Multielement airfoil analysis
hi maruthamuthu_venkatraman
my self NAVEEN from INDIA...i hav completed my naca 0012 airfoil analysis case in openfoa 1.4.1 and 1.5....i got good results in both the versions...thanks for your suggestions....now i am doing MTech project on multielement airfoil analysis with double slotted flaps and i hav completed my grid in gambit(c-grid) and now i need to solve in openfoam...i am getting some errors like this during solving in openfoam 1.4.1 #0 Foam::error::printStack(Foam::Ostream&) in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #2 ?? in "/lib64/libc.so.6" #3 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #4 Foam::fvMatrix<double>::solve(Foam::Istream&) in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libfiniteVolume.so" #5 main in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/simpleFoam" #6 __libc_start_main in "/lib64/libc.so.6" #7 Foam::regIOobject::readIfModified() in "/home/openfoam14/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/simpleFoam" can u give me some suggestions whare i am going wrong and also suggest how to set boundary conditions..... |
Quote:
I was just having a look around for useful/interesting discussions about external aerodynamics on unstructured grids, and I found this old but quite interesting tread...So, my question is: how did you obtain a so low max-skewness value on a 3D tetrahedral mesh? I think that my case is pretty different (bluff-body instead of streamlined-body, much larger mesh, etc.) but, however, using ANSA and/or Tgrid till now I was not able to reach max-skewness values lower than 1.8/2 ... Thank you in advance Best Regards V. |
My doubt is: did you try to use
leastSquares or cellMDLimited leastSquares 1 for gradients? |
Hi V,
Quote:
As an example... The mesh you commented on was generated in Gambit, at the moment I am using Pointwise and I get a max skew of 0.75-0.8... :o Hi Alberto, Quote:
maddalena |
Thanks Maddalena...What you're saying is a big truth (I mean the need for a big amount of patience in building good quality meshes). Anyway, I've never heard about this Pointwise mesher: is it for free? Is it (in your opinion) better or simpler to use compared to the most famous commercial alternatives (Gambit, ANSA, Tgrid)? Thank you once Again
Alberto, if this is a suggestion for me, thank you too, but the leastSquares option (whether limited or not) does not seem to give any benefits in my case (I don't know if it's something about the OF version: you and another guy of the forum started a little discussion about it in the tread concerning the second order schemes, but I didn't understand if the leastSquares option is well implemented in all the newest OF versions, namely from the 1.6 till now, or not). Till today the best combination I've found for the fvSchemes is: // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) cellMDLimited Gauss linear 1; } divSchemes { default none; div(phi,U) Gauss linearUpwindV cellMDLimited Gauss linear 1; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(R) Gauss linear; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default Gauss linear limited 0.5; // laplacian(nuEff,U) Gauss linear corrected; // laplacian((1|A(U)),p) Gauss linear corrected; // laplacian(DkEff,k) Gauss linear corrected; // laplacian(DepsilonEff,epsilon) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default limited 0.5; } fluxRequired { default no; p ; } // ************************************************** *********************** // Curiously, this leads to good convegrence (and, indeed, to quite nice flow features description) only for the 35° slant case of the Ahmed body...The 25° slant case reaches only partial convergence (the residuals first fall down, than grow up and start to oscillate around quite high values, from 10^-03 to 10^-02), but interestingly the results in terms of flow visualization and aerodynamic force coefficients seem to be not so far fom the experimental ones (and also from other RANS steady-state studies I've found in the literature). Finally, the above mentioned settings lead (for both slant configurations) to a significant underprediction of the pressure-drag coefficient in the nose region of the body (about 0.0045 vs. 0.02 from the experiments), whether the drag contribution from the other body-components (lateral skin friction, slant and base pressure drag contribution) are much more coherent both with the experimental data and with previous numerical studies. Best Regards Vesselin (V sounds too much lke "V for Vendetta" ;) ) |
Hi,
Quote:
1. It is the software I knew better when I started to look for a new mesher; 2. It has a direct Pointwise -> OpenFOAM export 3. It has a good way to handle with cyclic patches, that is an important feature for me. That's it. However, I have not too much experience with other commercial grid mesher: only a couple of meshes with Gambit and with GridPro. And some (bad) experience with salome. Quote:
Cheers mad |
Quote:
Quote:
Best Regards Vesselin |
Quote:
The implementation is different in OF from OpenCFD and in -dev/-extend, since the weights are "area based" in the OpenCFD version, and distance based (which is standard) in -dev/-extend. Best, |
Quote:
Quote:
Thanks Vesselin |
Quote:
Usually Gauss linear is more stable than leastSquares. If you want to have a distance-based leastSquares in OpenCFD implementation, you can use extendedLeastSquares. Quote:
Best, |
Quote:
Quote:
Quote:
Quote:
Thanks for all the comments Vesselin |
I asked already elsewhere, but is the mesh quality low (what does checkMesh say?).
