I have recently tried to simulate the acceleration due to friction in the a micro channel flow. I find that even though the peak mach numbers match up with previous experiments, the jet breakdown occurs much sooner than expected.
This gives birth to the question on whether the making the grid finer near the nozzle exit and continuing till the boundary would help carry on the jet further, how influential would this be.
In my understanding, having a high aspect ratio cell would lead to more dissipation, can anyone help me in understanding how much effect would the cell aspect ratio would have on the jet breakdown.
thanks,
This is a multi-fold question. The primary issue is the type of turbulence modeling you are using - LES is best, but perhaps not practical. From your problem description, you should be using at minimum a 2-equation model such as Menter's SST (fully 3D). Even better would be a hybrid URANS-LES approach - even DES would help. Next is your spatial scheme and its inherent dissipation. If you are using a commercial CFD code, watch out as dissipation is added for code robustness, but it can interfere with your solution. With respect to the mesh, it depends on the problem. A grid study is typically necessary, and I recommend it here, though you can do a rapid assessment in 2D steady to determine the mesh dependency before moving to 3D unsteady. Make sure that your y+ at the wall is less than 1 and your stretching ratio gives you 35-50 points in the boundary layer. For aspect ratios, obviously a 1:1:1 is optimum, but usually not practical. Do that mesh refinement study (halve the mesh in each direction and compare convergence and important quantities until they change less than what you can tolerate in your simulation). Set any dissipation terms to the lowest you can set them without loss in stability.
Dear Professor Smith,
Thank you very much for your answer. Sincere apologies for responding after a year.
I would like to let you know that we have attributed the jet breakdown to the inherent unsteady nature of the under-expanded flow and not due to numerical dissipation. We were simulating using 2D unsteady code due to resource limitations, Although there were major issues in numerical stability, we were able to achieve robustness using a lower under-relaxation factor.
Also , in some cases where some solution was better than no solution, we found that switching between a first/ second order spatial discretization in those cells that were blowing up helped to reach convergence without much loss in accuracy.
I had developed grids with wall y+ less than one and aspect ratio of 2.5 (after independence check) for this simulation. Also, from the mach contour shown the under-expanded flow results in shock cells just outside the exit adding to the instability. The flow observed is also oscillatory in the vertical direction.
Thank You,
Gautham Narayan
- Badges
- Science topic