
[Sponsors] 
How to setup Boundary Layer for Compressible hypersonic flow in Ansys Fluent? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 2, 2020, 08:41 
How to setup Boundary Layer for Compressible hypersonic flow in Ansys Fluent?

#1 
Member
Join Date: May 2020
Posts: 32
Rep Power: 4 
Hello,
I already read many threads in this forum regarding this topic but unfortunately none of them were helpful. I am trying to simulate the airflow around a 2Dwedge which is moving at hypersonic speed (Mach=8 at 30000 m). I understand and have read that for my application pressure inlet, pressure outlet and pressure farfield boundary conditions are applicable. My problem is that my solution won't converge at all. I have tried changing the boundary conditions and the solution methods, switching on and off the turbulence modeling and so on. Here are my settings: Density based Energy on Viscous komega Fluid: Air: Density idealgas and viscosity according to sutherland law Boundary Conditions: Inlet: Pressure inlet: I calculated a total pressure of p(total) = 2.93e8 Pa (isentropic relation with Ratio of Specific Heats = 1.4, Ma=8 and p(static, 30000 m, ISA)=301hPa. I set the "Gauge Total Pressure" to my calculated total pressure value. The "Supersonic/Initial Gauge Presse" I set to my p(static). The temperature is 228.75 K (ISA, 30000 m) Outlet: Pressure outlet: Here I set the "Gauge Pressure" to the aforementioned p(static) = 301hPa and the Temperature to 228.75 K. The outer "walls" defined as pressure far field BoC: Ma = 8 and Gauge pressure to p(static) = 301hPa. I also set the "Operating Pressure" to 0. Solution Methods: Implicit, RoeFDS, Gradient: Least Squares, Flow, Turbulent Kinetic Energy and Specifiy Dissipation Rate: Second Order Upwind Now first of all as I mentioned the solution doesn't converge at all. Then when I check the Reference Values, I see that the calculated velocity in the inlet doesn't represent the numbers I would have expected. I would be very thankful if you could help me find the solution for my problem. I am new to CFD/Ansys which is why I want to gain as much knowledge as possible. Thank you very much. 

June 2, 2020, 08:48 
Boundary Condition

#2 
Senior Member

It would be preferable to set all outer boundary conditions as farfield, provided there is no wall touching the farfield boundary. Furthermore, use fmginitialization. Ensure that the fmginitialization is successful. If it is not, then there is some issue with the setup.
What's the Knudsen number for the system since it is operating at 30 km?
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. 

June 2, 2020, 09:38 

#3 
Member
Join Date: May 2020
Posts: 32
Rep Power: 4 
Hello Vinerm,
thank you for your suggestions. I tried setting all BoC as far field already but still the solution didn't converge. I set the Mach Number to 8, the Gauge Pressure to the absolute pressure for a height of 30000 m (>p=30100 Pa) and the Temperature to the according temperature of 228.75 K. Please correct me if I already made a mistake here already. I tried just tried out the fmginitialization but as an "answer" I receive the following: "Error: floating point exception Error Object: #f" I read that there are multiple possible reasons for this error. So the error seems to be somewhere with my setup. Attached I send you pictures of my mesh. I haven't done a "mesh independence study", I just focused on having a fine enough mesh at the boundary layer and not too small angles. My Knnumber is approximately 1.8e7, so we are looking at continuum flow in this case. Next I would try to revise my mesh and look for potential errors. If you have any more suggestions I would be very thankful. Best regards 

June 2, 2020, 09:39 
FMG Initialization

#4 
Senior Member

If fmginitialization is failing, then there is problem with the setup. It could be any where starting from bad mesh to operating conditions. Do note this has got nothing to do with numerical setup, only physical setup.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. 

June 2, 2020, 09:48 

#5 
Member
Join Date: May 2020
Posts: 32
Rep Power: 4 
Alright, thank you. It's good to know that I have to look at the physical setup instead of the numerical one in this case.


June 2, 2020, 12:22 

#6 
Member
Join Date: May 2020
Posts: 32
Rep Power: 4 
I now changed my mesh and deleted any node bias which I had originally implemented for a refined boundary layer resolution.
With these changes the problem converges (using farfield boundary conditions and fmginitialization). As soon as I implement even a slight bias the solution doesn't converge anymore. I couldn't find anything regarding this problem... Do you maybe have an idea on how I can continue on this? best regards 

June 9, 2020, 09:31 

#7 
Member
Join Date: May 2020
Posts: 32
Rep Power: 4 
In case anybody is interested: The mesh had to be refined, especially the transitions between the finer and coarser parts.
Unfortunately the residuals mostly only converge to the order e3 but the solution looks reasonable. 

