Hello,
i have a convergence problem in OpenFoam on a high Re flow of 10^5. I'm using simpleFoam as solver and i have a noncompressible flow. My mesh has two inlets and 8 outlets. Perhaps someone has a hint for me, to increase stability. I use the following boundary conditions.
- U: fixedValue for Inlet, inletOutlet for outlets
- p: zeroGradient for inlet, fixedValue for outlets
Additionally i initialized the volume with potential foam. For the first simulations everything worked fine, but a small change within the mesh decreased my stability that big, that i am not possible to get a converged simulation anymore.
Dear Hendrik,
I agree with Alexander, try to use zeroGradient insetead of inletOutler. Futhermore try to run the simulation without the turbulence model and reach a stable condition. Than turn on the turbulence.
Furthermore, which values for y+ do you have?
Franco
Interesting. Thank you both so far. The Problem is I already use laminar as turbulence model. Also i used the inletOutlet because the i could only reach a convergence if i allowed the back stream.
What do you mean with y+? If this is the courant number... I use an steady state solver. I also tried to use the pimpleFoam with courant number of nearly 1.
Have you checked on your relTol in your fvSchemes for solving your fields? May be it's some value defined, if so set it as zero that can allow the problem to converge. Try using relaxation factors for your p.
While decreasing ur mesh, have u run checkmesh utility? It helps to get an idea about your mesh whether it is tested ok or not
Best Regards
Akr
I've encountered another cause for this problem. The problem related to outlet boundary conditions plagued me for half a year. The fixedValue boundary condition for the pressure on outlet severely affects convergence in case of backflow. With this boundary condition simpleFoam solver converges poorly and pimpleFoam solution blows up due to the infinitely accelerating backflow on outlet. Solution develops nonphysical flow near outlet even in case of the inletOutlet condition for velocity with zero vector for backflow. This happens because the internal static pressure decreases when the velocity increases and it stays constant on outlet boundary patch in case of the fixedValue condition. This leads to pressure gradient on boundary which accelerate liquid even further and lowers internal pressure and so on.
I solved this problem by using totalPressure condition on outlet. The totalPressure boundary condition on outlet impose the fixed value condition for pressure p = p0 in case of outflow and p = p0 - 0.5*U^2 in case of inflow (the density is omitted because in OpenFOAM pressure in incompressible solvers is actually p/rho). Under this condition there is no nonphysical pressure gradient on boundary and solution converges pretty well.
Hi, I have the same issue. My setup has one inlet and two outlets. At the outlets I get some vortices and backflow after some simulation time. I used fixedValue for Prgh at the outlets with PressureInletOutlet for the velocity.
I am wondering if you solved the problem.
The solution is shown in the video on this page: http://bit.ly/35Svcr0. The page shows an example that one can download. The conditions are set to
outlet:
- velocity: “pressure inlet outlet velocity”
- pressure: “total pressure” = 0
inlet:
- velocity: “volumetric flow rate inlet” = 0.1
- pressure: zero gradient
The video is on youtube https://www.youtube.com/watch?v=2cywdPboXyw
May that helps
Hendrik
Dear Hendrik Otto,
Thanks a lot for your reply. I am wondering if you have experience with multiphase solvers.
Best Regards,
Abdallah Ghazal
- Badges
- Science topic