CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Hypersonic Flow simulation using Fluent (http://www.cfd-online.com/Forums/fluent/111876-hypersonic-flow-simulation-using-fluent.html)

beanlee999 January 17, 2013 02:19

Hypersonic Flow simulation using Fluent
 
Dear all,

I am trying to do a hypersonic flow simulation over a sphere of 0.3m radius. Does Fluent has any tutorials or guides regarding setup conditions for hypersonic simulations?

My simulation Mach number is 22. I am using volumetric (species and transport). The mixture comprises of NO,N,O,O2,N2. I set piecewise polynomial for the Cp of each constituent. My operating pressure is 0. My underrelaxation factor is 0.3 and courant number is 0.3. My temperature limit is set to 24000K. The solver is set to second order upwind.

However, my residual level for either NO,O or N is always rather high. It can be as high as 10e12. Does anyone has any idea what is wrong? Pls kindly help to point out my mistakes... I tried to increase the positivity rate limit to between 25 and 30. The residual level drops a lot to around 10e2, but solution does not converge. Should I have taken this approach as well?

Thank you.

Panboy January 20, 2013 02:00

Hi beanlee,

I am currently tackling this same problem.
Maybe we can work on it together and discuss each others problems.
I have not found any tutorials that show hypersonic simulations in fluent.

What turbulence model are you using?
which real gas model are you using
which radiation model are you using?
Can you give me a little more detail on your species transport setup?

In the mean time, here are some links from this forum that I found somewhat interesting, and useful.

http://www.cfd-online.com/Forums/flu...onic-flow.html

http://www.cfd-online.com/Forums/flu...ock-waves.html



Panboy

beanlee999 January 20, 2013 04:27

hi Panboy,

My simulation for now, is a laminar hypersonic flow around a sphere. I have yet to reach the stage of incorporating turbulence models into my simulations. Are you doing one that has turbulence model?

I am using density-based, axis-symmetric implicit steady solver. what do you mean by real gas model in this case?

I have yet to use any radiation model. What i did is to fix my sphere's wall temperature at either 1000K or 300K, depending on the gas components and the free stream Mach number i am using.

For my species transport setup, i am using volumetric with no stiff chemistry solver turned on. The below are the 6 chemical reactions i am using.

Dunn-Kang Model
02+M-2O+M
Af: 3.60E+15
Bf:-1
Eaf: 4.94E+08
Third body efficienies: N2:2 O2:9 NO:1 N:1 O:25

N2+M-2N+M
Af:1.92E+14
Bf:-0.5
Eaf:9.40E+08
Third body efficiecies: N2 2.5 O2:1 NO:1 N:0 O:1

N2+N-3N
Af:4.15E+19
Bf:-1.5
Eaf:9.40E+08
Third body efficiencies: None

NO+M-N+O+M
Af:3.97E+17
Bf:-1.5
Eaf:6.29E+08
Third body efficiencies: N2:1 O2:1 NO:20 N:20 O:20

NO+O-O2+N
Af:3.18E+06
Bf:1
Eaf:1.64E+08
Third body Efficiencies: None

N2+O-NO+N
Af:6.75E+10
Bf:0
Eaf:3.12E+08
Third Body efficiencies: None

Can you share more about your simulation experience and problems as well?

Thanks!

Panboy January 22, 2013 00:53

Hey beanlee,

Sorry im out of town but ill get back to you with my simulation setup in a day or 2.

Talk to you soon!

Panboy

dreamchaser June 18, 2014 19:30

How to Input Third Body "M" into reactions
 
Hello Panboy and Beanlee,

I am doing the similar problem of doing hypersonic flow over a sphere of .2m. I am trying to input my chemical reactions. However, how do I put in the third body "M" into the reaction set?? For example, taking Beanlee's example below how would I input the third body "M" into Fluent? Would I just specify one reactant(O2) and one product(2O) and include the third body efficiencies??

I appreciate your help,

Dreamchaser

Dunn-Kang Model
02+M-2O+M
Af: 3.60E+15
Bf:-1
Eaf: 4.94E+08
Third body efficienies: N2:2 O2:9 NO:1 N:1 O:25

Panboy June 18, 2014 21:39

Quote:

Originally Posted by dreamchaser (Post 497702)
Hello Panboy and Beanlee,

I am doing the similar problem of doing hypersonic flow over a sphere of .2m. I am trying to input my chemical reactions. However, how do I put in the third body "M" into the reaction set?? For example, taking Beanlee's example below how would I input the third body "M" into Fluent? Would I just specify one reactant(O2) and one product(2O) and include the third body efficiencies??

