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

Sig Turbomachinery Organize the next meeting

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 18, 2008, 09:13
Default Hi all, I'm starting a thread
  #1
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 9
cedric_duprat is on a distinguished road
Hi all,
I'm starting a thread about the geometry proposed by the organiser of the turbomachinery session of the 2008 OpenFOAM Workshop. (http://www.openfoamworkshop.org/08/i...itle=Main_Page)
I know that we can already use the Wiki to add comments from our work and I think that a thread will also be usefull also to work.

I'm focusing my work on the inlet boundary condition. I read the Clausen's article and I agree that from his swirl number (Sw) definition, we can calculate the rotation of the wall.
But, my point is that he usually defined swirl number otherwise : ratio of angular momentum flux in the radial direction to the axial momentum flux in the axial direction.

Is someone developped a tool to calculate Sw like that ?

The idea here will be to use Sw as a parameter of the calculation. Changing Sw during the calculation (so the wall velocity), we could see the evolution of the flow motion for different rotation.

Regards,

Cedric

PS: I played with the solver, adding Coriolis force and the centrifuge one but, results are not changing a lot ... according to my run :o)
cedric_duprat is offline   Reply With Quote

Old   February 18, 2008, 16:56
Default Hi Cedric, I'm glad to hear
  #2
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 9
hani is on a distinguished road
Hi Cedric,

I'm glad to hear that you are having a look at the proposed case study! I have a master student helping me do the same thing. We have currently studied different schemes and are on the way to study different solvers. We have of course also spent some time setting up everything in the svn and in the Wiki.

There is a sourceForge mail list for discussions within the turbomachinery field, but we can of course also have a discussion in the forum. Please organize your findings in the Wiki as well - the forum threads tend to lose their structures after a while.

I'm not quite sure if I understand your question. Clausen made a definition of the swirl number. You can use that swirl number to get the inlet rotation. If you prefer another swirl number you can use his measured profile and calculate any swirl number definition you would like. You don't need OpenFOAM for that.

If you vary the swirl number you should be able to verify that at higher swirl you get recirculation at the center, and at lower swirl number you get separation at the wall. During the measurements they made sure that neither of these flow features should happen. That it the reason why they picked exactly this swirl number. I'm however not sure if there are any detailed measurements to compare with at other swirl numbers.

It sound great that the solution is unaffected by a system rotation, which it ideally should.

I added some automatic postprocessing routines to the svn and the Wiki. Have a look at it. David Wood allowed us to distribute the measurements (he said that also Philip Clausen would be pleased
that their work has proven useful).

Håkan.
hani is offline   Reply With Quote

Old   February 19, 2008, 10:11
Default Hi everybody, I've just see
  #3
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 10
vinz is on a distinguished road
Hi everybody,

I've just seen the possibility to access the test case you're talking about.
Since the wiki is dead for an undetermined time, I'd like to know if there is another way to access the files?
I saw you were talking about a svn or source forge repository, would it be possible you directly post the links here?
Thanks for your help.

Vincent
vinz is offline   Reply With Quote

Old   February 19, 2008, 11:08
Default Hi Vincent, here is the way
  #4
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 9
cedric_duprat is on a distinguished road
Hi Vincent,

here is the way on SourceForge :

http://openfoam-extend.svn.sourceforge.net/svnroot/openfoam-extend/trunk/Breeder /OSIG/TurboMachinery/

In the wiki there was some tricks but, you can manage from SourceForge easily.
If you have more questions don't hesitate.

Cedric
cedric_duprat is offline   Reply With Quote

Old   February 19, 2008, 15:05
Default Hi Vincent, In the svn repo
  #5
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 9
hani is on a distinguished road
Hi Vincent,

In the svn repository you will find two different test cases, Case0 and Case1. Case0 refers to the original set-up proposed for the ERCOFTAC workshop. There is however not yet any inlet boundary condition added for that case in the svn. I have been working on Case1 myself, which is the same as Case0, but with some more domain before and after the diffuser. Read the README file in constant/polyMesh to see how to generate the grid (using m4 and blockMesh). Copy the 0_orig directory to a 0 directory, which will then contain the basic boundary conditions for the case. There is a utility that adds swirl and rotation to the inlet, the rotating walls and the internal cells attached in the svn. For this case a plug flow with a solid body swirl is assumed at the location of the rotating honeycomb. Run the case using simpleFoam until it stops at 1000 iterations. Postprocess the results by following the instructions in the postProcessing directory in the Case1 directory.

I hope that will help!

Håkan
hani is offline   Reply With Quote

Old   February 29, 2008, 04:45
Default Hi all, here are some of my ob
  #6
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 9
cedric_duprat is on a distinguished road
Hi all, here are some of my observations.

from the references in Wiki website, there is one from proceedings of 23rd IAHR Symposium, Yokohama, 2006.
The extensionLength of the outlet is quite different from our test case (Case0, Case1), the diameter of the dump is there between 3 and 5 times the difuseur exit diameter.
Even if it doesn't change anything at the inlet, the outlet seems to be better with such outlet (velocity).
with basics numerics (every thing by default)
but kinetic energy is still very strange in the center of the diffuseur (higher), I don't really get why.
...
that's all

pictures:
comparaison of U and W for Case0, Case1, Case2 with experiments:


here is for the kinetic energy:

cedric_duprat is offline   Reply With Quote

Old   February 29, 2008, 14:13
Default Hi Cedric, Nice to see that
  #7
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 9
hani is on a distinguished road
Hi Cedric,

Nice to see that you are working on the case!

