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

Problem using AMI

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

Like Tree28Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   May 24, 2012, 08:04
Default
  #101
kid
Senior Member
 
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 8
kid is on a distinguished road
I blindly followed "linnemann"'s suggestion above. Put some time reading his answers to my silly question.
Keeping his suggestions used SALOME to generate a rotor mesh and stator mesh.
Use salome document to make suitable groups name like AMI,inlet,outle,uWall etc.
The document is available use google. (this step is very importent.
Then exported UNV file of mesh to OpenFOAM case directory.
ideasUnvToFoam mesh_name
Used mergeMeshes to merge two meshes.
And made changes in boundary file to implement cyclicAMI.
Also used this command below before running pimpleDyFoam
splitMeshRegions -makeCellZones -overwrite
pimpleDyFoam

Though i need to improve my mesh now.

__________________
________________________________________
Regards,
CFDkid

It never gets easier You just get Better

Last edited by kid; May 24, 2012 at 08:04. Reason: just
kid is offline   Reply With Quote

Old   May 24, 2012, 08:08
Default
  #102
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
The procedure is the same for me except I'm using ICEM CFD and exporting to FLUENT V6. I think you are just simply lucky with your mesh.

Can you give me the mesh sizes on the interfaces? Whats the height of the first BL?

Quote:
Originally Posted by kid View Post
I blindly followed "linnemann"'s suggestion above. Put some time reading his answers to my silly question.
Keeping his suggestions used SALOME to generate a rotor mesh and stator mesh.
Use salome document to make suitable groups name like AMI,inlet,outle,uWall etc.
The document is available use google. (this step is very importent.
Then exported UNV file of mesh to OpenFOAM case directory.
ideasUnvToFoam mesh_name
Used mergeMeshes to merge two meshes.
And made changes in boundary file to implement cyclicAMI.
Also used this command below before running pimpleDyFoam
splitMeshRegions -makeCellZones -overwrite
pimpleDyFoam

Though i need to improve my mesh now.

__________________
CFD= Cleverly Formatted Data
Attesz is offline   Reply With Quote

Old   May 24, 2012, 08:13
Default
  #103
kid
Senior Member
 
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 8
kid is on a distinguished road
attesz
I have not concentrated on mesh for BL.
Need to do it now.
See a snap picture here. Also my case is simple rotating cube.
Attached Images
File Type: jpg rotor_stator.jpg (100.8 KB, 173 views)
__________________
________________________________________
Regards,
CFDkid

It never gets easier You just get Better
kid is offline   Reply With Quote

Old   May 24, 2012, 08:16
Default
  #104
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
you have huge size difference on the AMI, and it's working? I have equal sizes on the sides and not...weird!
__________________
CFD= Cleverly Formatted Data
Attesz is offline   Reply With Quote

Old   May 24, 2012, 08:22
Default
  #105
kid
Senior Member
 
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 8
kid is on a distinguished road
Attesz,
When you say working, let me clarify one point. My AMI patches are not coming zero, though previously when i used sHM it was giving 0 same as yours.

solidBodyMotionFunctions::rotatingMotion::transfor mation(): Time = 0.422334 transformation: ((0.207161 0.0515734 0) (0.24158 (0 0 -0.970381)))
AMI: Creating addressing and weights between 640 source faces and 92 target faces // this could be because of huge difference u pointed.
AMI: Patch source weights min/max/average = 0.943968, 1.0575, 0.999964
AMI: Patch target weights min/max/average = 0.956902, 1.10444, 1.00906

That is all working.
But result still blows after few iteration, though results are good before it blows and mesh difference on either side of AMI might be the culprit.
__________________
________________________________________
Regards,
CFDkid

It never gets easier You just get Better
kid is offline   Reply With Quote

Old   May 25, 2012, 02:48
Default
  #106
kid
Senior Member
 
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 8
kid is on a distinguished road
Hi,
AMI problem was fixed and results of rotating cube seems to converged.
Sharing a vedio for pressure of rotating cube, implemented using OpenFoam-21x and Salome mesher.
http://db.tt/T8ycTsE3
__________________
________________________________________
Regards,
CFDkid

It never gets easier You just get Better
kid is offline   Reply With Quote

Old   May 25, 2012, 04:18
Default
  #107
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 490
Rep Power: 9
samiam1000 is on a distinguished road
Dear All,

I am trying to simulate an opening windows.