I appreciate your help,

Dreamchaser

Dunn-Kang Model
02+M-2O+M
Af: 3.60E+15
Bf:-1
Eaf: 4.94E+08
Third body efficienies: N2:2 O2:9 NO:1 N:1 O:25

Yes you are correct, check the box for third body and input those values into the box correlated to the third bodies.

dreamchaser June 24, 2014 19:50

Quote:

Originally Posted by Panboy (Post 497707)
Yes you are correct, check the box for third body and input those values into the box correlated to the third bodies.

Hello Panboy,

Thanks for the reply.

I had another question with setting up the transport phenomena equations.
I am going off of literature and would like to use kinetic theory to find the fluid viscosity,thermal conductivity, and mass diffusion.

I am getting confused between setting properties for the mixture material (under the model tab) and setting properties for the individual species (under the material tab). For example, if I set the density to be ideal gas under the materials tab for each species, do I also need to set it under the mixture material section under the model tab?

These are the things I have done:

Under
Materials-->Fluid
1) I have put in all my species (e,N,O2,NO,O,NO+,N) using Parks air 7 model. For the Cp (specific heat) of each species I am using piece-wise polynomial and have used appropriate constants from literature. For each species, I have also set kinetic theory settings for calculating the thermal conductivity and viscosity. I have also set the density to ideal gas for each species since I am modeling compressible flow (Mach 38 over a sphere).

Under Models-->Species-->Edit-->Reaction
1) I have put in my reactions with the appropriate pre exponential factor, activation energy, and temperature exponent. I am using Park's air 7 model.

Under Models-->Species-->Edit-->Density
2) i have put ideal-gas since it is compressible (mach 38 over a sphere).

Under Models-->Species--Edit-->Cp (specific heat)
3) I am not sure what to put here. I have already included the polynomial coefficients for fitting a piece-wise polynomial for each species under the materials tab.

Under Models-->Species--Edit-->Viscosity
4) Here I do not see an option for kinetic theory?

Under Models-->Species--Edit-->Mass Diff

5) I have set this to kinetic theory

I would appreciate any insight you can provide.

Panboy June 25, 2014 20:14

Hey there, if you choose ideal gas under mixture and save it and reopen it then the option for density should not be there for any single species. It should only depend on the mixture ideal gas.

Did you input the correct Lennard Jones parameters for each species since you are using kinetic theory? Some of the defaults for Fluent are incorrect.

For the cp of the mixture I would choose mixing-law, it finds a cp dependent on the weight (mole fraction or something similar) of each species in the mixture.

For viscosity of the mixture I would choose Ideal-gas-mixing-law.

I would set the thermal conductivity of the mixture to ideal-gas-mixing-law also.

If you want to read up on what mixing law is, you can google it or look it up in the ansys manuals. Basically it finds one value for that parameter for a fluid that has many species.

Hope this helps. Let me know how it goes.

Panboy

dreamchaser June 26, 2014 18:38

Quote:

Originally Posted by Panboy (Post 498711)
Hey there, if you choose ideal gas under mixture and save it and reopen it then the option for density should not be there for any single species. It should only depend on the mixture ideal gas.

Did you input the correct Lennard Jones parameters for each species since you are using kinetic theory? Some of the defaults for Fluent are incorrect.

For the cp of the mixture I would choose mixing-law, it finds a cp dependent on the weight (mole fraction or something similar) of each species in the mixture.

For viscosity of the mixture I would choose Ideal-gas-mixing-law.

I would set the thermal conductivity of the mixture to ideal-gas-mixing-law also.

If you want to read up on what mixing law is, you can google it or look it up in the ansys manuals. Basically it finds one value for that parameter for a fluid that has many species.

Hope this helps. Let me know how it goes.

Panboy


Hi Panboy,

Thanks for the information.
I have followed your advice and made the following changes.

To clarify, the species I am considering consists of [e,N,O2,NO,O,NO+,and N2]. I was reading up that the Lennard-Jones Potential is a reasonable representation of the potential between nonpolar molecules. Since I have the ion NO+ (and I did not find any Lennard Jones Potential for any ions) should I just use Sutherlands Law for all of the species?

dreamchaser June 26, 2014 20:29

1 Attachment(s)
Quote:

Originally Posted by dreamchaser (Post 498881)
Hi Panboy,

Thanks for the information.
I have followed your advice and made the following changes.

To clarify, the species I am considering consists of [e,N,O2,NO,O,NO+,and N2]. I was reading up that the Lennard-Jones Potential is a reasonable representation of the potential between nonpolar molecules. Since I have the ion NO+ (and I did not find any Lennard Jones Potential for any ions) should I just use Sutherlands Law for all of the species?


Hello Panboy,

I just wanted to ask you about the setting of my boundary conditions and other Fluent settings.
To clarify, I am trying to model Mach 38 flow over a sphere. I am trying to model this at an altitude of 80km and have obtained the corresponding temperature and pressure at this altitude from tables which is 198.6K and 1.096Pa. First I just wanted to make sure I am choosing the right boundary conditions for my problem. I have attached a picture of my geometry which shows a solution which I obtained using CFD++.

