[KruX]

Hi,

For my thesis I have to simulate the flow in an aerospike nozzle. Unfortunately I still have some problems to get a sufficient solution.
I am of the opinion that my mesh is ok, because the most important key figures are kept (Max. Skewness < 0.98, Min. Orth. Quality > 0.1, Average Element Quality > 0,775, AR <5 besides some cells at the wall where the AR is up to 30). The outlet is also far enough away from the actual nozzle geometry (about 10 times the length of the nozzle). I currently aim for 30 < y+ < 300 as I use wallfunctions to simulate the viscous sublayer.

I am using the following settings (on Ansys 19.2):

-density based solver
-axissymmetric
-energy equation
-realizable k-epsilon
-pressure inlet at 68,9476 bar and 2616.532 K (default turbulent intensity and viscosity ratio)
-pressure-farfield for all non wall boundaries and as the outlet
-All second order upwind methods

My Simulation converged when I applied a free stream Mach number of M=0.6 (at the left boundary and at the outlet), but at M=0.4 the simulation isn't converging anymore. I tried to initialize it with a inviscid flow, but it isn't converging as well.

Some ideas/questions I had:
- Can I apply a pressure farfield at the left boundary (Face E in the overview)? It is not really a free stream condition as the nozzle wall is at the buttom.
- I have a quiet high element area growth rate after the throat, max this cause the problems? I need a very high resolution at the curvature before and after the throat because otherwise the AR is too high.

I attached some pictures showing the hole domain as well as some close ups. But I will gladly supply everything else that is needed to assess my problem. I'd appreciate any help!

Thank you and best regards,
Roman

[AlexanderZ]

- I have a quiet high element area growth rate after the throat, max this cause the problems?

yes, it could be a problem

- Can I apply a pressure farfield at the left boundary (Face E in the overview)?

I think, you can apply, cause flow near that wall is not important for you.
Also you may change the angle of E and F boundaries. Now they are at 90 and 0 degrees respectively. I recommend you to use something like 80 and 15 degrees, it may increase convergence speed

My Simulation converged when I applied a free stream Mach number of M=0.6 (at the left boundary and at the outlet), but at M=0.4 the simulation isn't converging anymore.

get solution for 0.6 Mach, decrease external speed to 0.5, and CONTINUE simulation, DONT initialize. repeat again after convergence

[KruX]

Originally Posted by AlexanderZ

get solution for 0.6 Mach, decrease external speed to 0.5, and CONTINUE simulation, DONT initialize. repeat again after convergence

Thank your for your response. I am currently running the simulation to try this. I have a few additional questions:

- At the beginning of the simulation both the inlet and outlet massflows are negative. With the inlet massflow this seems a bit strange to me. At the end however the inlet massflow is positive. Shouldn't this mass flow be positive from the very beginning? (I attached a picture of the inlet and outlet massflow from the currently running simulation)
- Do I need to specify the flow direction at the Pressure-Farfield according to the sign of the massflow? Like an axial component of 1 for Face E and an axial component of -1 for the outlet at Face D? What would be with the upper bundary Face F?

Many thanks for the help!

[AlexanderZ]

have no idea, why you do have negative mass flow. Could be because of inverse normal in fluent, whatever.

If I were you, I'd put D boundary conditions as far-flied also.

Put flow direction for all far-fields boundaries the same (default is along with nozzle axis, actually this is the only option, cause you are using 2D)

[Guvennergiz]

Hi Roman,
Fluent is a really sensetive software, so can you improve your mesh due to attached figure (min ortho. - max. skewness) ?

P.s: I am not sure but; while M=0.4 maybe flow can not be axisymmetric and also turbulent? Because turbulence is a chaotic situation.

I hope it helps to you.
Best regards,
Güven

[KruX]

Originally Posted by AlexanderZ

get solution for 0.6 Mach, decrease external speed to 0.5, and CONTINUE simulation, DONT initialize. repeat again after convergence

Unfortunately that did not work either. I think my problem is of a more fundamental nature.

Originally Posted by Guvennergiz

Hi Roman,
Fluent is a really sensetive software, so can you improve your mesh due to attached figure (min ortho. - max. skewness) ?
Güven

Thank you for your response. So over so weekend I tried to take a step back and reduce the complexity of my problem. I am now simulating only the divergent part of the aerospike nozzle. By doing so I am now able to achieve a better mesh. My max. Skewness is now 0.52 (Average is 4.9e-3) and the min. Ortho. is 0.698 (Average is 0.999). The simulations are running now, but at the end I get the message 'Divergence detected - temporarily reducing Courant number to 0.5 and trying again...' and then the residuals explode. This happens exactly when the mass flows converge, i.e. the incoming mass flow corresponds to the outgoing mass flow. Does anybody have an idea what this is due to?

