CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Running, Solving & CFD (
-   -   Capabilities (

christianhf March 2, 2007 02:40

Hi. After reading the featur
After reading the feature section, I am still uncertain whether OpenFoam supports:

1) 2-way coupling in the Lagrangian particle tracking model?
2) Rotating frames, i.e I have a rotating arm in my setup. Can that be modeled in some way?
3) is it possible to make unconformal meshes?

stephan March 2, 2007 05:58

hi, i'm not sure about 2) a

i'm not sure about 2) and 3) but the two-way-coupling is included. the change of momentum of each particle in each cell is used to determine the momentumchange in a time step.
the summation does not include the gravity (as least in the former versions of foam), so i guess the gravity term should be included in this statement (grep for "nmom" and "omom" -should be in parcel.c) since accelaration caused by gravity is external not internal).
if you are interested in a 4-way-coupling - let me know - it will take quit a while to bring it in a "exportable" style - so maybe in the end of april there will be a foam version with 4-way-coupling.

christianhf March 5, 2007 04:48

Hi, Thanks for your answer.

Thanks for your answer. I won't need a 4-way coupling, but thanks for the offer.

I have re-read the feature section a few times, and it might be that non-conformal meshes are possible.
I can however not find any hints about whether rotating boundaries are possible (like in a rotating propeller in a tank).

hjasak March 5, 2007 04:58

Hi Christian, Non-conformal
Hi Christian,

Non-conformal meshes are indeed possible - basically, the cell next to the "non-conformal interface" is a polyhedron and that's all. I am not sure if your non-conformal interface is sliding or stationary, but in any case both work. The issue may be how to create this mesh, and there is a number of options like blockMesh with non-conformal block or Star-CD converter. Where are you getting the mesh from?

Regarding the other questions, rotating refrerence frames are easy, but you may need to do some top-level code modifications to add the forces into the momentum equation (or have someone do it for you). 2-way coupling with a Lagrangian model is a standard part of the story.



christianhf March 6, 2007 08:30

Hi Hrvoje I don't know yet
Hi Hrvoje

I don't know yet if the non-conformal mesh will be sliding or not – it depends on how I need to make the rotating propeller (in which there are small cavities upon which I intended the non-conformal mesh).
I have also not yet decided with what I will make the mesh. Preferably, I would do the whole geometry and meshing with OpenFoam, if possible. Else, I will have to buy a limiting license for software (I don't know yet what geometry/meshing software to use if not OpenFoam). Maybe Gambit as this is the only pre-solver program that I have experience with. Do you perchance have any advice in that direction?

Ok, the tip about adding (centrifugal) forces are noted. Thanks.
When you mention rotating references, is that what are used when I will model a propeller-like device rotating I a stationary barrel?

hjasak March 6, 2007 09:07

Hi Christian, Tell me, is t
Hi Christian,

Tell me, is this meant to be a real propeller with little bits of cavitation damage or a simplified geometry? Have you every personally built some real propeller meshes or is this a first attempt?

The thing is that meshing real propellers is notoriously difficult. Depending on the age of the propeller and the expertise of the CAD use in the company you may get a bunch of points on blade surfaces (absolute nightmare), a complex definition of quadric surfaces (nightmare), or a CAD model (mini-nightmare). From what you are trying to do, it seems to me you are after a good hex mesh capable of doing justice to the cavitation physics + tons of cells to capture existing cavitation damage. I would strongly advise you consider your options, maybe including automatic polyhedral mesh gemeration.

Rotating frames: this depends what you're doing. If the propeller is in a barel with baffles, you probably need to handle the sliding; otherwise you can solve the whole lot in a relative reference frame.


christianhf March 7, 2007 02:24

Hi Hrvoje. No, it is not. The
Hi Hrvoje.
No, it is not. The "propeller" is a simple rotating arm with holes in it. I don't yet know the size of the holes, but definetly larger than cavitation pits.
It is the first time I shall model such a case.

As it is not a real propeller but only a stirring device which will turn slowly, there will be no cavitation and it is also not critical with capturing separation around the arm (it will be small as the arm has a small diameter compared to the barrel geometry).

The barel contains some fluid and maybe also particles, and I will be looking at the dispersion in the barrel.

The barrel has no baffles, so you recommend that I use relative reference frame? Will that capture the stirring that the arm does?


hjasak March 7, 2007 06:27

Hi Christian, This sounds m
Hi Christian,

This sounds much better. It would be probably best to do this in a rotating reference frame (there are issues with moving walls and scalars that I discovered recently and a rotating frame will neatly sort out the problem). Stirring will be captured with no problems.