1)In Fluent, I have defined the ‘inlet’ as a Pressure Far-Field. However, I am not sure if I am supposed to use a velocity inlet boundary condition. Here I have put in my Mach Number of 38 and have included a gauge pressure of 1.096Pa (corresponding to the freestream pressure since my operating pressure is set to zero.) Under the thermal tab I have set my freestream temperature to 198.6K. Under the species tab, I have specified O2 as a mole fraction of .23. I don’t see N2 listed (probably because I have listed it last in the mixture panel) but will assume Fluent will set this value to .77 thus mixing the composition of the freestream.

2) For the wall boundary condition, I have specified stationary and no slip. Under thermal I have set a temperature of 3000K with a heat generation rate of 0. I intend to first solve this problem with an isothermal setting.

3) For the ‘outlet’ I have specified pressure outlet with a gauge pressure of 1.052. However, I have a strong feeling that this should be outflow-vent.

4) I have used the axis boundary condition for ‘symm’ to model 2-D axis symmetric

My solution method is Implicit, AUSM, Least Squares Cell-Based and Second Order Upwind.

For my solution controls, I am not sure what the CFL number should be and have left it at a value of 5 and have made the under-relaxation factor a value of .9.

I am also confused about the Solution Control Limits. I sometimes get the message excessive temperature change and absolute pressure limited and suspect it has something to do with this setting.

Any advice for the settings for this problem would be greatly appreciated.
Thanks for your time,

Dreamchaser

Panboy June 26, 2014 20:31

I believe you can use sutherland's law but look into the derivation of it and make sure as I haven't work with it too much.

Panboy June 26, 2014 20:46

Everything should be set fine.

If N2 is your last species listed in the mixture, FLUENT will calculate the mole fraction by subtracting the sum of the mole fractions of the other species from one. You can verify that the initial settings are what you want by initializing your solution and before solving the solution go to results and plotting contours of the mole fractions and other variables to assure they are what you want.

I recommend dont changing under relaxation factors unless you have played with your CFL number and still cant get convergence. If you are having trouble converging, lower your CFL to 1 and possibly 0.1. I have done many simulations and rarely have to touch the under relaxation factors.

For the limits, if those messages dont disappear after a few thousand iterations I would limit the pressure and temperature to ranges not as drastic as FLUENT sets by default in order to help the solver not go too crazy with numbers and stay within a reasonable range while it solves.

lostinhypersonicspace July 21, 2014 13:55

Been running similar simulations...
 
Hi everyone,

I have been running similar simulations to:

http://www.cfd-online.com/Forums/flu...onic-flow.html

with little success. I am still having the "dasac error at temperature=..." error and don't quite know how to solve this. I have attempted turning on direct integration of the turbulence-chemistry interaction on, but this gives me worse results.

After having small success there, I am working on laminar flow similar to what has been described above. You have been helpful, thank you!

hesam.g September 27, 2014 11:33

Dear All..
I am trying to do a hypersonic flow simulation over a spiked blunt body at mach 6 using fluent 6.3
In my case, I use first order upwind scheme and get a very well converged solution. however, when I switch to second
order upwind scheme, totally diverge
Any one has some suggestion to resolve this problem?

Panboy September 29, 2014 20:54

Quote:

Originally Posted by hesam.g (Post 512156)
Dear All..
I am trying to do a hypersonic flow simulation over a spiked blunt body at mach 6 using fluent 6.3
In my case, I use first order upwind scheme and get a very well converged solution. however, when I switch to second
order upwind scheme, totally diverge
Any one has some suggestion to resolve this problem?

Can you look at your contour plots (pressure, temperature, velocity) and see where it is diverging and post a picture of it?

dreamchaser October 14, 2014 00:30

Quote:

Originally Posted by hesam.g (Post 512156)
Dear All..
I am trying to do a hypersonic flow simulation over a spiked blunt body at mach 6 using fluent 6.3
In my case, I use first order upwind scheme and get a very well converged solution. however, when I switch to second
order upwind scheme, totally diverge
Any one has some suggestion to resolve this problem?

Yes, please post some pics of the contour of your simulations.
I strongly believe your mesh is your problem. In hypersonic simulations, mesh is one of the most important things. I've had some many simulations not work because my mesh was bad. I assume that near your spike your mesh might need to improve.

First order will most likely always converge. However, the results will not be accurate at all and shock location will be wrong. You will need to switch to second order.

Also, I know in fluent, there is some kind of "hypersonic switch" which helps in setting up these problems.

Good luck


All times are GMT -4. The time now is 09:18.