Hi,

Started v6.1, Fluent implemented dynamic moving mesh which support birth/death of elements. I am wondering if OpenFOAM has something similar.

For example, a piston moving inside a cylinder. The computational domain changes with time. There are two ways to attack this:

1. keep the number of elements the same, but "squeeze" the elements when the piston moves toward the head of the cylinder.
2. Keep the element sizes about the same, but, dynamically removes the number of elements.

Pei

sounds like Kiva as well ... i noticed a kivatest directory somewhere in the package ...

Yes OpenFOAM includes this functionality.

Hi,

I've placed an 2D wedge example of how the this works here:

http://www.tfd.chalmers.se/~nordin/foam/engineEx.mpg

The layer where cell addition/removal is performed can be anywhere in the domain.
That means that you can either have the piston remove cell layers as the layer become 'small enough' or you can have the entire mesh move upwards and remove the layer at the top/deck.
In this example I've placed the addition/removal layer somewhere in between and as this layer hits the deck the mesh motions switches from layer addition to 'squeezing'.
The left part show you the entire picture while the right is just a zoom-in on the top part.

If you are interested in another mesh motion example there is the channel flow with a vibrating 'floor'
http://www.tfd.chalmers.se/~nordin/f...ingChannel.mpg

Niklas

Hi, Niklas,

These two movies looked very cool.

In the engineEx.mpg movie, toward the end of the simulation, I saw some clouds of green dots at the upper left corner, what are they?

Also, I have a cylinder that does not have a straight wall. It is somewhat conical. The radius at the bottom is about 10% smaller than the radius at the top. I do not have a piston, but a small pipe coming down toward the bottom of the cylinder. The cylinder is about 10% filled with liquid. Is it possible to create a cylindrical block the wraps the pipe. This portion will be moving mesh. And create another block that is stationary mesh which contains the rest of the geometry? An interface between the two meshes will be needed in this case (this is how Fluent attach this type of problem). Do you FOAM can handle something like this? Thanks!

Pei

A combination of automatic mesh motion and my mesh modifiers should cover it - you need a combination of a layer addition/removal and a sliding interface + appropriate mesh motion setup.

Enjoy,

Hrv

Heya Niklas,

Nice animation - is that spray doing the right thing, i.e. do you get problems loosing particles or similar on layer removal? Any problems with the simulation: spikes in the pressure trace for example. BTW, is this compressible?

Hrv

Hi,
Yes, the green dots is the spray.

And no Hrv, the new tracking algorithm does not lose particles
In fact, it can not lose particles and if you are trying to lose them anyway, i.e you treat them incorrectly at the boundary, you will end up in an infinite loop (my choice since I dont want particles flying outside the domain)
The only restriction is that it must be possible to draw a line from cell centre to face centre without crossing a face.

Yes, the calculation is compressible and yes there are 'spikes' in the pressure, but this is depends on where you do the layer addition/removal and how small you want the cells before removing them... and time step.

It also seems to be more difficult adding layers than removing them!!!

And if I remember correctly removing cells at the piston top is worse than doing it somewhere 'in the middle'.

N

Thanks for that, I bet you're really proud of not losing particles - well done (there's a very few people in CFD today who can say the same)!

Any hope of a warning/debug when there's no way from the infinite loop - that would be useful info! [:-)]

We'll need to do something about the spikes at some stage, although this business with layer addition vs. removal is against my intuition. If you break the layering, pls let me know as there's a number of fixes I've got for a future release...

Enjoy,

Hrv

I am interested in the vibrating floor in the channel flow case.

http://www.tfd.chalmers.se/~nordin/f...ingChannel.mpg

My understanding is that we should specify the wall moving velocity motionU(x,y,t) for that 2D case. When I dig into the source code for the motionSolver, I felt a little bit lost.

Does any one can show me some sample code to specify that motionU on the moving wall?

