CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Pointwise & Gridgen

Anisotropic tetras

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

Like Tree2Likes
  • 2 Post By cnsidero

Reply
 
LinkBack Thread Tools Display Modes
Old   January 27, 2013, 02:33
Default Anisotropic tetras
  #1
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,906
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Please refer to following link (specially Page # 9 and Fig. #10). Do you think quality is acceptable for the high quality CFD simulation? I am not saying it is wrong, but I am interested to find out mathematical reasoning (from CFD point of view in terms of accuracy, convergence etc) behind this. As it will help me to create the less dense mesh on the body of the wings with large length to chord ratio.


http://www.pointwise.com/T-Rex/Pointwise_T-Rex.pdf
Far is offline   Reply With Quote

Old   January 27, 2013, 10:40
Default
  #2
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 368
Rep Power: 12
cnsidero is on a distinguished road
Far,

Generally speaking, solution accuracy, regardless of mesh type, is a function of the chosen solver numerical methods. In my review of the literature concerning tet element quality, a commonly used metric is the maximum included dihedral angle. As max included angle increases, tri/tet quality decreases. You will notice that anisotropic tris/tets from Pointwise have max included angles generally < 90. So by the max angle metric they are of high quality.

Continuing, there is one additional metric to consider. The deviation angle between the face normal and the vector connecting the cell centers on each side of the face. If you have a hard time understanding this, simply draw a picture of a long, narrow rectangle and split at two opposing corners to give you two aniso tris. First draw the normal vector of the long hypotenuse - this is the face vector. Second find the cell center of each triangle and draw a line connecting the two. The angle between them is that deviation angle.

Large deviation angles commonly causes issues for cell-centered, finite volume based CFD solvers - the method used by many of the popular commercial codes. The reason being is that when one wants to compute the fluxes on a face - a necessary procedure for finite volume method - you need to compute face information by interpolating the adjacent cell center information. In particular, when you need the gradient at the face center, the simplest way is to compute the gradient along the adjacent cell centers vector. This is where deviation angle comes into play. As the adjacent cell center vector deviates from the face normal (direction of the gradient at face center), the interpolated gradient direction is clearly not aligned and likely not representative of the face normal gradient. Hence, error and solution stiffness start coming into play.

Now you can attempt to rectify this by interpolating the gradient from the cell-center to the face-center a little more intelligently. It's called the non-orthogonal correction to the gradient. There's various ways to do it, it's best to dig around in the literature if you're interested. In addition, the correction is usually added explicitly, ie. to the RHS of the linear system, meaning it can make solution convergence more difficult.

Where I've seen these meshes used most successfully is with vertex-centered finite volume or finite element based solvers. It seems the numerics lend themselves better to stretched tet meshes and the solver writers are trying to consider them during algorithm development.

Most finite volume based solvers (cell centered or vertex centered) and users would still prefer to stay away from stretched tet meshes, partly because of the unknown behavior they might incur but most simply because they contain lot more cells. Pointwise addresses this by allowing the combination of anisotropic tets into prisms***. For every three neighboring anisotropic tet you can make one prism. Ideally, if the mesh was initially 100% aniostropic tets and every triplet could be combined you would get a two thirds (67%) reduction in cell count. First, no mesh has 100% aniostropic tets and second not every anisotropic tet can be recombined. In practice, Pointwise's aniostropic combination algorithm typically reduces the cell count between 55-60% and I've seen it higher sometimes. This procedure gives you the desired prisms in the boundary layer while significantly reducing the cell count. The aniso tet combination method in Pointwise can combine ansio tets into prisms anywhere in the boundary layer - it doesn't require each prism layer to be complete before moving to the next one. This is how it achieves such high combination percentages.

-Chris

*** The anisotropic combination algorithm is invoked during CAE export. Solvers that support mixed-element meshes (Fluent, OpenFOAM, CGNS, etc) will have a check box that says "Combine Anistropic Tetraheda" option during exporting the mesh to the solvers format. The Pointwise message window will report the combination stats after export.
Far and Hybrid like this.
cnsidero is offline   Reply With Quote

Old   January 27, 2013, 11:27
Default
  #3
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,906
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Thankyou Chris for very detailed and informative reply covering meshing from solver point of view. It is simply great.

Once again thankyou. Have a nice day.
Far is offline   Reply With Quote

Old   February 1, 2013, 12:47
Default
  #4
Senior Member
 
Ali
Join Date: Jan 2012
Location: Pakistan
Posts: 100
Rep Power: 7
Hybrid is on a distinguished road
Thanks Chris for such an expert opinion.

Will you help me, how to improve quality of unstructured meshes in Pointwise? I face skewness angle about 1.0 and hardly achieve prisms.

How to make prisms?
__________________
Best Regards
Ali


Hybrid is offline   Reply With Quote

Old   February 1, 2013, 12:53
Default
  #5
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,906
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Do you need hybrid mesh?

You can get prisms using extrude option
Far 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
anisotropic porosity in CFX Chander CFX 19 June 17, 2014 04:51
Anisotropic Tetrahedral Meshing using Gridgen? Turbomachinery Pointwise & Gridgen 2 May 7, 2007 07:13
Anisotropic Thermal Conductivity Saturn CFX 4 January 30, 2007 13:34
Help for modeling of anisotropic porous media, thx TobeFlowMaster FLUENT 10 January 31, 2005 12:13
Anisotropic subgrid model (LES) h.jordi Main CFD Forum 1 August 29, 2002 15:49


All times are GMT -4. The time now is 18:11.