Thank you and best regards,
Roman

[AlexanderZ]

use your first mesh, cause you can define boundary conditions there (for chamber)

predefine pressure and small velocity fields in chamber using PATCH tool

use FMG initialization (with and without patching)

find case when you can reach convergence and move from it slightly changing flow parameters

if all of that doesn't work switch to transient simulation

[KruX]

Okay, but with the first geometry my max. skewness is around 0.8 and I can't really improve it. I read that for a 2D Mesh a max. skewness of 0.5 is desirable. Should I try an unstructured Mesh in this area?

Since I know the throat conditions I thought that I can define those BC as well.

Best regards,
Roman

[KruX]

Okay, so I tried FMG-Initialization at the first grid. This was prompted in the console:

Creating multigrid levels...
Grid Level 0: 510250 cells, 1022230 faces, 511981 nodes; 6 clusters
Grid Level 1: 128113 cells, 513405 faces, 511981 nodes; 6 clusters
Grid Level 1: 128113 cells, 283978 faces, 0 nodes
Grid Level 2: 35421 cells, 278704 faces, 511981 nodes; 6 clusters
Grid Level 2: 35421 cells, 88002 faces, 0 nodes
Grid Level 3: 10802 cells, 165036 faces, 511981 nodes; 6 clusters
Grid Level 3: 10802 cells, 30057 faces, 0 nodes
Grid Level 4: 3467 cells, 103617 faces, 511981 nodes; 6 clusters
Grid Level 4: 3467 cells, 10796 faces, 0 nodes
Grid Level 5: 1177 cells, 68299 faces, 511981 nodes; 6 clusters
Grid Level 5: 1177 cells, 4381 faces, 0 nodes
Done.


FMG: Converge FAS on level 5 [eps = 0.001000, max-iter=500]
.......... -> Normalized residual = 0.620857
.......... -> Normalized residual = 0.685669
.......... -> Normalized residual = 0.717004
.......... -> Normalized residual = 0.772636
.......... -> Normalized residual = 0.887685
.......... -> Normalized residual = 0.980624
.......... -> Normalized residual = 1.03261
.......... -> Normalized residual = 0.937003
.......... -> Normalized residual = 0.715479
.......... -> Normalized residual = 0.558359
.......... -> Normalized residual = 0.442348
.......... -> Normalized residual = 0.349808
.......... -> Normalized residual = 0.280429
.......... -> Normalized residual = 0.22814
.......... -> Normalized residual = 0.186506
.......... -> Normalized residual = 0.164774
.......... -> Normalized residual = 0.128299
.......... -> Normalized residual = 0.0666921
.......... -> Normalized residual = 0.0446356
.......... -> Normalized residual = 0.0716607
.......... -> Normalized residual = 0.0761571
.......... -> Normalized residual = 0.0288275
.......... -> Normalized residual = 0.0161657
.......... -> Normalized residual = 0.0228791
.......... -> Normalized residual = 0.0129814
.......... -> Normalized residual = 0.0132236
.......... -> Normalized residual = 0.0259083
.......... -> Normalized residual = 0.0108733
.......... -> Normalized residual = 0.0140829
.......... -> Normalized residual = 0.0165374
.......... -> Normalized residual = 0.0186223
.......... -> Normalized residual = 0.0254944
.......... -> Normalized residual = 0.0343955
.......... -> Normalized residual = 0.0555848
.......... -> Normalized residual = 0.0834148
.......... -> Normalized residual = 0.0612789
.......... -> Normalized residual = 0.0554939
.......... -> Normalized residual = 0.0542144
.......... -> Normalized residual = 0.0551109
.......... -> Normalized residual = 0.0536847
.......... -> Normalized residual = 0.0475517
.......... -> Normalized residual = 0.0477755
.......... -> Normalized residual = 0.0439204
.......... -> Normalized residual = 0.0407838
.......... -> Normalized residual = 0.0467082
.......... -> Normalized residual = 0.0402134
.......... -> Normalized residual = 0.0438325
.......... -> Normalized residual = 0.0471261
.......... -> Normalized residual = 0.0420513
.......... -> Normalized residual = 0.0417182

FMG: FAS reached maximum iterations.
Normalized residual = 0.0417182

FMG: Finished work on level = 5

FMG: Interpolate solution on next level .. . end


FMG: Converge FAS on level 4 [eps = 0.001000, max-iter=500]
.
FMG: FAS converged.

FMG: Finished work on level = 4

FMG: Interpolate solution on next level .. . end


FMG: Converge FAS on level 3 [eps = 0.001000, max-iter=100]
.
FMG: FAS converged.

