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   July 3, 2012, 03:10
Default
  #121
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi,

I have improved the convergence using:
grad(p) cellLimited leastSquares 1;// (new)
instead of
grad(p) Gauss linear corrected;// (old)

Any other advice ?

Stephane
kiddmax likes this.
openfoam_user is offline   Reply With Quote

Old   September 20, 2012, 07:59
Default
  #122
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi OF-users,

which maxCo are you reaching for pimpleDyMFoam computation with AMI patches ?

What manner do you use to increase maxCo ? Manually or a more sophisticated method ?

Regards,
Stephane.
openfoam_user is offline   Reply With Quote

Old   September 20, 2012, 11:52
Default
  #123
New Member
 
Alexander Tagirov
Join Date: Feb 2011
Location: Moscow, Russia
Posts: 7
Rep Power: 6
Randomizer is on a distinguished road
What about your mesh non-orthogonality? In your fvSolution file you set nNonOrthogonalCorrectors to zero. Is your mesh orthogonal?
Randomizer is offline   Reply With Quote

Old   September 20, 2012, 11:55
Default
  #124
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Quote:
Originally Posted by openfoam_user View Post
Hi OF-users,

which maxCo are you reaching for pimpleDyMFoam computation with AMI patches ?

What manner do you use to increase maxCo ? Manually or a more sophisticated method ?

Regards,
Stephane.
Hi,

I could use Co numbers up to 1. At the beginning of the simulation the max Co increases a lot, so the solver decreases the timestep. Later, the timestep as well as the meanCo increases. At the beginning, using 0.5 is a good start. Later switching to 1 or maybe higher is also possible. meanCo is more important than maxCo. And yes, I increase it manually...
__________________
CFD= Cleverly Formatted Data
Attesz is offline   Reply With Quote

Old   September 20, 2012, 11:57
Default
  #125
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Quote:
Originally Posted by openfoam_user View Post
Hi,

I have improved the convergence using:
grad(p) cellLimited leastSquares 1;// (new)
instead of
grad(p) Gauss linear corrected;// (old)

Any other advice ?

Stephane
did you try cellLimited Gauss Linear 1?

cellLimitation helped you to have better convergence. leastSquares is slower than linear in my opinion.
__________________
CFD= Cleverly Formatted Data
Attesz is offline   Reply With Quote

Old   September 21, 2012, 02:17
Default
  #126
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi,
checkMesh gives me:

*Number of severely non-orthogonal faces: 182.
Non-orthogonality check OK.
<<Writing 182 non-orthogonal faces to set nonOrthoFaces

So you suggest to set nNonOrthogonalCorrectors 1;

I will try the schemes you suggest me to have a better convergence. Thanks.

Some words about maxCo.
Now I have a simulation that seems to run well. In my controlDict file I have set maxCo = 2 (like the propeller tutorial case). And the log file gives me: Courant Number mean: 0.00127652 max: 1.99524. So you say to increase manually the maxCo in order to have obtain a Courant Number mean = 1 ! Is it right ?

Regards,
Stephane.
openfoam_user is offline   Reply With Quote

Old   September 21, 2012, 02:35
Default
  #127
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
modify nNonOrthogonalCorrectors to 1 or 2 only if you have problems with the pressure residuals. this correction may help, but not too much as I experienced. It increases the calculation time as well.

maxCo can be adjusted during run, too. Set it initially to 1, but your meanCo is 0.001 which is quite low.

are you using adjustable time stepping?



Quote:
Originally Posted by openfoam_user View Post
Hi,
checkMesh gives me:

*Number of severely non-orthogonal faces: 182.
Non-orthogonality check OK.
<<Writing 182 non-orthogonal faces to set nonOrthoFaces

So you suggest to set nNonOrthogonalCorrectors 1;

I will try the schemes you suggest me to have a better convergence. Thanks.

Some words about maxCo.
Now I have a simulation that seems to run well. In my controlDict file I have set maxCo = 2 (like the propeller tutorial case). And the log file gives me: Courant Number mean: 0.00127652 max: 1.99524. So you say to increase manually the maxCo in order to have obtain a Courant Number mean = 1 ! Is it right ?

