Hi everyone. I'm testing Fluent on the Poiseuille problem (long straight tube, Newtonian fluid, parabolic inlet velocity profile, zero pressure outlet) both with bricks and tetrahedral elements. I have been told that Fluent works fine with tetra elements, but when I check the pressure loss between the inlet and the outlet, with bricks I get a value that is close to the analitic solution even with coarse grids and a thin boundary layer, while with tetras I get a pressure loss that is near to double than the correct one, even with grids that are more than double finer that the one made of bricks. I'm trying to change convergence, solution methods, to change outlet pressure value, but with no result. I also tried to check the pressure loss between two internal surfaces, to avoid boundary effects, but I coulnd't find the correct values. Can anyone who knows give me a hint? Thanks a lot

Luca

Did you use 2nd oder discretisation? And did you also resolve the boundary layer in the tetrahedral case?

Volker

Thanks a lot, I'm working on discretization order and boundary layer for tetrahedreal case, and also on upwinding scheme, and things are getting better, even if not yet precisely correct. I am looking forward to get the right numbers!

(1). I am glad that someone is doing this test. (2). There is no question that the brick mesh is more accurate than the tet mesh. (3). If you Change the stream-wise mesh size distribution, you can observe the change in stream-wise wall skin friction distribution. Run a few meshes with different stream-wise mesh distributions, this will give you some ideas about the results. (4). I think, the readers here would be very interested in your results related to the mesh size, distributions, and the accuracy.

It's also nice to check this simple case with the equations of momentum. You have the pressures, the velocities and all the forces at the tube. Are there differences between the different cell-types ?

I'm using a cilynder of L=10*D. Tetrahedral mesh size is dependent on how many nodes I use to discretize the two edges on the bases of the cilynder. So far I used three different interval counts, of 20, 35, 50. Boundary layer was set to have a first row of D/33 or D/50 (depends on the case), a growth factor of 1.25 and a number of rows so that the most interior element is nearly squared (e.g. 4 for the 50 case, and 6 for the 20 case). So far I have noticed that even with the finest mesh (base mesh interval count of 50, resulting in 41133 nodes), if I don't include a boundary layer the pressure drop is overestimated by a 25% in respect to the analytical results. With the 20 case, the error is only 2% with previously described boundary layer (resulting in 11320 nodes), while 40% without boundary layer (3313 nodes). (I realize that these results are messed up, but I'm going to put some order). All the simulations were performed with segregated approach, second order discretization and upwinding, and SIMPLE coupling algorithm. Parabolic velocity inlet profile and zero pressure outlet. My question is: how can I change stream-wise mesh distribution without changing the overall mesh distribution? The number of triangles on the wall is implicitly set with the discretization of the base edges. Thank you all for your attention!

Luca