FMG: Finished work on level = 3

FMG: Interpolate solution on next level .. . end


FMG: Converge FAS on level 2 [eps = 0.001000, max-iter=50]
.......... -> Normalized residual = 0.0013315
.......... -> Normalized residual = 0.00132221
.......... -> Normalized residual = 0.00131677
.......... -> Normalized residual = 0.00131406
.......... -> Normalized residual = 0.00131139

FMG: FAS reached maximum iterations.
Normalized residual = 0.00131139

FMG: Finished work on level = 2

FMG: Interpolate solution on next level .. . end


FMG: Converge FAS on level 1 [eps = 0.001000, max-iter=10]
.......... -> Normalized residual = 0.0049139

FMG: FAS reached maximum iterations.
Normalized residual = 0.0049139

FMG: Finished work on level = 1

FMG: Interpolate solution on next level .. . end
0.
time step reduced in 135 cells due to excessive temperature change

absolute pressure limited to 1.000000e+00 in 2 cells on zone 3

absolute pressure limited to 5.000000e+10 in 21041 cells on zone 3

temperature limited to 5.000000e+03 in 86312 cells on zone 3
->1.->2.->3.->4.->5.<<<<<

turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 4604 cells

turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 4545 cells

Does it mean that the mesh quality in those cells is too bad or is there a more generell problem?

[karachun]

Try to make additional slices that are perpendicular to walls. This will enforce the mesher to make elements with less skewness.

[KruX]

Originally Posted by karachun

Try to make additional slices that are perpendicular to walls. This will enforce the mesher to make elements with less skewness.

Thank you! I was now able to achieve a max. skewness of about 0.5 and a min. ortho. of 0.6 in my first mesh. But the FMG-Initialization isn't working as well. At the end comes the message:

time step reduced in 93 cells due to excessive temperature change

absolute pressure limited to 5.000000e+10 in 6575 cells on zone 3

temperature limited to 5.000000e+03 in 17105 cells on zone 3
->1.->2.->3.->4.->5.<<<<<

turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 419 cells

turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 408 cells

Do I need to refine the mesh or do I need to work on my BC setup? Thank you all for your help.

[AlexanderZ]

most likely the problem is in your boundary conditions, materials properties or other setup conditions.

there are several good simulation examples on gasflow from nozzle.
Copy their boundary conditions first.

Keep trying

[KruX]

Okay, I will try that. You guys already helped me a lot, but if one has the time and patience to look at my setup it would be verry appreciated. I attached some picture of the BC setup.

[AlexanderZ]

BC looks ok,
but why UPPER pressure-far-field has Mach 0.1 ? same conditions should be applied for all pressure-far-field BC

also you may start with first order equations and switch to second order later.

you may decrease under-relaxation factors

[KruX]

Originally Posted by AlexanderZ

BC looks ok,
but why UPPER pressure-far-field has Mach 0.1 ? same conditions should be applied for all pressure-far-field BC

also you may start with first order equations and switch to second order later.

you may decrease under-relaxation factors

Since I wanted to simulate the engine in flight, I thought that I could not assume the same speed in radial direction as in axial direction. I tried it now with the same Mach number (and first order equations), but then I got the message 'Divergence detected - temporarily reducing Courant number'. Maybe my mesh is just not fine enough? This is honestly the only idea I have left.

[KruX]

Hello,

I had to work on a few different things about my thesis but I am now back to the simulations.
They are still diverging when I apply pressure farfields as all of the domain boundaries. Therefore I have a quastion regarding the specification of the pressure farfields. Do I have to specify the flow direction, for expample an axial component of -1 for a pressure farfield which serves as an outlet? Do I need to specify a radial component for a horizontal pressure farfield? (Does the radial/axial refer to the overall coordinate system or to the respective plane?)

Thank you and kind regards,
Roman

[AlexanderZ]

by default PFF uses global coordinate system
you don't need to do this:

for example an axial component of -1 for a pressure farfield

just put same condition for all you PFF boundaries

what you can do:
1. Try a Spalart All-maras turbulence model first
2. Try a range of courant numbers starting from the default number of 5 and lowering it up to 1 and less and observe which courant number provides the best convergence.
3. You may switch to transient simulation, cause usually the solution is not steady state
4. Write data during simulation, check whats going on just before divergence
5. Of course, mesh could be a problem, so you may try to read on the y plus value and make sure for this specific problem to have the y plus be less than 1 to get accurate results regarding the shock placement along the nozzle wall (if you make step 4, check where the problem comes from, where the mesh should be refined)
6. You may try 3D case, cause turbulence is 3D phenomena (in that case I recommend to use full 3D if you have enough computational power)
7. And again, patching flow parameters in chamber increase convergence

[KruX]

I am now running the simulation with SA. I also applied the left, upper and right boundary to the same Pressure-Farfield (before that they were all in seperate PF).
So I tried to observe what happens right before the simulation diverges. There is a sudden spike in temperature in a few cells which you can see in the pictures I attached. The amount of cells with limited temperature is growing ('temperature is limited to 5000' and 'time step reduced due to excessive temperature change' is displayed in the console) and than the residuals explode and the simulation diverges.

I don't really understand it, beause it occurs in a region where no high temperature gradients are located and the Mesh is quiet refined in this region (at least for a free stream region)

[AlexanderZ]

no idea, what is the reason of this behavior, but what you can do is to patch that region with flow parameters, which you expect to have