CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Capabilities

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 2, 2007, 02:40
Default Hi. After reading the featur
  #1
New Member
 
Christian Holm
Join Date: Mar 2009
Posts: 8
Rep Power: 7
christianhf is on a distinguished road
Hi.
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?
christianhf is offline   Reply With Quote

Old   March 2, 2007, 05:58
Default hi, i'm not sure about 2) a
  #2
Senior Member
 
Stephan Gerber
Join Date: Mar 2009
Location: Germany
Posts: 118
Rep Power: 7
stephan is on a distinguished road
hi,

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.
stephan
stephan is offline   Reply With Quote

Old   March 5, 2007, 04:48
Default Hi, Thanks for your answer.
  #3
New Member
 
Christian Holm
Join Date: Mar 2009
Posts: 8
Rep Power: 7
christianhf is on a distinguished road
Hi,

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).
christianhf is offline   Reply With Quote

Old   March 5, 2007, 04:58
Default Hi Christian, Non-conformal
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,747
Rep Power: 20
hjasak will become famous soon enough
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.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   March 6, 2007, 08:30
Default Hi Hrvoje I don't know yet
  #5
New Member
 
Christian Holm
Join Date: Mar 2009
Posts: 8
Rep Power: 7
christianhf is on a distinguished road
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?
christianhf is offline   Reply With Quote

Old   March 6, 2007, 09:07
Default Hi Christian, Tell me, is t
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,747
Rep Power: 20
hjasak will become famous soon enough
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.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   March 7, 2007, 02:24
Default Hi Hrvoje. No, it is not. The
  #7
New Member
 
Christian Holm
Join Date: Mar 2009
Posts: 8
Rep Power: 7
christianhf is on a distinguished road
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?

Christian
christianhf is offline   Reply With Quote

Old   March 7, 2007, 06:27
Default Hi Christian, This sounds m
  #8
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,747
Rep Power: 20
hjasak will become famous soon enough
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,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 1, 2007, 14:45
Default Hrv, You said .."there are
  #9
sek
Member
 
Sung-Eun Kim
Join Date: Mar 2009
Posts: 76
Rep Power: 7
sek is on a distinguished road
Hrv,

You said .."there are issues with moving walls and scalar..". Can you please elaborate on that?
sek is offline   Reply With Quote

Old   May 1, 2007, 15:03
Default Yup, I can. Think of a roller
  #10
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,747
Rep Power: 20
hjasak will become famous soon enough
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,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 7, 2007, 05:42
Default Hi again, I have installed
  #11
New Member
 
Christian Holm
Join Date: Mar 2009
Posts: 8
Rep Power: 7
christianhf is on a distinguished road
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?
Furthermore:
Is the code capable of capturing the physics of an expanded bed?
Is it possible to have moving parts in the fluid bed?
christianhf is offline   Reply With Quote

Old   May 9, 2007, 04:55
Default No answers? I will try and ela
  #12
New Member
 
Christian Holm
Join Date: Mar 2009
Posts: 8
Rep Power: 7
christianhf is on a distinguished road
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.
christianhf is offline   Reply With Quote

Old   May 9, 2007, 10:02
Default Maybe you can simulate the rot
  #13
Senior Member
 
Billy
Join Date: Mar 2009
Posts: 167
Rep Power: 7
billy is on a distinguished road
Maybe you can simulate the rotating walls using a wall velocity. I don't understand why you want to use moving mesh.
billy is offline   Reply With Quote

Old   May 9, 2007, 11:06
Default Using moving parts is new to m
  #14
New Member
 
Christian Holm
Join Date: Mar 2009
Posts: 8
Rep Power: 7
christianhf is on a distinguished road
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.
christianhf is offline   Reply With Quote

Old   February 14, 2009, 02:07
Default Can openfoam solve cases havin
  #15
New Member
 
Chris
Join Date: Mar 2009
Posts: 2
Rep Power: 0
ccmica is on a distinguished road
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 is offline   Reply With Quote

Old   February 14, 2009, 02:10
Default Can openfoam solve cases havin
  #16
New Member
 
Chris
Join Date: Mar 2009
Posts: 2
Rep Power: 0
ccmica is on a distinguished road
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 is offline   Reply With Quote

Old   February 14, 2009, 06:29
Default I believe there is a tutorial
  #17
Member
 
Maruthamuthu Venkatraman
Join Date: Mar 2009
Location: Norway
Posts: 80
Rep Power: 7
maruthamuthu_venkatraman is on a distinguished road
I believe there is a tutorial with MRF case...

I havent tried it in OpenFoam, But the capabilities are there...
maruthamuthu_venkatraman is offline   Reply With Quote

Old   October 28, 2010, 21:02
Default Two way coupling in the Lagrangian particle tracking model
  #18
Member
 
Paul Reichl
Join Date: Feb 2010
Location: Melbourne, Victoria, Australia
Posts: 33
Rep Power: 6
preichl is on a distinguished road
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,

Paul.

Last edited by preichl; October 29, 2010 at 03:19.
preichl is offline   Reply With Quote

Old   November 9, 2010, 09:04
Default
  #19
New Member
 
Astrid Mahrla
Join Date: May 2010
Location: Munich, Germany
Posts: 22
Rep Power: 7
AMahrla is on a distinguished road
You could have a look at the OpenFOAMwiki entry of SIG on Multiphase flows: http://www.openfoamwiki.net/index.ph..._based_methods
There are some tutorials for particle based methods and test cases and literature...

Additionally, there's a user group on DEM on extend-project:
http://www.extend-project.de/user-gr...ewgroup/groups

Best,

Astrid Mahrla
AMahrla is offline   Reply With Quote

Old   November 11, 2010, 01:33
Default
  #20
Member
 
Paul Reichl
Join Date: Feb 2010
Location: Melbourne, Victoria, Australia
Posts: 33
Rep Power: 6
preichl is on a distinguished road
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,

Paul.
preichl is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
SMP Scaling Capabilities CK FLOW-3D 3 January 16, 2009 01:49
star-cd capabilities Ahmed CD-adapco 7 November 17, 2008 08:59
Capabilities christianhf OpenFOAM 0 February 28, 2007 10:02
FLUENT 6 capabilities Prashant FLUENT 3 October 17, 2001 16:08
Multiphase capabilities amc FLUENT 1 March 2, 2001 00:11


All times are GMT -4. The time now is 11:56.