Hint: hex-dominant meshes are so nice ;-) |
Quote:
points: 357845 faces: 3218365 internal faces: 3105296 cells: 1527609 boundary patches: 10 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 0 prisms: 213225 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 1314384 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology symmetry 22600 12584 ok (non-closed singly connected) floor 14660 7609 ok (non-closed singly connected) inlet 426 242 ok (non-closed singly connected) outlet 432 245 ok (non-closed singly connected) side 2228 1204 ok (non-closed singly connected) top 1648 910 ok (non-closed singly connected) body 54899 27768 ok (non-closed singly connected) nose 8704 4461 ok (non-closed singly connected) slant 3948 2058 ok (non-closed singly connected) back 3524 1841 ok (non-closed singly connected) Checking geometry... Overall domain bounding box (-1.26 0 0.1945) (6.27 1.44 1.1945) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (1.709e-17 -1.03646e-15 -2.57399e-16) OK. Max cell openness = 3.24287e-16 OK. Max aspect ratio = 5.97752 OK. Minumum face area = 1.71072e-06. Maximum face area = 0.0159908. Face area magnitudes OK. Min volume = 1.10751e-09. Max volume = 0.000575106. Total volume = 10.7878. Cell volumes OK. Mesh non-orthogonality Max: 54.8744 average: 14.5203 Non-orthogonality check OK. Face pyramids OK. Max skewness = 1.98187 OK. Mesh OK. End Quote:
Thanks Vesselin |
1 Attachment(s)
Hi,
the mesh is OK. Quote:
The -extend 1.6 release has the reconCentral scheme, which should improve this. Some time ago I took the freedom of compiling it for 1.7.x (see attachment). You can use it as interpolation scheme (add the library to controlDict) with the cellLimited option for gradients. Quote:
Best, |
Quote:
Thank you once again Best Regards Vesselin |
Quote:
|
Quote:
Could you post your fvSolution and fvSchemes as well as your control dict for the case of NACA0012 aifoil? Do you have any picture showing the convergence history? Regards, Guilherme |
Dear Maddalena,
Have you managed to solve your convergence issues? Could you post your fvSolution, fvSchemes, controlDict? I am trying to simulate a cylinder M=0.07 and Re=2.2E5 with heat transfer over a fully rough wall with rhoSimpleFoam. Regards, Guilherme |
Quote:
I solved the problem posted above, and was not (only) a problem of fvSchemes and fvSolution. In any case, the right setup is not unique and must be refined for your case, that is indeed really different from what I have. A suggestion: if your solution does not converge, it is probably a matter of BC that are not correctly tuned. Enjoy mad |
Quote:
my main problem is that I use an old version of ANSA which has some difficulties to manage volumetric meshes above 3-3.5 milions of cells (this is, I guess, a kind of "communication bug" between the software and the RAM memory of the PC...I know that the latest 64-bit versions of ANSA do not have such a trouble)...So, if my problem grows up above this limit, I just have to switch to another meshing software:( In any case, I do prefer to manage wiith the surface mesh and the prisms b.l. with ANSA, and then fill the remaining volume with tetras using Tgrid: it's a matter of personal taste, simply I don't like how Tgrid deals with surface meshing and b. l. building... Best Regards Vesselin |
All times are GMT -4. The time now is 09:21. |