CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

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

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 2, 2020, 08:41
Default How to setup Boundary Layer for Compressible hypersonic flow in Ansys Fluent?
  #1
New Member
 
Join Date: May 2020
Posts: 23
Rep Power: 3
CFDger is on a distinguished road
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 2D-wedge 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 k-omega
Fluid: Air: Density ideal-gas 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, Roe-FDS, 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.
CFDger is offline   Reply With Quote

Old   June 2, 2020, 08:48
Default Boundary Condition
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
It would be preferable to set all outer boundary conditions as far-field, provided there is no wall touching the far-field boundary. Furthermore, use fmg-initialization. Ensure that the fmg-initialization 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.
vinerm is offline   Reply With Quote

Old   June 2, 2020, 09:38
Default
  #3
New Member
 
Join Date: May 2020
Posts: 23
Rep Power: 3
CFDger is on a distinguished road
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 fmg-initialization 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 Kn-number is approximately 1.8e-7, 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
Attached Images
File Type: png Mesh_1.PNG (50.9 KB, 4 views)
File Type: jpg Mesh_2.jpg (126.4 KB, 4 views)
CFDger is offline   Reply With Quote

Old   June 2, 2020, 09:39
Default FMG Initialization
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
If fmg-initialization 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.
vinerm is offline   Reply With Quote

Old   June 2, 2020, 09:48
Default
  #5
New Member
 
Join Date: May 2020
Posts: 23
Rep Power: 3
CFDger is on a distinguished road
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.
CFDger is offline   Reply With Quote

Old   June 2, 2020, 12:22
Default
  #6
New Member
 
Join Date: May 2020
Posts: 23
Rep Power: 3
CFDger is on a distinguished road
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 fmg-initialization).


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
CFDger is offline   Reply With Quote

Old   June 9, 2020, 09:31
Default
  #7
New Member
 
Join Date: May 2020
Posts: 23
Rep Power: 3
CFDger is on a distinguished road
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 e-3 but the solution looks reasonable.
CFDger is offline   Reply With Quote

Old   January 5, 2021, 15:09
Default
  #8
New Member
 
roniroket
Join Date: Jan 2021
Posts: 4
Rep Power: 2
roniroket is on a distinguished road
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?



Quote:
Originally Posted by CFDger View Post
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 e-3 but the solution looks reasonable.
roniroket is offline   Reply With Quote

Old   January 7, 2021, 12:32
Default
  #9
New Member
 
Join Date: May 2020
Posts: 23
Rep Power: 3
CFDger is on a distinguished road
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
CFDger is offline   Reply With Quote

Old   January 10, 2021, 09:12
Default Divergence Issue
  #10
New Member
 
roniroket
Join Date: Jan 2021
Posts: 4
Rep Power: 2
roniroket is on a distinguished road
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 Spalart-Allmaras.

However, when I start running k-w SST with low-Re corrections and compressibility effects, it works fine, then after 1e-3 x-velocity residuals, it starts fluctuating between 1e-2 and 1e-3. Other residuals such as k, w, y velocity and energy can reach below 1e-4 residuals.

At the end, they start fluctuating but do not diverge like crashing. Actually, even 1e-3 residual results are not bad, contour is good, but I cannot reach to stable residuals as I have reached using Spalart-Allmaras.

What do I miss here?

Quote:
Originally Posted by CFDger View Post
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
roniroket is offline   Reply With Quote

Old   January 10, 2021, 16:27
Default
  #11
New Member
 
Join Date: May 2020
Posts: 23
Rep Power: 3
CFDger is on a distinguished road
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 k-w-SST 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 k-w-SST model and not the Spalart Allmaras. Maybe you can find something to that specific topic?

And if the result of your simulation with the k-w-SST 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 1e-06). 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
CFDger is offline   Reply With Quote

Reply

Tags
ansys, boundary condition, compressible, fluent, pressure boundaries

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
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
sliding mesh problem in CFX Saima CFX 45 September 22, 2015 10:53
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


All times are GMT -4. The time now is 17:15.