CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   SlidingInterface problem (http://www.cfd-online.com/Forums/openfoam-solving/58107-slidinginterface-problem.html)

ralph November 21, 2007 06:02

Hi all, Im experimenting wit
 
Hi all,
Im experimenting with the sliding interface.
As a testcase I chose the mixer2D example, which works for elder OpenFOAM versions (The case is taken off the tutorials of version 1.3, as it is not contained in version 1.4.1).
If I run the case with version 1.4.1 the following error occurs after at the beginning of the 3rd timestep:

FOAM FATAL ERROR : Duplicate point found in cut face. Error in the face cutting algorithm for global face 4(1318 1320 1341 1340) local face 4(14 16 37 36)
Slave size: 36 Master size: 36 index: 4.
Face: 4(825 826 856 855)
Cut face:
101
(
.
.
.

Does anyone know something about this?

Ralph

hjasak November 21, 2007 06:36

Yes. I have spent 2 weeks wor
 
Yes. I have spent 2 weeks working on this in 1.4.1-dev and now the sliding interface is 100% reliable.

Hrv

ralph November 21, 2007 06:59

Thanks a lot Hrvoje, Ill try
 
Thanks a lot Hrvoje,
Ill try it.

Ralph

rolando November 21, 2007 08:20

Hello Hrvoje, I tested your d
 
Hello Hrvoje,
I tested your development version for the same reason. The slidingInterface is realy working fine now.
In your development version I found the ggi.
Can you tell me something about the ggi? Is it working reliably?

Rolando

P.S:
I did some experiments with the mixerGgiFvMesh and the mixer2D case. The experiments showed, that I cannot run the mixer2D case (as it is posted) with the ggi. The simulation interrupted after some time with a singularity in the pressure equation.
If I doubled the number of cells in the circumferential direction, the simulation worked fine.
It was about 30% faster compared to the same case calculated with the slidingInterface.
Comparing the results (ggi - slidingInterface) showed very similar results for the velocities, but somewhat different results for the pressure distribution.

hjasak November 21, 2007 17:06

The GGI interface is an early
 
The GGI interface is an early development (and a basis for several projects), and is still being worked on in a collaboration with other groups. The mechanics of inplementation is in place, with the exception of weighting factor calculation.

I don't think you should be using this at the moment, as I am still not happy with the weighting factors - still under development.

Leave it alone for the moment, I will announce it when I'm happy with it.

Hrv

mahendra November 18, 2008 02:48

Hello everybody, I am tryin
 
Hello everybody,

I am trying this icoDyMFoam, for the mixerGgi tutorial from Hrvoje and I am ending up with this error.

Could anyone please help me resolve this error.

/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : icoDyMFoam
Date : Nov 18 2008
Time : 12:23:36
Host : linux
PID : 1670
Case : /home/ms.wankhede/OpenFOAM/ms.wankhede-1.5/tut/mixerGgi
nProcs : 1

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Selecting dynamicFvMesh mixerGgiFvMesh


Unknown dynamicFvMesh type mixerGgiFvMesh

Valid dynamicFvMesh types are :

5
(
dynamicRefineFvMesh
staticFvMesh
dynamicMotionSolverFvMesh
dynamicInkJetFvMesh
solidBodyMotionFvMesh
)


From function dynamicFvMesh::New(const IOobject&)
in file dynamicFvMesh/newDynamicFvMesh.C at line 79.

FOAM exiting


Thanks and Regards,
Mahendra

jaswi November 19, 2008 02:43

Hi Mahendra Please check th
 
Hi Mahendra

Please check the version you are using.

AFAIK mixerGgiFvMesh is not part of the official release.

Regarding the mixer2D or mixer3D, there are two appraoches available in OpenFOAM.

- sliding mesh method : available in both official and dev versions

- ggi (general grid interface) - available only in the dev version. This approach requires no topological changes and uses interpolation between the patches

If you have not done already then I would suggest you to try the mixer tutorial contained with the official release.

