[aeroboi]

Hi,
I am running a 3D steady hypersonic simulation with sharp (90 deg) external expansion corners and am curious if anyone has experienced a similar phenomena I'm getting. I'm using Fluent's (finite volume) density-based, implicit solver with energy on and SST k-omega viscous model. My Reynolds # is ~9.2e6. Density follows ideal gas, viscosity set to Sutherland's law, and thermal conductivity follows a Pr = 0.71.


In order to converge, I needed to reduce the solution limit for pressure minimum to be 1e-3 Pa, and from this there are timesteps is sadly on the order of 1e-12 (to maintain a CFL = 1.0). This is occurring right after the sharp expansion corner, at the wall.



I would like to use this steady solution as an IC for an unsteady simulation, but need to run with a very small timestep (even using a high CFL), which just isn't feasible.


Is this something that's actually expected in this situation? Can pressure/timestep truly be on this very low order of magnitude? It just seems a bit unphysical for this to be occurring. While trying to dive deeper into this, I also have completed numerous additional simulations on highly refined 3D structured grids modeling just a cuboid-shaped trailing edge.



I am able to easily reproduce it this pressure/timestep issue with this. I also am extremely confident it's not a mesh refinement issue (although maybe having very tiny cells at the corner are contributing?)



Any input is extremely appreciated!!

[LuckyTran]

The more the mesh refinement, the smaller the cells, the smaller the time-step you need to keep the Courant number low. Make your smallest cells bigger!


Even when there are warnings that the minimum pressure exceeds the minimum pressure limit, you shouldn't ever really lower the minimum. It is at best a bandaid and at worse exacerbates the problem. You get unphysical pressures because your solution is not good. The limiters prevent it from being non-physical. Now you lower the lower limit to unrealistic values so you get unrealistic time-steps, neither of which are the root cause of your problems.

[aeroboi]

Thanks for the reply, so are you saying essentially that my mesh may be too refined? Shouldn't greater refinement always entail a better solution given the cell quality remains good (which it does)?


I can understand that maybe too tiny cells lead to too tiny timesteps but not the nonphysical pressure part if that makes sense.

[agd]

The physical behavior is not uncommon for supersonic/hypersonic CFD simulations. In real life flow traversing a sharp corner will expand very quickly leading to low pressures in those expansion regions. Numerically this will become problematic if you are running a sufficiently high Mach number and trying to start from a uniform freestream initial condition, or if there are some relevant physics that you are leaving out (are you treating a thermally perfect physical problem as an ideal gas, or trying to ignore equilibrium chemistry, or something else?) In the first case you might be able to ramp up the oncoming Mach number over a series of timesteps to whatever the final value is. In the second case you need to determine what the relevant physics are and respect those.


Or it could be that you have a bad grid in the expansion region and fixing your grid will clean up your problems. Note - I have no experience with Fluent, but many years of running high speed flow simulations over a variety of air vehicles using density based solvers. And the behavior you are describing is not specific to Fluent. It is the flow solver doing its best to model the correct physics within the constraints of the grid and specified physical models.

[aeroboi]

Thanks for the reply - it is possible that there are relevant physics I'm leaving out: yes I'm currently modeling the gas to be calorically perfect and neglecting any effects of nonequilibrium since it is not something that I had been expecting.


Given your experience: would you also generally agree with LuckyTran that needing to adjust solution limits (to allow for pressure < 1Pa) typically means that something is wrong with how I'm modeling it computationally? I am confident that my grid refinement and quality are good - the structured 3D mesh (great ARs, volume ratios, etc.) had no cells with a y+ > 1, and plenty of layers within the BL.

[naffrancois]

What you are facing is vacuum formation which is often reached in expansion regions of supersonic flows. Density goes to zero and sound speed gets very high yielding high wave speed => very low time steps to maintain numerical stability. If you refine the grid it gets even worse. I don't know how fluent tackles this, vacuum is not well modeled with NS anyway as it reaches limits of continuum mechanics. Diffusion helps, whether numerical or physical.

[agd]

Well, as Aristotle once said - nature abhors a vacuum. In a real flow the pressure will drop quite low at expansion corners but you won't reach a vacuum state. The problem is that if your numerics are tripping up there then the problem is either in your numerics or in how you are implementing them. If your grid is good then my next question would be how are you starting the flowfield - what is your initial condition? If you are initializing the flowfield to M = 4 with the body of interest sitting still, then you are asking an awful lot of the numerics. In real life we don't get flight vehicles to go from M = 0 to M = 4 instantaneously. But if that is the only way you have to start your flowfield, then lots and lots of diffusion (as mentioned above) might help. Alternatively, you may need to get an initial solution on a coarse grid and then use that to initialize the finer grid solution once you get in the neighborhood of the Mach number you seek. Or you might see if there is a way to get your flowfield up to the desired speed by simulating how it is done in real life - ramp up the Mach number from 0 to the final value over a finite time with a transient solution.


But if you are leaving out some relevant physics then nothing may work. Nature is really good at solving the problems we can't because nature never makes assumptions, and nature always includes the physics.

[FMDenaro]

Originally Posted by aeroboi

Hi,
I am running a 3D steady hypersonic simulation with sharp (90 deg) external expansion corners and am curious if anyone has experienced a similar phenomena I'm getting. I'm using Fluent's (finite volume) density-based, implicit solver with energy on and SST k-omega viscous model. My Reynolds # is ~9.2e6. Density follows ideal gas, viscosity set to Sutherland's law, and thermal conductivity follows a Pr = 0.71.


In order to converge, I needed to reduce the solution limit for pressure minimum to be 1e-3 Pa, and from this there are timesteps is sadly on the order of 1e-12 (to maintain a CFL = 1.0). This is occurring right after the sharp expansion corner, at the wall.



I would like to use this steady solution as an IC for an unsteady simulation, but need to run with a very small timestep (even using a high CFL), which just isn't feasible.


Is this something that's actually expected in this situation? Can pressure/timestep truly be on this very low order of magnitude? It just seems a bit unphysical for this to be occurring. While trying to dive deeper into this, I also have completed numerous additional simulations on highly refined 3D structured grids modeling just a cuboid-shaped trailing edge.



I am able to easily reproduce it this pressure/timestep issue with this. I also am extremely confident it's not a mesh refinement issue (although maybe having very tiny cells at the corner are contributing?)



Any input is extremely appreciated!!

I don't understand you ... Your solver is implicit in time, thus you are already solving an unsteady problem. Then your goal is to get a steady solution as initial condition for a time-dependent problem??


And more, what is the physical meaning of performing an unsteady case using the URANS is not clear, I would have accepted if you was trying to get an initial condition for LES. And also in this case, there is no physical meaning for your IC.