[gokenq]

Hi all,

Recently I have been starting a new project testing supersonic cones at high altitudes in like a 2D simulation.

My goal is to try to analyze the front shock of a heat shield which is shown in the Mach graph, ignoring the backflow. But I can't get a clean shock, and I keep getting waves within the shocks. So I took a step back to use an angled hill to test out the flow. But it still won't converge, and appear some reflect waves within the shock in the blue graph.

For some reason, my flow keeps messing up even creating multiple different meshes. The following pictures are my setups and simulation results. I hope you guys can help me out.

Solver: Density-based (I tried Pressure based, but it also didn't work)
Turbulence model: Laminar ( I also tried spalart allamars)
Velocity inlet from left to right as the pressure outlet
the bottom is the axis, and the top is used as the wall but it is pretty far from the shock.

the wall is in the right corner where a hill-shaped bump. (so the bottom be like three lines, axis - wall - wall )

Velocity speed (960 m/s )
initial pressure (52 pa for high altitude )
material: air
density: ideal gas
viscosity: Sutherland law
energy: on (automatic for ideal gas)


All these are after 8000 iterations.

[LoGaL]

I don’t get what is messed up, could you elaborate?

[Indra]

Originally Posted by gokenq

Hi all,

Recently I have been starting a new project testing on supersonic cones at high altitudes in like a 2D simulation.

For some reason, my flow keeps messing up even creating multiple different meshes. The following pictures are my setups and simulation results. I hope you guys can help me out.

Solver: Density-based (I tried Pressure based, but it also didn't work)
Turbulence model: Laminar ( I also tried spalart allamars)
Velocity inlet from left to right as the pressure outlet
the bottom is the axis, and the top is used as the wall but it is pretty far from the shock.

the wall is in the right corner where a hill-shaped bump. (so the bottom be like three lines, axis - wall - wall )

Velocity speed (960 m/s )
initial pressure (52 pa for high altitude )
material: air
density: ideal gas
viscosity: Sutherland law
energy: on (automatic for ideal gas)


All these are after 8000 iterations.

i think that first of all your domain needs to be bigger for the shock and flow to develop properly. but anyways, what exactly is the problem here?

[gokenq]

Originally Posted by Indra

i think that first of all your domain needs to be bigger for the shock and flow to develop properly. but anyways, what exactly is the problem here?

Originally Posted by LoGaL

I don’t get what is messed up, could you elaborate?

I try to analyze the front shock of a heat shield (red graph), and it seems to be messed up somewhere since the shock never comes out clear but lots of small waves within the shocks. I tried to make a bigger flow field or small size of the mesh but it did not seem to be working.

So I took a step back and just do an angled hill and test from there (blue graph) but it also seems to be not working because that happens again even after 30,000 iterations or become invalid due to high residuals.

[LoGaL]

Ah ye, there's that kind of flow separation after the shock.

First, extend the domain as the other person above suggested. This won't probably change anything, BUT you need to do it anyways, otherwise the CFD is garbage


Second, is the solution converged? In my experience, that sort of post-shock flow separation problem is purely numerical, and it is because the steady solver didn't find a steady solution.

Can I see the residuals? I bet even after 30k iterations they didn't go down

[Indra]

Originally Posted by gokenq

I try to analyze the front shock of a heat shield (red graph), and it seems to be messed up somewhere since the shock never comes out clear but lots of small waves within the shocks. I tried to make a bigger flow field or small size of the mesh but it did not seem to be working.

So I took a step back and just do an angled hill and test from there (blue graph) but it also seems to be not working because that happens again even after 30,000 iterations or become invalid due to high residuals.

could you show us your solution methods as well as residuals. Also, try putting a structured mesh as your geometry is not that complex(perform a mesh check once in Fluent before running the sim).

[gokenq]

This is a quick report of the project. Please take a look at my whole process.https://docs.google.com/document/d/1...f=true&sd=true

My goal is to analyze the front shock structure and find its stable flow setting. Currently not dealing with any after shock or backflow in the afterbody (So the project can be easier)

But thank you for your time.

[LoGaL]

Please provide what was asked: residual plots. I don’t have time to go through your folder

If you ask for help, you must be willing to follow instructions xD

[gokenq]

Sorry about that. This is the residuals graph. All other simpler meshes tend to have similar residuals.

thank you!

[LoGaL]

So your simulation is not even converging eh? The residuals are actually exploding…pretty useless to show results if you ask me.. if you let it go longer you will eventually get floating point exception

What settings do you use for the simulation? If you do check mesh in fluent,do you get errors in the console?