Hope this solves your problem

Kind Regards
Jaswi

mahendra November 19, 2008 03:09

Dear Jaswi ! Thankyou for t
 
Dear Jaswi !

Thankyou for the quick reply.

If you have any sliding interface case (rotating interfaces) along with documentation can you please send me one, it will be more helpful for understanding the way sliding interfaces work. By the way I am using OpenFOAM 1.5.

You can reach me on mahendra.wankhede@gmail.com

Thanks and Regards,
Mahendra

jaswi November 19, 2008 08:23

Hi Mahendra Here is the tes
 
Hi Mahendra

Here is the test case.

In my opinion it would be best if you just get it working first and play around a bit.

Explaining how the mixerFvMesh works is possible. I can do that but getting into the details of the sliding mesh implementation will be a bit offtrack for now.

Here is the test case. Let me know if it spits out any errors.

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif mixer2D.zip

Hope this serves your purpose
Jaswi

mahendra November 20, 2008 01:25

Dear Jaswi Thankyou very m
 
Dear Jaswi

Thankyou very much for posting the case here but I am unable to download it, whenever I click on the attachment above it opens in a new window and shows some weired characters. Please guide me how to download the case properly to my machine.

If possible please send as an attachment on
mahendra.wankhede@gmail.com

Thanks and Regards,
Mahendra

louisgag November 21, 2008 17:04

Mahendra, try to right-clic
 
Mahendra,

try to right-click the attachment and choose "save link as", it should work fine.

-Louis

tino_boelke December 18, 2008 09:02

He Jaswi, i tried to run yo
 
He Jaswi,

i tried to run your mixer2D case, but didnt get it to work. Until now it was very usefull for me to understand how a sliding and rotation system works in OpenFoam, therefore a lot of thx.

Now my problem: after start solving with command icoDyMFoam, i got this error:

tino@:~/OpenFOAM/tino-1.5/run/mixer2D$ icoDyMFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : icoDyMFoam
Date : Dec 18 2003
Time : 13:42:10
Host : hpAIR2
PID : 19684
Case : /home/tino/OpenFOAM/tino-1.5/run/mixer2D
nProcs : 1

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Selecting dynamicFvMesh mixerFvMesh


Unknown dynamicFvMesh type mixerFvMesh

Valid dynamicFvMesh types are :

5
(
dynamicRefineFvMesh
staticFvMesh
dynamicMotionSolverFvMesh
dynamicInkJetFvMesh
solidBodyMotionFvMesh
)


From function dynamicFvMesh::New(const IOobject&)
in file dynamicFvMesh/newDynamicFvMesh.C at line 79.

FOAM exiting

As you can see im using version 1.5, so hopefully u can help me solving this problem.
Further i want to simulate an impellersystem, so your help at this point will help me to realize this.

thx Tino

gcollecutt December 19, 2008 16:26

Tino, The missing mixerFvMe
 
Tino,

The missing mixerFvMesh can be fixed by adding the libtopoMeshChanger library and include to the options file in the icoDyMFoam Make directory and recompiling it. However under version 1.5 I have problems running Hrvoje's mixer3D test case - it complains about 'patch face having a neighbour'. See how you go with the 2D case.

Interestingly, the only mixer tutorial shipped with the official 1.5 release appears to be mixerVessel2D in the MRFFoam tutorial folder - and it only uses the rotating reference frame stuff, not the sliding interface. There is no icoTopoFoam nor can I find any other tutorial that appears to use the sliding interface. The dynamic mesh types already included (dynamicRefineFvMesh, staticFvMesh, dynamicMotionSolverFvMesh, dynamicInkJetFvMesh, solidBodyMotionFvMesh) appear to work, just not the mixerFvMesh.

Has anyone else successfully used the sliding interface (mixerFvMesh or mixerGgiMesh) in OF-1.5?