The paper from Yokohama is by my PhD student Walter Gyllenram and myself. We added a dump in order to better approximate the outlet of the diffuser into open air. I agree that this is a better approximation than any of those in Case0 or Case1. If you have set up such a case for OpenFOAM using blockMesh and m4 you are free to add it to the svn repository and to the workshop wiki as Case2. For the paper in Yokohama we did it with ICEM CFD and we used our in-house solver. For case-studies like this it is however much better to distribute parameterized blockMeshDict files than full grids. For the grid in the Yokohama paper the dump consisted of 1.5E6 cells, just to mimic the outlet boundary condition!!!

Your results look the same as our results for Case1. The standard k-epsilon model seems to overpredict the turbulent kinetic energy in the solid-body-part of the swirl. I don't thing that is a big problem in this case since all the important things happen in the boundary layer. A better tubulence model should however not over-predict the turbulent kinetic energy like this. I have no previous experience with the k-epsilon model for this specific case. Anyone else?

In the paper from Yokohama you can find a proposed modification of the inlet velocity profile for Case1. Try that one and see if you get a better agreement.

It seems like you have studied Case0 also. Can you share your implementation of the inlet boundary condition in the svn repository? We did not have time yet to clean up our version of the inlet boundary condition, and it would also be nice to see different versions of implementations for the same purpose.

We have studied the results for Case1 for different discretization schemes, and we are currently looking at the convergence with different solvers for the pressure. We will inform you about those results as soon as we have the time. I'm in the middle of teaching, and my master student that is helping me with this work is also taking the course that I am giving. We should have more time soon.

Håkan.
hani is offline   Reply With Quote

Old   March 17, 2008, 09:45
Default Hi, Following the observat
  #8
New Member
 
Maryse Page
Join Date: Mar 2009
Posts: 8
Rep Power: 9
page is on a distinguished road
Hi,

Following the observations of Cedric and Hakan, I would like to mention that the Case1 that they are referring to, the inlet BC for the turbulent quantities are k=0.4 and epsilon=3.94. Based on the formula epsilon = (c_{mu} k^2)/ (nu (mu_T/mu) )), it corresponds to a ratio mu_T/mu = 270. If a smaller turbulent viscosity ratio is used, eg. mu_T/mu = 10, there is a much better agreement with the experimental results, especially in the core flow for the k values. See the plots below.

For Case0 that is in process of being fully contributed (an announcement about it will be made very soon), a ratio of mu_T/mu = 14.5 is used with the k based on the experimental measurements at the CS Z=-25mm for the ERCOFTAC conical diffuser testcase.



page is offline   Reply With Quote

Old   March 19, 2008, 09:28
Default Hi, I would like to bring t
  #9
New Member
 
Maryse Page
Join Date: Mar 2009
Posts: 8
Rep Power: 9
page is on a distinguished road
Hi,

I would like to bring to your attention that the testcase Case0 from the OpenFOAM Turbomachinery Working Group is now completely available for the ERCOFTAC conical diffuser case-study.

More informations about it are available on OpenFOAM wiki in Sig Turbomachinery / Organize the next meeting (Turbomachinery session at the Third OpenFOAM Workshop in Milano) (http://openfoamwiki.net/index.php/Si...e_next_meeting).

See also the message http://www.cfd-online.com/OpenFOAM_D...tml?1205924083 about the newly available boundary condition profile1DfixedValue to impose a 1D cylindrical fixed value profile.

Maryse Page
page is offline   Reply With Quote

Old   March 20, 2008, 10:18
Default Hi, I have updated Case1 wi
  #10
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 9
hani is on a distinguished road
Hi,

I have updated Case1 with new definitions for k and epsilon. You can find a discussion on this in the http://openfoamwiki.net/index.php/Sig_Turbomachinery_/_Organize_the_next_meeting #Case1

I have also added some info on how to automatically visualize the residuals, similar to how you visualize the results.