I have created (with Fluent) some meshes (1st with a closed door, then a 15 opening, then 30 and so on..).

I am now trying to understand how to link them. I tried a moveDynamicMesh, This could be a good idea, but I guess that 15 is too much. Hence I will need more meshes.

What about AMI? Do you think this could help? If so, what should I do?

Thanks,

Sam
samiam1000 is offline   Reply With Quote

Old   May 25, 2012, 04:54
Default
  #108
kid
Senior Member
 
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 8
kid is on a distinguished road
samiam,

You want to simulate opening window or open window at different angles as you say.

Also you are using 15,30 etc angles. I have less exposure to moveDynamicMesh.
What does moveDynamicMesh do ?

But my suggestion would be try using suitable solver for continuously opening Window ( that will include all the angles for a single swing).
Solver may be moveDynamicMesh.
Tthere is difference between simulating opening window and open window at different angles.
As far as pimpleDyFoam is meant for rotating object (360 degree), and your window might not do full swing of 360. But yes unless you implement it with some innovative idea like run solver for 1/4th time step , then may be yes try using pimpleDyFoam.
This is only suggestion to you.
__________________
________________________________________
Regards,
CFDkid

It never gets easier You just get Better
kid is offline   Reply With Quote

Old   May 25, 2012, 05:10
Default
  #109
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 490
Rep Power: 9
samiam1000 is on a distinguished road
Dear Kid,

what I would like to do is to simulate an opening windows. What I am doing - in order to get this result - is to simulate the opening through different steps (e.g. from 0 to 15, from 15 to 30 and so on..), passing the solution thanks to the mapField feature..

The moveDynamicMesh stretches the cells and allows to simulate a continuos rotation: the point is that - at a certain point - the aspect-ration becomes to high and I get a `floating point' error.

I will try again.

Which is the tutorial that uses the pimpleDyMFoam and studies a rotating object? I can not find it, sorry.
Also, what about AMI?
samiam1000 is offline   Reply With Quote

Old   May 25, 2012, 05:24
Default
  #110
kid
Senior Member
 
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 8
kid is on a distinguished road
/tutorial/incompressible/pimpleDyFoam/propeller or mixer2D etc
else
/tutorial/incompressible/pimpleFoam/pimpleDyFoam/propeller or mixer2D

either ot the above location has tutorial for pimpleDyFoam, try propeller or other mixer2D.
(names might differ do not remember)

AMI is a feature introduced from OpenFoam-2 and above.
GGI was previously used now AMI. You can look more details on OpenFOAM web
http://www.openfoam.org/version2.1.0/ami.php
__________________
________________________________________
Regards,
CFDkid

It never gets easier You just get Better
kid is offline   Reply With Quote

Old   May 29, 2012, 22:11
Default
  #111
Member
 
liping_he
Join Date: Feb 2011
Posts: 35
Rep Power: 6
liping_he is on a distinguished road
Dear linnemann and all


I created a case by combining the interDyMFoam (tutorials/multiphase/interDyMFoam/ras/damBreakWithObstacle) and pimpleDyMFoam (tutorials/incompressible/pimpleDyMFoam/propeller) to achieve the simulation of impulse turbine. The screenshot is shown in attachment containing three nozzles and a runner.
And now, I want to calculate the efficiency. A great issue comes out HOW can i obtain the moment of runner. Any advices will be appreciated.
Attached Images
File Type: jpg turbine.jpg (78.2 KB, 104 views)
liping_he is offline   Reply With Quote

Old   May 30, 2012, 02:55
Default
  #112
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 490
Rep Power: 9
samiam1000 is on a distinguished road
Dear Liping,

let's do a step back. Are you simulating a solid body () that moves into a fluid domain?

Could you explain me how you get this? Could you share your case (just the dictionaries if you can't/don't want to share the mesh)?

You can either upload the files here or send them to my email (samuele.zampini@gmail.com).

Thanks a lot,

Samuele
samiam1000 is offline   Reply With Quote

Old   May 30, 2012, 03:16
Default
  #113
Member
 
liping_he
Join Date: Feb 2011
Posts: 35
Rep Power: 6
liping_he is on a distinguished road
Hi Stephane

Did you kown how to calculate the torque of runner.