Regards,
Stephane.
__________________
CFD= Cleverly Formatted Data
Attesz is offline   Reply With Quote

Old   September 21, 2012, 02:46
Default
  #128
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi,
yes I use adjustable time stepping.

As you can see my maxCo = 2 and my resulting meanCo is around 0.0012.
I can only play my the maxCo number.

So you suggest to increase maxCo till I get meanCo = 1 ! I hope my computation won't blow up.

Regards,
Stephane.
openfoam_user is offline   Reply With Quote

Old   September 21, 2012, 02:47
Default
  #129
New Member
 
Alexander Tagirov
Join Date: Feb 2011
Location: Moscow, Russia
Posts: 7
Rep Power: 6
Randomizer is on a distinguished road
I guess you could set nNonOrthogonalCorrectors 2; if it won't make the calculations to long
Randomizer is offline   Reply With Quote

Old   September 21, 2012, 02:48
Default
  #130
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
No, absolutely not. I said decrease maxCo to 1. if you have conv. errors, attach the conv. curve here.

Quote:
Originally Posted by openfoam_user View Post
Hi,
yes I use adjustable time stepping.

As you can see my maxCo = 2 and my resulting meanCo is around 0.0012.
I can only play my the maxCo number.

So you suggest to increase maxCo till I get meanCo = 1 ! I hope my computation won't blow up.

Regards,
Stephane.
__________________
CFD= Cleverly Formatted Data
Attesz is offline   Reply With Quote

Old   October 24, 2012, 10:49
Default
  #131
Member
 
Jason Eason
Join Date: Jan 2010
Location: Portage, Michigan
Posts: 44
Rep Power: 7
JulytoNovember is on a distinguished road
My AMI works with blockMesh, I saw someone stated there was a problem in a previous post. My AMI is made of internal faces, then using topoSet , I created my patch for my AMI. I think the problem is the topoSet, previously I created a patch for my AMI. After the topoSets ran my AMI was incorrect, when initially it was correct.
__________________
Debian Squeeze - OpenFOAM-2.1.x, Paraview-3.12.0
JulytoNovember is offline   Reply With Quote

Old   April 4, 2013, 13:02
Default Problems combining Salome meshes & pimpleDyMFoam & AMI interfaces
  #132
New Member
 
arnau1985's Avatar
 
Arnau
Join Date: Jan 2012
Posts: 17
Rep Power: 5
arnau1985 is on a distinguished road
Hello everyone,

I am experiencing some troubles when running cases with pimpleDyMFoam and AMI meshed with Salome. These cases worked properly with GGI, so I assume the mesh is OK.

Does anybody have any case or tutorial I can use as a reference to fix my problems, please? The OpenFOAM tutorials, meshed with snappyHexMesh, blockMesh and so on, are not being very helpful. I would really appreciate it.

Thanks a lot,

Arnau.
arnau1985 is offline   Reply With Quote

Old   April 11, 2013, 07:48
Default AMI query
  #133
Member
 
Andrew Glassby
Join Date: Sep 2009
Posts: 65
Rep Power: 7
ADGlassby is on a distinguished road
I'm looking at possibly using AMI for a model I am putting together but I want to be sure this is the right approach.
Looking at the propellor example in the OPENFOAM tutorials the cylindrical AMI1 and AMI2 regions are situated with their axes oriented with the flow direction. What about if i wanted to model a centrifugal device where the exit is in the radial direction? or the flow field is actually across the axis (like a quarter turn ball valve) would AMI be an appropriate technique to use?

Trust this has a straight forward response :-)

Kindest Regards

Andrew
ADGlassby is offline   Reply With Quote

Old   April 11, 2013, 09:56
Default
  #134
New Member
 
Alexander Tagirov
Join Date: Feb 2011
Location: Moscow, Russia
Posts: 7
Rep Power: 6
Randomizer is on a distinguished road
Hi,Andrew, i don't see any problem with using AMI with your case. AMI is just an interface between 2 patches with differnt mesh topology, and it shouldn't care whether the flow is axial or not. Mesh movement is provided by dinamic mesh library, and it works with non-axial flows.
Randomizer is offline   Reply With Quote

Old   April 11, 2013, 10:45
Default
  #135
Member
 
Andrew Glassby
Join Date: Sep 2009
Posts: 65
Rep Power: 7
ADGlassby is on a distinguished road
Hi Alexander, thanks for your response, just what I was looking for. I just didn't want to go through the effort of setting up a new model only to find that it was the wrong technique to use! I'll look more closely at this now.