Greg.

hjasak December 19, 2008 17:35

Yes. You will need 1.5-dev fo
 
Yes. You will need 1.5-dev for this because in 1.5 the complete topology engine is so riddled with bugs that it is useless.

I have a pre-release 1.5-dev on:

http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/release/

and it will be in the SVN soon.

Hrv

gcollecutt December 20, 2008 02:19

Hrvoje, Thanks very much fo
 
Hrvoje,

Thanks very much for this. Your 1.5-dev version compiled fine on my system and the mixer2D tutorial works well (though had to change the fvSchemes file to reference rAU rather than rUA).

Greg.

hjasak December 20, 2008 06:56

Thanks for this - we will get
 
Thanks for this - we will get it into SVN so that you can change the tutorial yourself http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Good luck with more complex cases. There is 1 more bug fix that you need that I have just found (a new version uploaded just now). If you get into trouble, please shout.

Enjoy,

Hrv

philippose December 20, 2008 12:46

Hello Hrv, A Good evening t
 
Hello Hrv,

A Good evening to you... :-)!

I successfully compiled OpenFOAM-1.5-dev on Fedora 10 with GCC-4.3.2, and... it went off without any hitches... Thank you :-)! I have been waiting for your version for a while now :-)!

So, after compilation, I got back into my sliding mesh tests (after a very long break !)...

The case is basically two blocks, one larger, and above a smaller block. The smaller block "slides" on the bottom face of the larger block, and the system starts off, with the sliding face of the smaller block completely within the bounds of the sliding face of the larger block, and both surface meshes perfectly matched, both in cell density, and position.

The system was constructed using blockMesh (100% hexahedral cells).

The "linearValveFvMesh" library is used for the sliding interface.

To test the motion, I used the "moveDynamicMesh" utility.

The simulation aborted after the second time step with an "Incompatible size before mapping" error in the "decoupling sliders" phase.... here is the log file (didnt paste it here because the indentation would be ignored):

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif log

What might I be doing wrong?

For completeness, I have also included the case itself...it would be great if you could probably have a look to see if I am setting up something incorrectly.

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif 002_slidingTest_hex.tgz

Have a nice day and a great weekend :-)!

Philippose

philippose December 20, 2008 15:40

Hello again Hrv, I think I
 
Hello again Hrv,

I think I have more or less solved the issue (as of now) :-)!

I created a new topo-changer library which is basically a modification of the mixerFvMesh library, to handle linear motion rather than rotary motion.

The way I have understood it, is that it looks like the normal motion solvers (such as laplaceFaceDecomposition, and velocityLaplacian, etc...etc...) have a problem working together with a mesh modified by the "linearValveFvMesh" library.

So far, I was under the impression, that once the sliding interface was "detached", the downstream setup would not be aware that the mesh was modified by a meshModifier, hence, allowing the normal motion solvers to function as though it was the only system controlling the mesh topology (and vice-versa). However, I think I understood that wrong....

In the modified library, the motion of the mesh is handled within the topoChanger library (as in mixerFvMesh), and the motion Solvers are not used any more.

I confirmed that this works for the test case I posted above (100% hex), as well as for my target case (100% tet... though here I did see warnings of high skew elements after a certain amount of penetration between the sliding interfaces... but that would a mesh related issue I would think)

Could you explain why there seems to be this problem between the topology modifiers and the motion solvers?

I must say....the sliding interface function looks really cool :-)! I hope I can directly implement it into my systems when I get back to work next year :-)!

Have a great evening!

Philippose

bastil December 23, 2008 15:52

Can somebody please clear the
 
Can somebody please clear the difference between the git-Version (sometimes called 1.5.x and sometimes called "dev") and the subversion "dev" Version? IS the subversion-Version based opon the git-Repository, e.g. does it include bugfixes?

antonio_ing December 31, 2008 06:20

i have some problem downloadin
 
i have some problem downloading the ThirtyPart software because the source file could not be read. Did I do something wrong??

thanks and happy 2009


All times are GMT -4. The time now is 09:16.