Regards,

Liping.
liping_he is offline   Reply With Quote

Old   May 30, 2012, 03:27
Default
  #114
Member
 
liping_he
Join Date: Feb 2011
Posts: 35
Rep Power: 6
liping_he is on a distinguished road
HI Samuele,

This case is using to simulate dynamic mesh and multiphse flow. The dictionaries are attached.

regards,
Liping
Attached Files
File Type: zip DICT.zip (2.0 KB, 51 views)
liping_he is offline   Reply With Quote

Old   May 31, 2012, 04:25
Default
  #115
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi Liping,

Have a look at the motorbike tutorial.

Add the following 4 lines in your controlDict file

functions
{
#include "forceCoeffs"
}

Copy and put the forceCoeffs file in the system directory.

Then you will obtain a file with forces (thrust) and moment (torque).

Regards,
Stephane.
openfoam_user is offline   Reply With Quote

Old   May 31, 2012, 06:28
Default
  #116
Member
 
liping_he
Join Date: Feb 2011
Posts: 35
Rep Power: 6
liping_he is on a distinguished road
Hi Stephane,

I exactly follow the steps you said,
But I only got Cd Cl and Cm. I dont know what these parameters means.

And I added the following code into forceCoeffs file
Quote:
forces
{
type forces;
functionObjectLibs ("libforces.so");
patches ("motorBike.*");
rhoName rhoInf;
rhoInf 1025;
CofR (-1 0 0);
outputControl timeStep;
outputInterval 1;
log true;
}
This time I got the forces and moment. But I dont know the axis of moment, and how to set the axis of moment. I want to obtain the torque of Y axis and i dont know how to set. What the parameters CofR, liftDir, dragDir, pitchAxis,magUInf, lRef.and Aref means and how to set them. Thanks a lot.

regards.
liping
liping_he is offline   Reply With Quote

Old   May 31, 2012, 06:47
Default
  #117
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi Liping,

add following lines

liftDir (1 0 0); // lift direction
dragDir (0 0 1); // drag direction (thrust)
pitchAxis (0 1 0);

Stephane.
kid likes this.
openfoam_user is offline   Reply With Quote

Old   June 11, 2012, 05:35
Default
  #118
Member
 
wided
Join Date: Jul 2010
Posts: 54
Rep Power: 7
wiedangel is on a distinguished road
Dear all,
I am using AMI for some time now to simulate a pitching airfoil (with a cylindrical leading-edge), the results look ok as long as the time step stays small at the beginning of the simulation.
What I never paid attention to are the weights, Can someone please explain to me (us) what are they for and how one knows that they are correct or not?

Thank you !

PS: I will be happy to post some of my results if any one is interested in them
wiedangel is offline   Reply With Quote

Old   June 27, 2012, 19:01
Default
  #119
Member
 
Jason Eason
Join Date: Jan 2010
Location: Portage, Michigan
Posts: 44
Rep Power: 7
JulytoNovember is on a distinguished road
My cellzone has some weird things happening. When I run the blockMesh the mesh has no errors, also checkMesh is fine. Then I viewed the mesh with paraFoam before running my case and everything is fine. However; when I run my topoSets the cellzone here is the result. My case is exactly the same as the propeller case. The 2 differences are my case was created with blockMesh, and I have a rotor not a propeller. Does anyone know what the problem is?.
Attached Images
File Type: png edge.png (9.2 KB, 44 views)
__________________
Debian Squeeze - OpenFOAM-2.1.x, Paraview-3.12.0

Last edited by JulytoNovember; June 29, 2012 at 14:44.
JulytoNovember is offline   Reply With Quote

Old   June 28, 2012, 05:25
Default
  #120
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi,

I have some problem to converge my propeller case using AMI.

Can someone look at my fvSolution and fvScemes files and give me some advice about how to improve the convergence (and for pressure in particular). Thanks in advance.

Regards,
Stephane.
Attached Images
File Type: jpg residuals.jpg (51.0 KB, 63 views)
Attached Files
File Type: txt fvSchemes.txt (1.5 KB, 23 views)
File Type: txt fvSolution.txt (1.9 KB, 25 views)
openfoam_user 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
UDF compiling problem Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43
Gambit - meshing over airfoil wrapping (?) problem JFDC FLUENT 1 July 11, 2011 05:59
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13
Is this problem well posed? Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52


All times are GMT -4. The time now is 10:26.