sloshingtank3dof would support 3 degrees of freedom or not. I cannot tell. From your response it appears that 3d would be good for translation in one direction, whereas 3d3dof would be suitable for translation in three direction. Translation being defined in my case as pure horizontal motion without any rotation about any of the axes. I hope that makes sense.

-------------

Also, may I suggest that the sloshing tank cases in 2d and 3d be eliminated in favor of the 6dof one, since one can turn of the motion or axes one does not need. Even 2d is solving a restricted 3d case. Just a suggestion.

[wyldckat]

• SDA stands for Ship Design Analysis 3DoF motion function
• SKA stands for Sea Keeping Analysis 6DoF motion function - https://github.com/OpenCFD/OpenFOAM-...ions/SKA/SKA.H

The two exist because they were designed for 2 different analysis.

Originally Posted by musahossein

Also, may I suggest that the sloshing tank cases in 2d and 3d be eliminated in favor of the 6dof one, since one can turn of the motion or axes one does not need. Even 2d is solving a restricted 3d case. Just a suggestion.

If I understood you correctly, what you're advocating is the elimination of a feature that apparently comes in handy for people that need to do SDA.

Please do keep in mind that just because it's a bit confusing for you and because these cases might seem redundant, it's actually an extremely important lesson that is taught with these 4 very similar cases! It shows that the smallest detail can result in having to make several adjustments in the right places, in order to still achieve correct results!

[musahossein]

Originally Posted by wyldckat

• SDA stands for Ship Design Analysis 3DoF motion function
• SKA stands for Sea Keeping Analysis 6DoF motion function - https://github.com/OpenCFD/OpenFOAM-...ions/SKA/SKA.H

The two exist because they were designed for 2 different analysis.


If I understood you correctly, what you're advocating is the elimination of a feature that apparently comes in handy for people that need to do SDA.

Please do keep in mind that just because it's a bit confusing for you and because these cases might seem redundant, it's actually an extremely important lesson that is taught with these 4 very similar cases! It shows that the smallest detail can result in having to make several adjustments in the right places, in order to still achieve correct results!

Well not exactly. What I would propose that there be only one sloshingTank6DoF case. Since this case examines all 6 degrees of freedom it is the maximum case. Cases with reduced degree of freedom can be run by setting the unused degree of freedom to zero -- the user can "collapse" the degree of freedom that are not required. The SDA and SKA are axis specific. So you can still do SDA and SKA. As I understand it, the 2D sloshing tank case is a restricted case with the tank thickness made very small to simulate two dimensions. I think having so many variations of the same thing (sloshingTank2D, SloshingTank2D3DoF, SolshingTank3D, SloshingTank3DoF, SolshingTank6Dof etc) can create confusion as to which is more appropriate for the problem at hand. -- Just a thought I felt I should share.

[wyldckat]

Originally Posted by musahossein

Just a thought I felt I should share.

Well... I don't agree with your point of view on this, although I do understand the need to keep things simple... problem is that "keeping things simple" is not always the best approach.

Anyway, if you feel strong about this, feel free to report this on the official bug tracker for OpenFOAM: http://www.openfoam.org/bugs/ - the people on the official development team are the ones who have power to get that changed. I'm only a user part of the community that uses OpenFOAM technology.

[musahossein]

Originally Posted by wyldckat

Well... I don't agree with your point of view on this, although I do understand the need to keep things simple... problem is that "keeping things simple" is not always the best approach.

Anyway, if you feel strong about this, feel free to report this on the official bug tracker for OpenFOAM: http://www.openfoam.org/bugs/ - the people on the official development team are the ones who have power to get that changed. I'm only a user part of the community that uses OpenFOAM technology.

I think you are right. I looked at SDA and SKA and understood the need to have all these variations.

[musahossein]

As I compare sloshingtank2d and 3d, I noted that in the blockMeshDict, in sloshingtank2d, the front and back patches are described as empty. In the 3d, it is not. is this what differentiates between the 2d and 3d?. If that is the case, can I edit the blockMeshDict in 2d so that the front and back are not empty and run it as a 3d case?