Håkan.
hani is offline   Reply With Quote

Old   March 20, 2008, 11:19
Default Hi again, I should also men
  #11
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 9
hani is on a distinguished road
Hi again,

I should also mention the following modifications to the ercoftacConicalDiffuser svn:

Log Message:
-----------
Normalization of measured K, and scaling

Modified Paths:
--------------

trunk/Breeder/OSIG/TurboMachinery/ercoftacConicalDiffuser/cases/Case1/p
ostProcessing/compareK.gplt

##########

Log Message:
-----------
Default outlet bc for pressure and alternatives

Modified Paths:
--------------

trunk/Breeder/OSIG/TurboMachinery/ercoftacConicalDiffuser/cases/Case1/0
_orig/p.gz

##########

Log Message:
-----------
writeInterval 100;

Modified Paths:
--------------

trunk/Breeder/OSIG/TurboMachinery/ercoftacConicalDiffuser/cases/Case1/s
ystem/controlDict

##########

Log Message:
-----------
div(phi,U) Gauss linearUpwind Gauss;

Modified Paths:
--------------

trunk/Breeder/OSIG/TurboMachinery/ercoftacConicalDiffuser/cases/Case1/s
ystem/fvSchemes

##########

Log Message:
-----------
Lower tolerances and specific versions for 1.4.1 and 1.4.1-dev

Modified Paths:
--------------

trunk/Breeder/OSIG/TurboMachinery/ercoftacConicalDiffuser/cases/Case1/s
ystem/fvSolution

Added Paths:
-----------

trunk/Breeder/OSIG/TurboMachinery/ercoftacConicalDiffuser/cases/Case1/s
ystem/fvSolution-1.4.1

trunk/Breeder/OSIG/TurboMachinery/ercoftacConicalDiffuser/cases/Case1/s
ystem/fvSolution-1.4.1-dev

Håkan
hani is offline   Reply With Quote

Old   March 31, 2008, 11:21
Default Hi every one! i want to do
  #12
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 10
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
Hi every one!
i want to do some numercial simulation in centrifugal pump by using MRFSimpleFoam,and now i have some question,would you please give me some advice?

http://www.cfd-online.com/OpenFOAM_D...tml?1206976586
waynezw0618 is offline   Reply With Quote

Old   May 9, 2008, 06:16
Default Hi, I just added two new ca
  #13
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 9
hani is on a distinguished road
Hi,

I just added two new cases for the ERCOFTAC conical diffuser case studies, see http://openfoamwiki.net/index.php/Sig_Turbomachinery_/_Organize_the_next_meeting . The files can be checked out from the OpenFOAM-extend project at sourceForge.

These cases, named Case2 and Case2.1, include a dump to better model the outlet of the diffuser. Case2.1 also includes the inlet velocity profile proposed by Gyllenram and Nilsson at IAHR2006 in Yokohama.

Håkan.
hani is offline   Reply With Quote

Old   June 8, 2008, 16:39
Default Hi, I have added a couple o
  #14
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 9
hani is on a distinguished road
Hi,

I have added a couple of new cases for the ERCOFTAC conical diffuser case studies, see http://openfoamwiki.net/index.php/Sig_Turbomachinery_/_Organize_the_next_meeting.

The cases that are now available in both the Wiki and in the svn are the following:

* Case0: Base case
* Case1: Extended base case
* Case1.1: Case1 with a radial mesh
* Case1.2: Case1 with MRFsimpleFoam
* Case1.3: Case1 as a 2D wedge case
* Case2: Dump case
* Case2.1: Dump case with the Gyllenram/Nilsson-IAHR/Yokohama inlet profile
* Case2.2: Case 2 with a radial mesh

For all these cases you have a parameterized grid generation procedure, instructions on how to run and post-process the case, and xfig files to generate figures for inclusion in your future manuscripts. The computational results are automatically compared with the ERCOFTAC measurements.

Enjoy!
Håkan.
hani is offline   Reply With Quote

Old   June 17, 2008, 07:04
Default Hi, The ERCOFTAC conical di
  #15
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 9
hani is on a distinguished road
Hi,

The ERCOFTAC conical diffuser case study has been moved to: http://openfoamwiki.net/index.php/Sig_Turbomachinery_/_ERCOFTAC_conical_diffuser

Håkan.
hani is offline   Reply With Quote

Old   June 17, 2008, 09:59
Default The link doesn't seem to work:
  #16
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 12
dmoroian is on a distinguished road
The link doesn't seem to work:
Quote:
Not Found

The requested URL /forum/messages/1/ http://openfoamwiki.net/index.php/Si...nical_diffuser was not found on this server.
Apache/2.2.3 (CentOS) Server at openfoam.cfd-online.com Port 80
dmoroian is offline   Reply With Quote

Old   June 17, 2008, 10:26
Default If you copy/paste the link to
  #17
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 9
hani is on a distinguished road
If you copy/paste the link to your browser it works, however when you click on it it does not work. I don't know why.

Here is a new link that should work:
http://openfoamwiki.net/index.php/Sig_Turbomachinery_/_ERCOFTAC_conical_diffuser

Håkan
hani is offline   Reply With Quote

Old   June 21, 2008, 05:27
Default I have moved the addSwirlAndRo
  #18
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 9
hani is on a distinguished road
I have moved the addSwirlAndRotation utility in the Sig Turbomachinery svn in order to align it with the other implementations of that part of the svn. See the Sig Turbomachinery Wiki for the details.

Those who have checked out these files previously should be able to do an 'svn update' to update to the new structure.

Håkan.
hani 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
User Meeting proceedings Bruno NUMECA 9 March 17, 2003 04:04
Fidap User Group Meeting jk FLUENT 1 June 9, 2002 06:28


All times are GMT -4. The time now is 18:25.