Regards

Andrew
ADGlassby is offline   Reply With Quote

Old   April 11, 2013, 15:48
Default
  #136
New Member
 
Alexander Tagirov
Join Date: Feb 2011
Location: Moscow, Russia
Posts: 7
Rep Power: 6
Randomizer is on a distinguished road
Hi,Arnau, what exactly is not working? Does the calculation crash after some iterations? Or it doesn't start?
Randomizer is offline   Reply With Quote

Old   April 20, 2013, 17:16
Default
  #137
Member
 
Andrew Glassby
Join Date: Sep 2009
Posts: 65
Rep Power: 7
ADGlassby is on a distinguished road
Alexander,

I wonder if you could help me? I am trying to implement the AMI methodology using a snappyHexMesh generated mesh but I am experiencing problems introducing the AMI interfaces. My mesh becomes cut at the position of the AMI interface. How can I introduce the AMI interfaces in the snappyHexMesh procedure?

I tried introducing the cylinders into the STL of the whole geometry. should I produced a separate geometry STL file for the AMI interface cylinders? if so WHEN and HOW should this be done?

My geometry is not TOO complex but I have curves which look quite involved in producing with simple blockMesh that's why I'm using snappyHesxMesh since I can use CAD to pro due my STL geometry file.

I'm really looking for some general advice/pointers since I THINK I'm almost there and just need the last little pointer (hopefully!!)

Best Regards

Andrew
ADGlassby is offline   Reply With Quote

Old   April 21, 2013, 13:04
Default
  #138
New Member
 
Alexander Tagirov
Join Date: Feb 2011
Location: Moscow, Russia
Posts: 7
Rep Power: 6
Randomizer is on a distinguished road
Andrew, did Iunderstand correctly that you make your whole mesh with snappyHexMesh and then try to cut it with surfaces? This way it won't work, I think. I would recomend you to create two parts of your mesh (divided by ami surfaces) separately. Each part should have one of the ami surfaces. Then you can union the with mergeMeshes utility, for example. I do this way for my ami cases, but I use Salome. Hope it helps.
Alexander.
Randomizer is offline   Reply With Quote

Old   April 21, 2013, 14:39
Default
  #139
Member
 
Andrew Glassby
Join Date: Sep 2009
Posts: 65
Rep Power: 7
ADGlassby is on a distinguished road
Hi Alexander, What I'm trying to achieve is something similar to the mixerVessel2DAMI example. My problem is that I have used snappyHexMesh to develop the mesh and I'm not understanding how to introduce the AMI interface ring like in the mixer geometry. I'm going to have a look at building the mesh using blockMesh (since it's not THAT complex really) and then when I get it working this way I'll have a look at SnappyHexMesh again since I can see the advantages of being able to work up my geometry in a CAD package.

I've attached a jpeg of part of my geometry, the moving bit.

It would be great if you had any pointers based on the mixerVessel2DAMI example as I could then apply any pointers from there.

Thanks again for your kind help!

Best Regards

Andrew
Attached Images
File Type: jpg Domain.jpg (59.1 KB, 40 views)
ADGlassby is offline   Reply With Quote

Old   April 21, 2013, 16:18
Default
  #140
New Member
 
Alexander Tagirov
Join Date: Feb 2011
Location: Moscow, Russia
Posts: 7
Rep Power: 6
Randomizer is on a distinguished road
Andrew, the simplest way is to divide our geometry in two parts, separated by this ami "ring". And then connect them together in one case. Just choose some ring inside your geometry so the moving part would rotate around it (like in mixerVessel2DAMI case). In your case this ring should be inside the circle on your picture. So each mesh part would have a patch, which will represent the ami interface.
Randomizer 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 13:16.