[mAlletto]

Since openfoam.com recently released the chimera or overset mesh capability, I was wondering if there are already some validation attempts ongoing.


Are there any standard simple test cases which are usually used for the validation of chimera application. Are there good experimental data out there that can be trusted?


I'm rather new in this topic and I sow that there was no thread regarding this application so I thought to open one.


Best


Michael

[mAlletto]

Just out of curiosity I made a small tutorial which consists in a moving squared cylinder in a closed pipe. It seams to work but I have no clue if the results obtained are correct.


I'll attach i hear just in case someone is interested in . It works with OF17.12

[mAlletto]

I basically try to follow the list of testcases in Simulating flows with moving rigid boundary using immersed-boundary method, Liao et al 2009.


The first test case is an oscillating cylinder in a fluid at rest. The flow is laminar. The scope is to check if the overset grid can capture the forces exerted by the cylinder on the fluid an of the resulting velocities are correct.


For this simple testcase the two quantities are in good agreement with the experiments cited in the above paper.



Find attached the tutorial I created to this test case.

[mAlletto]

The second test case I tried is an inline oscillating cylinder in a constant inflow. First I computed the case where the cylinder is a rest and compared the lift and drag coefficients with the reference inside the paper I cited. The agreement is good.



After that I computed the shedding frequency and let the cylinder oscillate with a frequency twice the shedding frequency (actually also one and four times) and for a frequency twice the shedding frequency of the lift coefficient tripled with respect to the other cases. This is in good agreement with the results of the above cited paper and also the references provided therein.


Find attached the cases.

[mAlletto]

The third test case is a sphere settling onto the influence of gravity in a fluid at rest. For this I used the 6Dof solver. Since the hydrostatic pressure is not considered in overpimpledymfoam I reduced the mass of the sphere in order the the weight is equal to the weight of the original case minus the buoyancy force.



Unfortunately I had to use a very low maximum Co number (0.01) to get the case working. with higher values i had a lot of oscillations in the velocity of the settling sphere. If someone has a hint how to increase the time step it would be very nice.



Ah and i downloaded the snappyHexmeshdict to generate the mesh around the sphere from this forum. Unfortunately I do not remember where I got it.

[mAlletto]

Just wanted to report that by underrelaxing the acceleration much bigger time steps were possible. Probably the coupling between the fluid solver and the displacement solver is too loose to allow bigger timestps

[canik01@yahoo.com]

Dear Michael,

Thank you for posting sphereSettling example. I have tried that on Windows but could not succeeded. Do you have Windows version of that without errors?

Best regards,

Senel

[mAlletto]

Did you try to download it from here https://wiki.openfoam.com/Settling_S...ichael_Alletto

[canik01@yahoo.com]

I tried this link. It works fine. Thank you very much for this usefull and nice study. I have couple of questions:

What is the fluid? How do you define it? For example, for the water, which parameters must be set?

Can we give initial velocity?
velocity (0.001 0 0);// 0.001 m/s in X direction

[mAlletto]

Usually a fluid is defined by its density and viscosity. Yes you can give an initial velocity

[canik01@yahoo.com]

There are three files containing rho values:

1) dynamicMeshDict: I assume this rho=970 is for sphere, not for the fluid.

2) transportProperties: rho=970 sphere or fluid?

3) controlDict: rho=970 is for sphere I think.

Would you please advice?

[mAlletto]

This is the fluid density. The one of the sphere is 1120 kg / m3

[hbulus]

Originally Posted by mAlletto

The third test case is a sphere settling onto the influence of gravity in a fluid at rest. For this I used the 6Dof solver. Since the hydrostatic pressure is not considered in overpimpledymfoam I reduced the mass of the sphere in order the the weight is equal to the weight of the original case minus the buoyancy force.



Unfortunately I had to use a very low maximum Co number (0.01) to get the case working. with higher values i had a lot of oscillations in the velocity of the settling sphere. If someone has a hint how to increase the time step it would be very nice.



Ah and i downloaded the snappyHexmeshdict to generate the mesh around the sphere from this forum. Unfortunately I do not remember where I got it.

Hello mAlletto,

I worked on your cases, thanks for this great tutorials. However, i am curios about why you didn't prefer to first get a steady solution than begin to move sphere ? Maybe with this way you can get good agreements for higher Re.

When i work on Fluent, i always get a steady overset solution than start to move. In openfoam, there are steady state overset solvers.

My second concern is about how you define zones. To define c0, do you get a point from outside of the refinement zone ? I tried to view on paraview, but i cant open it with openfoam reader, there i cant view the zones. How are you be sure zones are defined as correct in your works ?

[mAlletto]

Hm in the experiment the sphere is released from rest. So if one wants to reproduce the experiment the simulation setup should be as close as possible

[hbulus]

Originally Posted by mAlletto

Hm in the experiment the sphere is released from rest. So if one wants to reproduce the experiment the simulation setup should be as close as possible

I think you misunderstood me. What i am saying is that first get a steady state solution, then start the simulation which is falling of sphere from rest. In that way, some stiffness in equations can be reduced.

Did you ever tried such a way while working on dynamic meshs?

[mAlletto]

If the sphere is at rest, than the fluid is also at rest. This is how I initialized the solution

[mAlletto]

In this tutorial I initialized the solution of the dynamic mesh case with a stationary solution https://wiki.openfoam.com/Dynamic_st...ichael_Alletto

[hbulus]

Originally Posted by mAlletto

If the sphere is at rest, than the fluid is also at rest. This is how I initialized the solution

Yeap you are right to model real case exactly you should do that. But for higher Re, stiffness of equations increase and linear solvers cant handle with them. To handle it, it can be good idea to get steady solution first. If you dont agree, i ll be glad if you explain .

I try to fall sphere under flight conditions of 1e7 Re and AOA 5 degree. I am using fully tetrahedral meshes. When i try to get steady state solution with overRhoSimpleFoam, pressure solver blow ups at second steady time step. When i tried to solve directly with overRhoPimpleDyFoam (after initializing with potentialFoam), it blows up after many iterations. My question is that what would you choose to follow for this case; 1. initialize with potentialFoam and start to move mesh overRhoPimpleDyFoam 2. get a steady solution, then after initialization go with overRhoPimpleDyFoam 3. other ways

I really need help and i am not sure how to approach this case and insist on with.

[mAlletto]

Use a lot of outer iterations and small time steps. I experienced convergence issues with fully thetraedra meshes

[govind_IITD]

Hi,


I am wondering where sphere's density is define exactly. I see that, in dynamicMeshDict:
rho rhoInf;
rhoInf 970;


Which one is for solid and which one is for fluid? I couldn't find 1120 kg/m^3 of solid. If I can change solid density then it would be easy to generate settling of various Re without any need to change other parameters of fluid.




Visualization:

How do I make the solid body to move in paraviw? I







Govind