Good luck with the simulation,


sek May 1, 2007 13:45

Hrv, You said .."there are

You said .."there are issues with moving walls and scalar..". Can you please elaborate on that?

hjasak May 1, 2007 14:03

Yup, I can. Think of a roller
Yup, I can. Think of a roller bearing and consider the coordinate system set up around the main axis of rotation. For the two rings of the bearing there are no problems: the rotational velocity is tangential to the surface. Now consider the ball: it simultaneously rotates around the main axis and around its own axis. When you draw the resulting velocity on the surface, you will see that it has got a normal component (because of precession, right?). Therefore, we have now chosen a coordinate system where the mesh does not move but the wall has got a wall-normal velocity component.

A non-zero normal velocity on the wall means a non-zero flux (OK). The flux can go either into the domain ("wall moving forwards") or out ("wall moving back"). Now think of a scalar, like volume fraction in VOF: what it the boundary condition on the wall?

Ideally (assume no contact angle effect), the boundary condition would be zero gradient: gamma on the wall is equal to whatever is next to the wall. However:
- if I do zero gradient and have a flux going in, the b.c. will be unstable (blow up)
- if I say i "know" gamma on the wall, all is well for the incoming flux. However, if the flow is going out, the fixed value outlet will make it blow up again!

Basically, for such situations, I must pick the coordinate system such that the wall-normal velocity on all walls is zero. If I choose any other reference frame, I cannot set up a valid boundary condition for a scalar: whatever I do, it will blow up.

Hope this helps,


christianhf May 7, 2007 04:42

Hi again, I have installed
Hi again,

I have installed the code, but am uncertain regarding a few issues:

I need to simulate a rotating device in an expanded fluid bed (the state where the bed is only just "lifted" or fluidized). The rotating device will be close to the wall.

I am uncertain of which approach to use to simulate this. Can you comment on this?
Is the code capable of capturing the physics of an expanded bed?
Is it possible to have moving parts in the fluid bed?

christianhf May 9, 2007 03:55

No answers? I will try and ela
No answers? I will try and elaborate my questions:

Hrvoje said that moving walls can be problematic. I am uncertain whether I can use moving mesh and not moving walls when simulating my rotating device that are positioned close to the walls (the rotating device will, I guess, be a rotating wall and as the device is close to the external walls which are stationary, I imagine that having the mesh rotating with a stationary and rotating wall close to each other, will be problematic. Does that sound correct or is it possible to avoid the moving wall.

And as the device rotates inside the fluid bed, the model needs to be able to capture the stiirring. Hrvoje mentioned that a fluid will be stirred by the rotating motion, but as the fluid bed models and fluid models are separate, I would like to confirm that the stirring of the fluid bed material will be captured when a rotating device is placed in the bed.

billy May 9, 2007 09:02

Maybe you can simulate the rot
Maybe you can simulate the rotating walls using a wall velocity. I don't understand why you want to use moving mesh.

christianhf May 9, 2007 10:06

Using moving parts is new to m
Using moving parts is new to me - and OpenFoam is also, so the strategy I need to use to solve my problem is not one I am sure of.
I have not heard of a wall velocity, but it sounds like moving walls, which Hrvoje warned against.
The moving mesh strategy sounded more robust.

But then again - I am new to OpenFoam, and may have misunderstand something.

ccmica February 14, 2009 02:07

Can openfoam solve cases havin
Can openfoam solve cases having weak rotor-stator interactions using multiple rotating reference frames?
Usually I do this using fluent where the stator is in a stationary frame of reference and the rotor is in a rotating reference frame.
If yes, any suggestions on how to set it up.

ccmica February 14, 2009 02:10

Can openfoam solve cases havin
Can openfoam solve cases having weak rotor-stator interactions using multiple rotating reference frames?
Usually I do this using fluent where the stator is in a stationary frame of reference and the rotor is in a rotating reference frame.
If yes, any suggestions on how to set it up.

maruthamuthu_venkatraman February 14, 2009 06:29

I believe there is a tutorial
I believe there is a tutorial with MRF case...

I havent tried it in OpenFoam, But the capabilities are there...

preichl October 28, 2010 20:02

Two way coupling in the Lagrangian particle tracking model
Hi All,

I am interested in looking at 2 way Lagrangian particle coupling and I was wondering if anyone could point me to some examples that show its usage.

In my case I am interested in both the the flow field that results when a series of discrete particles are injected into the domain and the influence of this flow on the particles subsequent trajectories. Is this possible using one of the standard solvers in openFoam?, or do I need to modify one to do this?.

I am also interested in reading the feature article that the first post in this tread makes reference to. Any pointer to where I could find this article?.

Thanks in advance,


AMahrla November 9, 2010 09:04

You could have a look at the OpenFOAMwiki entry of SIG on Multiphase flows:
There are some tutorials for particle based methods and test cases and literature...

Additionally, there's a user group on DEM on extend-project:


Astrid Mahrla

preichl November 11, 2010 01:33

Thanks Astrid,

solidParticleFoam looks very interesting. I am currently using openFoam 1.7 and it appears as if solidParticleFoam requires openFoam 1.5.x. I will try getting version 1.5.x and post a reply if I get it working.

Thanks again,


All times are GMT -4. The time now is 09:21.