[gokenq]

I don't have any error in mesh from the fluent check quality or check meshes.

setting:
Solver: Density-based (I tried Pressure based, but it also didn't work)
Turbulence model: Laminar ( I also tried spalart allamars)
Velocity inlet from left to
right is the pressure outlet
the bottom is the axis, and the top is used as the wall but it is pretty far from the shock( I can have a bigger flow field) .

Velocity speed (960 m/s )
initial pressure (52 pa for high altitude )
material: air
density: ideal gas
viscosity: Sutherland law
energy: on (automatic for an ideal gas)

The simple shape I did is in the right corner where a hill-shaped bump is. (so the bottom be like three lines, axis - wall - wall )( the blue graph)

[Indra]

Originally Posted by gokenq

I don't have any error in mesh from the fluent check quality or check meshes.

setting:
Solver: Density-based (I tried Pressure based, but it also didn't work)
Turbulence model: Laminar ( I also tried spalart allamars)
Velocity inlet from left to
right is the pressure outlet
the bottom is the axis, and the top is used as the wall but it is pretty far from the shock( I can have a bigger flow field) .

Velocity speed (960 m/s )
initial pressure (52 pa for high altitude )
material: air
density: ideal gas
viscosity: Sutherland law
energy: on (automatic for an ideal gas)

The simple shape I did is in the right corner where a hill-shaped bump is. (so the bottom be like three lines, axis - wall - wall )( the blue graph)

What I meant by solver setting in the solution methods that detail all the discretization schemes used, usually we'd advise using a first order scheme to begin with if you have convergence issues. Please share a snapshot of that and also a snap of your mesh. Do perform the mesh check in fluent. Additionally, try using fmg initialisation, it's a better form of initialisation. Also if you mesh is similar to the one in first image, try putting structured grid.

[gokenq]

This is the setting.

I will try using face mashing.

Thank you for helping me out!

[LoGaL]

To be fair, I think the mesh quality is quite good…and also the setup might be correct. it could just be that you are simulating quite difficult flow conditions.. this 60 pa at 1000 m/s is quite extreme


Did you already try to slowly ramp up the velocity? So say you start the simulation at 100 m/s, converge the simulation, increase to 200, run, increase to 400, run ecc ( at one point , you can also script it, rather than doing it manually)

[gokenq]

Because of the shape of the heat shield, it is hard for me to do face meshing because I need to assign different regions and it often comes out of that blue stop sign. So I used vertex sizing for different radii around the wall, I used multiple circle zone with decreasing cell size for the meshes to get a better quality of the mesh-like above 0.9 average element quality. For face mesh, I often get a 0.41 average element quality, even if I try different zones' dirstrubtion. What would be a good range for the face mesh quality?

The reason I doing a high velocity and low pressure is that I want to simulate a reentry situation at a higher altitude.

I did not try to slowly ramp up the velocity, but I can definitely do that! Thank you! I will let you know what is the result.

[AlexanderZ]

1. as was suggested you may gradually increase velocity
2. your may increase your domain so the shock wave don't interfer with outflow BC. ACtually you want domain as large as possible

[Indra]

[QUOTE=gokenq;832893]This is the setting.

I will try using face mashing.

Thank you for helping me out![/QUOTE

Alright so there's a few things you can do here. Chnage fradient scheme to least square or node based.
First start with first order scheme for flow and when residuals go down, change to second order.
Also turn on pseudo time step and use a low time scale factor, i.e reduce from 1 to 0.5 or even lower and let the residuals go down.

Furthermore you can use high order term relaxation but that comes later on. Try firstly with the above changes.

[wrosendoeng]

First of all, the turbulence model used in this case is wrong. Laminar modelling doesn`t serve due to high Reynolds number presented in this situation.

Three suggestions:
1. Use RANS modelling: Spalart-Allmaras or SST k-omega (2nd option is better, but SA model is cheapier for computational cost and is also good)
2. Check the mesh next from the wall for each RANS modelling (y plus has to be between 0 and 10 for linear region of boundary layer, greater than that the buffer region of boundary layer may be calculated and it's not good due to high possibility of numerical errors.)
3. Include "pressure-far-field" BC on the top region. It's a good option for inviscid supersonic flows that uses ideal gas law, like your case.

[LoGaL]

Lol, at that pressure it is definitely laminar.. it is almost rarified

[wrosendoeng]

Originally Posted by LoGaL

Lol, at that pressure it is definitely laminar.. it is almost rarified

Yeah, I have to apologize me. I didn't see the pressure in BC. I considered it as a sea-level pressure and, yes, it's quite low and then, laminar condition may be applied.