[wyldckat]

Quick answer: OpenFOAM User Guide, sub-section "2.1.1.1 Mesh generation": http://www.openfoam.org/docs/user/cavity.php

[musahossein]

I thought so!. So essentially, all these variations 2d,3d, 3dof,3d6dof, are one and the same with necessary adjustments to turn of DOF's that are not needed.

[musahossein]

Originally Posted by wyldckat

Quick answer: OpenFOAM User Guide, sub-section "2.1.1.1 Mesh generation": http://www.openfoam.org/docs/user/cavity.php

I have a question on the difference between using a patch or wall when modeling a tank that only has horizontal motion (front and back patch are empty), fluid pressure is only on the left and right wall. The tank is like a rectangular box open to the atmosphere. The walls are assumed to be rigid and do not flex. And the tank is subject to back and forth horizontal motion only. Some tell me that for such a simple case it does not matter. But I see in cavity foam example the patch wall has been used. Should then wall be used to be "proper"? or is it an absolute necissity to ensure correct boundary conditions? If this question sounds sill, please accept my apologies.

Thankyou.

[musahossein]

Originally Posted by wyldckat

Quick answer: OpenFOAM User Guide, sub-section "2.1.1.1 Mesh generation": http://www.openfoam.org/docs/user/cavity.php

I am running a case in OpenFOAM sloshingTank2D. The tank is 2m long, 0.1m deep and fluid depth is 0.8m. I am supplying discrete displacements to OpenFOAM to calculate the wall forces on the left and right wall. After several iterations, the wall forces are huge, and the tank literally files of the grid. My question is, how is that possible. With only 0.8m of fluid in a tank that is only 0.1m deep (measured in and out of the paper), the force generated will be very small. Appended is an snipped of the displacement sent to openfoam and the force returned. The magnitude is unbeliviele considerin only 0.8m of fluid is in the tank. The inertia force from TLD is the force read from OpenFOAM. The wall pressures are calculated using libforces.so in controlDict, and the values are stored in sloshingTank2D/postprocessing/forces/ dir in each time folder.
================================================== ==
Iteration number 12 Time Count 0.2400 Acceleration -0.9961646
Story Force (kg) Inertia Force (kg) Adjusted Force (kg):
-0.39846584E+01 -0.62075402E+04 -0.62115249E+04
Transformed force vector is as follows
0.30908440E+04
-0.30405180E+03
DOF Structure displacement (m), velocity (m/sec), acceleration (m/sec^2)
2 -.90003217E+000 -.29679854E+002 -.61926779E+003
OpenFoam analysis start time(seconds), end time(seconds), starting displacement(m), end displacement(m)
0.24000000E+000 0.26000000E+000 0.44445424E+000 -.90003217E+000
Inertia force from TLD0.95264404E+005kg
OpenFoamstart_displacement 0.44445423667291778
OpenFoamend_displacement -0.90003216825813903
================================================== ==

The image of the tank flying of into space is attached. Can anyone help? Is some setting possibly wrong somewhere?

[wyldckat]

Greetings musahossein,

Originally Posted by musahossein

I have a question on the difference between using a patch or wall when modeling a tank that only has horizontal motion (front and back patch are empty), fluid pressure is only on the left and right wall. The tank is like a rectangular box open to the atmosphere. The walls are assumed to be rigid and do not flex. And the tank is subject to back and forth horizontal motion only. Some tell me that for such a simple case it does not matter. But I see in cavity foam example the patch wall has been used. Should then wall be used to be "proper"? or is it an absolute necissity to ensure correct boundary conditions? If this question sounds sill, please accept my apologies.

The difference between "walls" and "patches" is that walls are strictly for boundaries that need conditions specific to walls. For example: turbulence wall treatment and "moving wall".

