[danielparmar]

Dear all CFD community,

I recently started working on a project related to FSI of flexible wings. I am using turekHron fsi case from solids4foam. Since for flexible wing, atmospheric conditions are needed. Thus, I changed the boundary conditions in U directory to freestream (inlet,top,bottom patches) at 1.5 ms-1,the simulation runs perfectly(considering default fluid and solid-material properties).

But as soon as change the fluid properties to air (rho-1.23, nu 1.47e-5) and solid material properties of polyethylene foam (rho 32.9, poisson ratio 0.2, E-0.849e+5) keeping freestream conditions the solution crashes after 2 seconds, showing run time error.

I would be glad if you all can tell me is there anything else I need to consider to look at changing along with these porperties that leads to smooth.

log file :
https://drive.google.com/file/d/1wiC...ew?usp=sharing

[bigphil]

Hi Daniel,

One thing to note is that in the HronTurek example cases in solids4foam, the FSI coupling is enabled at 2 seconds; this is done to allow the flow to develop first before enabling the coupling. If you are using the same settings then the FSI coupling is obviously unstable and blows up.

If that is the case, then try make the problem easier and find what is breaking it and how to stop it breaking. e.g. try more slowly reducing the solid stiffness and density and changing the fluid properties (do one at a time), and experiment with other FSI coupling settings, egg, try Aitken's coupling.

[efendi]

Originally Posted by bigphil

Hi Daniel,

One thing to note is that in the HronTurek example cases in solids4foam, the FSI coupling is enabled at 2 seconds; this is done to allow the flow to develop first before enabling the coupling. If you are using the same settings then the FSI coupling is obviously unstable and blows up.

If that is the case, then try make the problem easier and find what is breaking it and how to stop it breaking. e.g. try more slowly reducing the solid stiffness and density and changing the fluid properties (do one at a time), and experiment with other FSI coupling settings, egg, try Aitken's coupling.

Hi, I am a new user for openFoam. Can you help me?
I want to ask a question about solids4Foam. Can this solver dissolve air and water together such as interFoam?

[bigphil]

Originally Posted by efendi

Hi, I am a new user for openFoam. Can you help me?
I want to ask a question about solids4Foam. Can this solver dissolve air and water together such as interFoam?

Yes, you can use the "interFluid" fluid model, which is just a ported version of interFoam. Have a look at the solids4foam training slides (e.g. at https://www.researchgate.net/profile...f/publications) which show an FSI version of the damBreak case (air, water and deformable solid).

[efendi]

Originally Posted by bigphil

Yes, you can use the "interFluid" fluid model, which is just a ported version of interFoam. Have a look at the solids4foam training slides (e.g. at https://www.researchgate.net/profile...f/publications) which show an FSI version of the damBreak case (air, water and deformable solid).

Thank you very much.

[efendi]

Originally Posted by bigphil

Yes, you can use the "interFluid" fluid model, which is just a ported version of interFoam. Have a look at the solids4foam training slides (e.g. at https://www.researchgate.net/profile...f/publications) which show an FSI version of the damBreak case (air, water and deformable solid).

Hi bigphil,
I want to study elastic material behavior for two-phase flow with solids4Foam. I want to use variableHeightFlowRateVelocity in inlet but I get an error for foamExtend 4.1 (trying to construct an genericFvPatchField on patch inlet of field rho). I tried to continue with the interElasticBeam tutorial but I am getting an error. For OpenFOAM 7, I get the error that the version is not suitable. Can you help with this? In short, I want to do something like the weirOverflow tutorial in OpenFoam 7.

[bigphil]

Originally Posted by efendi

Hi bigphil,
I want to study elastic material behavior for two-phase flow with solids4Foam. I want to use variableHeightFlowRateVelocity in inlet but I get an error for foamExtend 4.1 (trying to construct an genericFvPatchField on patch inlet of field rho). I tried to continue with the interElasticBeam tutorial but I am getting an error. For OpenFOAM 7, I get the error that the version is not suitable. Can you help with this? In short, I want to do something like the weirOverflow tutorial in OpenFoam 7.

One solution could be to use the nextRelease branch of solids4foam, which compiles with OpenFOAM-9 (see http://solids4foam.github.io/). That should be able to run the weirOverflow tutorial.

[efendi]

Originally Posted by bigphil

One solution could be to use the nextRelease branch of solids4foam, which compiles with OpenFOAM-9 (see http://solids4foam.github.io/). That should be able to run the weirOverflow tutorial.

Thank you very much. I will try it.

[efendi]

Originally Posted by bigphil

One solution could be to use the nextRelease branch of solids4foam, which compiles with OpenFOAM-9 (see http://solids4foam.github.io/). That should be able to run the weirOverflow tutorial.

Hi bigphil,
I compiled solids4Foam with of9 as your suggestion but now ı see this message "not implemented for this version of OpenFOAM"

[bigphil]

Originally Posted by efendi

Hi bigphil,
I compiled solids4Foam with of9 as your suggestion but now ı see this message "not implemented for this version of OpenFOAM"

Which fluid model are you using? Are you running a fluid-only case or is it FSI?

[efendi]

Originally Posted by bigphil

Which fluid model are you using? Are you running a fluid-only case or is it FSI?

I am working on fsi model. I want to examine the behavior of fluid and elastic materials using the same boundary conditions as in the weirOverFlow tutorial.

[bigphil]

Originally Posted by efendi

I am working on fsi model. I want to examine the behavior of fluid and elastic materials using the same boundary conditions as in the weirOverFlow tutorial.

I just checked using the nextRelease branch of solids4foam (from GitHub) using OpenFOAM-v2012, and weirOverflow tutorial work fines in solids4foam.


I did the following:

1. Change to the run directory: > cd $FOAM_RUN
2. Copied the weirOverflow tutorial from the tutorials: > cp -r $FOAM_TUTORIALS/multiphase/interFoam/RAS/weirOverflow .
3. Change into the case: > cd weirOverflow
4. solids4foam needs two extra files: physicsProperties and fluidProperties
5. Get physicsProperties from the solids4foam cylinderInChannel tutorial: > cp ../solids4foam/tutorials/fluids/cylinderInChannel/constant/physicsProperties constant/
6. Get fluidProperties from the solids4foam flexibleDamBreak tutorial (as it uses interFluid): > cp ../solids4foam/tutorials/fluidSolidInteraction/flexibleDamBreak/constant/fluid/fluidProperties constant/
7. Prepare the case as per the Allrun script: > cp -r 0.orig 0 && blockMesh && setFields
8. Run solids4Foam solver: > solids4Foam

If you want to make the weir deformable then start with the flexibleDamBreak tutorial and modify the solid and fluid meshes, solid and fluid boundary conditions, and other settings (e.g. controlDict).