January 5, 2021, 15:09 

#8 
New Member
roniroket
Join Date: Jan 2021
Posts: 4
Rep Power: 4 
Can you give more information about this setup?
I try to solve a hypersonic flow problem, 2D 10 degrees of shock generator and shock boundary layer interaction. I tried to do very good mesh, but my solution diverges. If you were able to obtain a good result, can you list your settings as a guideline for others? 

January 7, 2021, 12:32 

#9 
Member
Join Date: May 2020
Posts: 32
Rep Power: 4 
Hi,
ok what I have learned is that there are multiple possible reasons for a diverging solution. 1) Mesh. You said that you think that yours is good. Could you maybe send a picture of your mesh? This way it is easier to see errors and to understand your specific problem 2) Which numerical solver settings did you use? Which turbulence model? Which air model? For hypersonic flows you can't model air as calorically ideal gas etc... 3) Which Boundary Conditions have you used? oh and just fyi: When people refer to a "real gas model" in the context of hypersonic external flow they often actually mean a model which takes into account "high temperature effects" which occur at hypersonic flows 

January 10, 2021, 09:12 
Divergence Issue

#10  
New Member
roniroket
Join Date: Jan 2021
Posts: 4
Rep Power: 4 
Sorry for the late reply.
Let me summarize issues. I obtained results with a very good mesh for such a setup like 200.000 faces. Orthogonality and mesh quality values are good. In fact , I am able to obtain %99 similar results with experimental setup and other CFD papers using SpalartAllmaras. However, when I start running kw SST with lowRe corrections and compressibility effects, it works fine, then after 1e3 xvelocity residuals, it starts fluctuating between 1e2 and 1e3. Other residuals such as k, w, y velocity and energy can reach below 1e4 residuals. At the end, they start fluctuating but do not diverge like crashing. Actually, even 1e3 residual results are not bad, contour is good, but I cannot reach to stable residuals as I have reached using SpalartAllmaras. What do I miss here? Quote:


January 10, 2021, 16:27 

#11 
Member
Join Date: May 2020
Posts: 32
Rep Power: 4 
I haven't used Spalart Allmaras so I unfortunately can't comment on that or compare my solution to one using Spalart Allmaras turbulence model.
I only used kwSST model. I got fluctuating residuals when I meshed the wake flow of my hypersonic object aswel. As soon as I cut the fluid domain at the tail of my flying object, the fluctuations disappered. The reason for that is that the wake region often behaves unsteady/transient. A steady numerical approach will lead to oscillating residuals if unsteady regions in your domain exist. But this unfortunately doesn't answer the question why this phenomenom only occurs with the kwSST model and not the Spalart Allmaras. Maybe you can find something to that specific topic? And if the result of your simulation with the kwSST turbulence model makes sense and is comparable to the experimental values, the residuals are not that important (they still are of course, but not in every case you actually need or can reach desired residuals of 1e06). You should also look at other parameters and look if they converge. Like for example the mass flow balance at the inlet and outlet or the value of the coefficient of friction, ... etc. Why are you using compressibility effects? Did they have a positive effect with Spalart Allmaras model? I would be careful with this setting as the ansys fluent user guide/theory guide discourages the user from using this if the coefficient of friction is of importance for the cfd user... Always try to go one step a time and evaluate the steps in order to be able to explain them and why you applied them. And what air model are you using? Calorically perfect gas, thermally perfect gas, or are you even considering reactions? Best regards 

December 30, 2021, 05:15 
Boundary condition

#12 
New Member
Borde Ganesh
Join Date: Oct 2021
Posts: 1
Rep Power: 0 
Has u given boundary condition,u give the density as ideal gas,you mentioned that 30000 is altitude at that altitude the density is differnt,so how u considered as ideal gas
can u please explain 

Tags 
ansys, boundary condition, compressible, fluent, pressure boundaries 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
sliding mesh problem in CFX  Saima  CFX  46  September 11, 2021 07:38 
Wind turbine simulation  Saturn  CFX  58  July 3, 2020 01:13 
3D Windturbine simulation in SU2  k.vimalakanthan  SU2  14  February 8, 2019 14:43 
CFX overwhelming Fluent in mass convergence of boundary layer separation case  Pierre1  FLUENT  7  March 26, 2015 21:43 
New topic on same subject  Flow around race car  Tudor Miron  CFX  15  April 2, 2004 06:18 