Originally Posted by musahossein

I am running a case in OpenFOAM sloshingTank2D. The tank is 2m long, 0.1m deep and fluid depth is 0.8m. I am supplying discrete displacements to OpenFOAM to calculate the wall forces on the left and right wall. After several iterations, the wall forces are huge, and the tank literally files of the grid. My question is, how is that possible. With only 0.8m of fluid in a tank that is only 0.1m deep (measured in and out of the paper), the force generated will be very small. Appended is an snipped of the displacement sent to openfoam and the force returned. The magnitude is unbeliviele considerin only 0.8m of fluid is in the tank. The inertia force from TLD is the force read from OpenFOAM. The wall pressures are calculated using libforces.so in controlDict, and the values are stored in sloshingTank2D/postprocessing/forces/ dir in each time folder.
================================================== ==
Iteration number 12 Time Count 0.2400 Acceleration -0.9961646
Story Force (kg) Inertia Force (kg) Adjusted Force (kg):
-0.39846584E+01 -0.62075402E+04 -0.62115249E+04
Transformed force vector is as follows
0.30908440E+04
-0.30405180E+03
DOF Structure displacement (m), velocity (m/sec), acceleration (m/sec^2)
2 -.90003217E+000 -.29679854E+002 -.61926779E+003
OpenFoam analysis start time(seconds), end time(seconds), starting displacement(m), end displacement(m)
0.24000000E+000 0.26000000E+000 0.44445424E+000 -.90003217E+000
Inertia force from TLD0.95264404E+005kg
OpenFoamstart_displacement 0.44445423667291778
OpenFoamend_displacement -0.90003216825813903
================================================== ==

The image of the tank flying of into space is attached. Can anyone help? Is some setting possibly wrong somewhere?

Advice: If you do not know the depth of a pool, you should not jump from 50 metre high in the air into the pool.

This to say that you're probably trying to do something that you do not have yet the skills to do, because you're jumping directly into the final simulation you want to do. If you were using "commercial" CFD software, you probably would have already solved this problem. Since you're using OpenFOAM... well, you're jumping to a pool for which you don't know the depth, therefore you should first go to the pool and check/measure how deep it is. In other words: http://openfoamwiki.net/index.php/Tu...#State_of_Mind

2. Complexity is in the eye of the beholder - This to say that you should never - not ever - try to solve your final problem directly... at least not until you've gained enough experience.

• And experience can only be gained if you start with one or more very simple example cases and then gradually add complexity, one detail at a time.

Originally Posted by musahossein

I am dealing with a bizzare OpenFoam problem where the pressure forces grows out of bounds. If I have a small tank of water say L=2m, D=0.1m and water level h=0.8m, then regardless of how hard and fast I push it, the computed pressure cannot increase out of bounds. But this has happened. I posted it in the forum hoping to get an opinion. Does OpenFOAM allow numerical simulations grow without bounds?

There are only a few items in the OpenFOAM dictionaries that one can adjust, would they be responsible?

Quoting again: http://openfoamwiki.net/index.php/Tu...#State_of_Mind

4. Every single detail matters more than you're likely willing to care about. This will be exemplified in the next section Common mistakes.

Last but not least: choose your questions wisely, both when trying to ask OpenFOAM what's the solution to your problems, and when asking here on the forum. Because answers here on the forum can take any time from 1 minute to 2 or 4 years, if not more.
In addition: OpenFOAM can answer small questions very easily. Here on the forum the same does not apply, i.e. people don't have enough time to answer everyone.

Good luck! Best regards,
Bruno

[Ron de Vos]

After the research of the resistance of the windship. I want to study the seakeeping motions of the ship . With witch tutorial is the beste way to start?

[wyldckat]

Originally Posted by Ron de Vos

After the research of the resistance of the windship. I want to study the seakeeping motions of the ship . With witch tutorial is the beste way to start?

Quick answer: Study the tutorial "$FOAM_TUTORIALS/multiphase/interDyMFoam/ras/sloshingTank3D6DoF"

[Ron de Vos]

I want to ask how I get a hull (stl) in a sloshing tank?
Ron

[wyldckat]

Quick answer: Please check the following tutorials for ideas:

• incompressible/pimpleDyMFoam/movingCone - simple example of empty object moving inside mesh in 2D.
• multiphase/interDyMFoam/ras/floatingObject - more complex example of a floating body in a multiphase environment.