How to calculate grid width in control volume

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

November 15, 2010, 13:03
How to calculate grid width in control volume
#1
Member

Javier Basurco
Join Date: Jan 2010
Location: Rio de Janeiro, Brazil
Posts: 33
Rep Power: 7
Dear Foamer's

I would like to know is there any class to calculate the cell width of all grid?
I need this distance to calculate a step function while the solver is running. This help me to calculate a properties weighted in this distance.

Somebody can help me?

Respectfully
Javier Basurco
Attached Images
 control volume.jpg (16.6 KB, 11 views)

 November 16, 2010, 06:26 #2 Senior Member   Kathrin Kissling Join Date: Mar 2009 Location: Besigheim, Germany Posts: 134 Rep Power: 8 Dear Javier, if you are using cubical cells it is really easy : you need to grab the mesh and then you can go pow(mesh.V().1/3) which gives you the cell width. If you don't have those values, you might need to get the distance between the cell center (mesh.C()) and the centers of the cell's faces(mesh.Cf()). Than you might estimate the cell width. Or you can go to the edges directly if you have access to the primitiveMesh myMesh.cells()[i].cellEdges() gives you a labelList ( j, k, l, m, n, o, p, ...) of the edges of the cell i. Then you need to check out the edges from myMesh.edges()[j] (just for example) and then you can acces the length of the edge by myEdge.mag() Hope this helps Kathrin PS: How to get the mesh: It depends on the environment. Can you give us a litte snapshot from the code you want to implement your function? mm.abdollahzadeh and m_mousavi88 like this.

November 16, 2010, 09:08
#3
Member

Javier Basurco
Join Date: Jan 2010
Location: Rio de Janeiro, Brazil
Posts: 33
Rep Power: 7
Dear Kathrin,

I did my mesh in icemcfd ANSYS 12.1. I exported the mesh to fluent and then convert to openfoam, for now is not problem. The solver that I am working is level set method, for two phase flow. Maybe do you hear some thing. The level set method is used to reconstruct the interface between two fluids. In OpenFOAM is there another method similar VOF method.
The level set method obtain a distance that will be stored in the nodes of a cell and from the difference of level set distance to the normal edge are calculated values of density and viscosity are used in the equation of conservation of momentum.
I think that I am not a cubical cell maybe hexahedral trying to converve a structural mesh.
Could you explain me better how can go to the edges directly if I have access to the primitiveMesh.

I look a forward to hearing from you

Respectfully
Javier Basurco
Attached Images
 duto2metros.jpg (96.8 KB, 40 views)
Attached Files
 Level set.pdf (52.2 KB, 26 views)

 November 16, 2010, 13:02 #4 Senior Member   Kathrin Kissling Join Date: Mar 2009 Location: Besigheim, Germany Posts: 134 Rep Power: 8 Hi Javier, ok I know about the Level-Set Method. What you want to do is implement the Heavyside-Function. Okay let my try to code without compiling.... mesh is defined as fvMesh or primitiveMesh or ... edgeList edg = mesh.edges(); forAll(edg, edgeI) { scalar width = edg[edgeI].mag(); } Where the scalar width gives you the length of the edge. I don't know in which context you need it. Whether as value or field or whatever... Can you give me a little more information? Best Kathrin

 November 16, 2010, 13:58 #5 Member   Javier Basurco Join Date: Jan 2010 Location: Rio de Janeiro, Brazil Posts: 33 Rep Power: 7 Dear kathrin, In the first instance thanks for your help. I am trying to implemented the Heaviside function. The H-function is used to smooth the density and the viscosity at the interface over a width of delta_n. In several reference, defined this delta_n like a thickness of the interface (Sussman et al, 1998). The delta_n is 1.5 of of grid with (Shu et al, 2007) was implemented in OpenFOAM. I think that this function is a value to do a weighted medium between the densities of two fluids to obtained a rho that was used in ddt(rho, U) and rho == rho2 + (rho1 - rho2)H. My first question is have been a possibility to obtain the minimum distance between all edge from volume control. My second question, what is the meaning of edgeI it is related to axis "y" maybe? is there another edgeII o edgeIII? My deep regards Once again thanks for your help Respectfully Javier Basurco PD.: If you need the reference, I could send you this information.

 November 24, 2010, 13:40 #6 Senior Member   Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 12 Since what you really want is the effective cell size in the surface normal direction and your mesh is unstructured, your best approach is probably something along the lines of what can be found here: \$FOAM_SRC/turbulenceModels/incompressible/LES/SpalartAllmarasIDDES/IDDESDelta.C You want to take the dot product of the cell-to-face-centre vectors with the level set surface normal direction and I would suggest you use some form of projected area weighting to get separate averages of all the positive and negative dot products. Then sum the absolute value of the negative and positive averages instead of just using 2x the maximum. What you are looking for is the average thickness of the cell in the direction of the level-set surface. Assuming the faces are flat, the above method will give you something close to the exact answer. If you want the maximum extent of the cell, then just do the same with the cell-centre-to-vertex vectors, but sum the maximum of the positive and abs(negative) dot products. To access cellPoint addressing: mesh.cellPoints().

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post kiran OpenFOAM Post-Processing 2 September 12, 2010 12:59 gaottino OpenFOAM Native Meshers: blockMesh 7 July 19, 2010 14:11 Josh ANSYS Meshing & Geometry 4 May 20, 2010 13:40 xujjun CFX 9 June 9, 2009 07:59 Gernot FLUENT 0 August 26, 2005 13:21

All times are GMT -4. The time now is 18:47.