Here's a piece of my original code from a while back. The setup is now much easier, using the motion solver - have a look at the current state of OpenFOAM-1.0/applications/utilities/mesh/manipulation/moveMesh

(I am one version ahead, so mine might me slightly different). Add

# include "setBoundaryMotion.H"

into moveMesh (your copy, of course!) before the points are moved. The file looks like this (you may want to read in the amplitude and frequency in from a control file and do additional tricks with findPathcID, so that the patch can be given by name etc etc.) I could not be botherred, mut here is a simple case with lots of comments :-)

The first lot calculates the boundary motion from the nodal coordinates and the last line sets the boundary condition for mesh motion:

ms.motionU().boundaryField()[movingPatchID] == motionBCPatch0;

This will work both for the face and cell decomposition.

There will be a paper coming out soon on the automatic mesh motion I have developed and implemented in foam and I would be grateful if people could refer to it in their applications/reports/papers - consider it a price to be paid for the work! :-)

setBoundaryMotion.H

{
label movingPatchID = 0;

scalar xfreq = 50;
scalar xampli = 0.0001;
scalar xlength = 0.01;

scalar xom = 2.0 * physicalConstant::pi*xfreq ;
scalar xomx = 4*physicalConstant::pi/xlength ;

// This statement gives you the position of points on the patch

const vectorField& motionPatchPoints =
ms.motionU().mesh().boundary()[movingPatchID].localPoints();

// This statement creates a vector field of the same size,
// which is set to zero

vectorField motionBCPatch0(motionPatchPoints.size(), vector::zero);

// This statement calculates the desired motion velocity
// and puts it as the y-component of the vector field above.
// The velocity will be different for every vertex.

Info << "Lift: " << xampli*Foam::sin(xom*runTime.value()) << endl;

motionBCPatch0.replace
(
vector::Y,
(
xampli*Foam::sin(xom*runTime.value())
*Foam::cos(xomx*motionPatchPoints.component(vector ::X))
- motionPatchPoints.component(vector::Y)
)/runTime.deltaT().value()
);

// This statement sets the velocity we have just calculated
// as the boundary condition for mesh motion

ms.motionU().boundaryField()[movingPatchID] == motionBCPatch0;
}

Hi, Niklas,

I am wondering if you can email me the steps to set up the moving mesh? Or any simple case file you have.

In my project, I will also need to setup a sliding interface. I have no idea how this is done in OpenFOAM.

Thanks!

Pei

Hi,

> I am wondering if you can email me the steps to
> set up the moving mesh? Or any simple case file
> you have.

I'm hoping this will be included in the next release of OpenFOAM

> I will also need to setup a sliding interface.
> I have no idea how this is done in OpenFOAM.
Neither do I.

N

sliding interface: the mixer2D tutorial case uses a sliding interface. The ./Alltest script should run the case or you can run it by hand.

Have a look at the createSlider application which creates all the nessecary files.

Mattijs

Well, it seems that I am the only one who knows precisely what needs to be done (I wrote the code). I would be happy to help, but under the condition that you convert your case into a fully-fledged tutorial and write up the setup for the manual.

In this way, we can easily extend the number of available tutorials and I won't have to explain the whole thing again.

Hrv

Hi, Hrv,

That will be great! If you can email me the steps to setup a moving mesh (with cell birth and death) with sliding interfaces, I will complete the tutorial case and write the detailed setup for the manual. This case will invlove air and water, so, interFoam will be applied.

Thanks!

Pei
Peiying2003@yahoo.com

Hi,
Can anybody help me ???
I want to simulate an air flow into an engine with a LES solver (oodles), but in the geometry there is a moving mesh (piston)... How can I do it???
Thanks

[henry]

The easiest way would be to replace the construction and calls of the turbulence model in engineFoam with the equivalent LES model construction and calls from Xoodles.

Hi Henry,
excuse me but this was not what I meant. My geometry is a simple box with a moving wall, so I haven't any crank angle....

[henry]

Is your flow compressible or incompressible?