[Hgholami]

Dear Foamer
I studied article "OpenFOAM FINITE VOLUME SOLVER FOR FLUID-SOLID INTERACTION" that describe fsiFoam solver and also see code of solid solver. it mentioned the deformation gradient as "F=I+trasnpose(DU)", but I saw in the others solid studies as "F=I+DU" for example"https://www.continuummechanics.org/deformationgradient.html". My problem is why it changed?
Thanks

[Hgholami]

In Article "A Lagrangian Cell-Centred Finite Volume Method for Metal Forming Simulation", Page (5), it mentioned "The relative deformation gradient is given in terms of the displacement increment as f = I + ∇(u)T". But I saw in solid mechanics book that the deformation gradient is f =I+∇(u), without transpose.
In OpenFOAM the code of deformation gradient was

volTensorField F = I + gradD_.T();

and I think the strain had this code E=0.5(transpose(F)*F-I)=0.5(gradD_ +gradD_.T()+gradD_ & gradD_.T() )

epsilon_ = symm(gradD_); //=0.5(gradD_+gradD_.T())
if(nonLinear == nonLinearGeometry::TOTAL_LAGRANGIAN)
{
epsilon_ += 0.5*symm(gradD_ & gradD_.T());
}

I thinks, the article wrote base on OpenFOAM definition not solid mechanics book, is it OK?
because for grad different in OpenFOAM, I found this

is it OK?

[bigphil]

Hi Hojatollah,

Yes your OpenFOAM definition of fvc::grad(U)().T() is correct, and you are correct that it is the same as \frac{\partial U}{\partial X} from your solid mechanics reference.

The OpenFOAM definition comes from the outer product of nabla (a vector) and U (a vector), where nabla = (\frac{\partial}{\partial x} \frac{\partial}{\partial y} \frac{\partial}{\partial z}).

Hopefully, this makes sense.

You can always double-check the components to be sure.

Philip

[Hgholami]

Originally Posted by bigphil

Hi Hojatollah,

Yes your OpenFOAM definition of fvc::grad(U)().T() is correct, and you are correct that it is the same as \frac{\partial U}{\partial X} from your solid mechanics reference.

The OpenFOAM definition comes from the outer product of nabla (a vector) and U (a vector), where nabla = (\frac{\partial}{\partial x} \frac{\partial}{\partial y} \frac{\partial}{\partial z}).

Hopefully, this makes sense.

You can always double-check the components to be sure.

Philip

Thanks for your reply

[HosseinB]

Hi community,



foam-extended 4.0, fsiFoam, 2D



I have a solid-fluid system that I'd like to model.


It is a thin horizontal plate (red in the attached figure) fixed at its two end vertical edges. The plate is on top of a flow with an inlet horizontal flow speed. In the middle of the flow, there is a rigid box diverting the flow.



I expect this flow diversion to deflect the plate. fsiFoam, however, doesn't capture any solid deformation. My problem is not its visualization in paraview. I have changed the inlet flow speed, elastic modulus and thickness of the plate and the plate just doesn't move.



I have built my model following the 3dTube and HronTurelFsi3 tutorials of the fe40/fsiFoam.



My case files are attached.




Note that I copy and paste the following in my command line to run my case:


sed -i s/tcsh/sh/g *Links ./removeSerialLinks fluid solid ./makeSerialLinks fluid solid cd fluid ./Allclean ./Allrun



I would be thankful if you could help me figure out what the issue is.



Hossein

[Hgholami]

Hi,
First in attached files. the coupled in fsiProperties is no, do you sure you change it to yes.

[HosseinB]

Originally Posted by Hgholami

Hi,
First in attached files. the coupled in fsiProperties is no, do you sure you change it to yes.

Thanks Hojatollah and Philip,


I set the "coupled" to "yes" and it is working now (wondering why in the 3DTube example with "coupled" set to "off", it was still working!)


Another question:


How can I add gravity forces to both solid and fluid?



Thanks a lot,
Hossein

[Hgholami]

Hi
first in 3DTube example, the coupled is yes. May you see Hron-Turek example that have coupled off and it turn on after 2s by HronTurekReport's object

bool Foam::hronTurekReport::execute()
{
const fvMesh& mesh =
time_.lookupObject<fvMesh>(regionName_);

fluidSolidInterface& fsi =
const_cast<fluidSolidInterface&>
(
mesh.lookupObject<fluidSolidInterface>("fsiPropert ies")
);

if (time_.value()>2)
{
if (!fsi.coupled())
{
fsi.set("coupled", true);
}
}

return writeData();
}

for another question:
In solid region we have bodyForce that read from solidProperties file (g)

if (solidProperties().found("g"))
{
bodyForce() = dimensionedVector(solidProperties().lookup("g"));
}

and use it in DEqn

fvVectorMatrix DEqn
(
rho_*fvm::d2dt2(D_)
== fvm::laplacian(2*muf_ + lambdaf_, D_, "laplacian(DD,D)")
+ fvc::div
(
mesh().Sf()
& (
- (muf_ + lambdaf_)*gradDf_
+ muf_*gradDf_.T()
+ lambdaf_*(I*tr(gradDf_))
)
)
+ rho_*bodyForce()
);

For fluid, as the flow is forced. usually the gravity is neglect. But you can add some code similar solid solver to fluid solver.
First define bodyForce (declare), then read bodyForce (fluidProperties.lookup) and finally add it to momentum equation (UEqn)
Don't forget to add similar variable to .H file

[HosseinB]

Originally Posted by Hgholami

Hi
first in 3DTube example, the coupled is yes. May you see Hron-Turek example that have coupled off and it turn on after 2s by HronTurekReport's object

for another question:
In solid region we have bodyForce that read from solidProperties file (g)

and use it in DEqn

For fluid, as the flow is forced. usually the gravity is neglect. But you can add some code similar solid solver to fluid solver.
First define bodyForce (declare), then read bodyForce (fluidProperties.lookup) and finally add it to momentum equation (UEqn)
Don't forget to add similar variable to .H file

Thanks for your reply.


My eventual goals is to simulate a case where the gravity and buoyancy (fluid pushing the plate up when the plate deflects into the fluid) are both taken into account.



I am aware that interFoam (VoF two-phase flow solver of openFoam) includes the gravity, but not the buoyancy. My simulation isn't a two-phase flow case since I only have the fluid and the plate.



Is fsiFoam suitable for this simulation?


Cheers,
Hossein

[wanghongjie]

Originally Posted by HosseinB

Thanks for your reply.


My eventual goals is to simulate a case where the gravity and buoyancy (fluid pushing the plate up when the plate deflects into the fluid) are both taken into account.



I am aware that interFoam (VoF two-phase flow solver of openFoam) includes the gravity, but not the buoyancy. My simulation isn't a two-phase flow case since I only have the fluid and the plate.



Is fsiFoam suitable for this simulation?


Cheers,
Hossein

Did you have a solution?