CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   problems in modeling hypersonic flow (http://www.cfd-online.com/Forums/fluent/85559-problems-modeling-hypersonic-flow.html)

cfd seeker March 1, 2011 12:45

problems in modeling hypersonic flow
 
hi all

i am trying to model hypersonic flow over 2D cone of length 0.5m, diameter 0.15838m and half cone angle of 9 degrees.

M.No=6.77
density based,implicit and steady solver
i have used Standard k-e,Realizable k-e and SST k-w turbulence models

During iterations it says temperature and pressure limited to default values(ofcourse that are in limit panel), sometimes it says time-step reduced in some cells due to excessive temperature change. After some iterations solution diverges and iterations stop by saying that floating point exception

I dont know where i am going wrong. Please give some suggestions as i am really stuckup.

I have to find CL,CD,CM values for 0 and 60 degrees angle of attack

smartnatu March 1, 2011 20:23

use invisid for compressible flows

DoHander March 1, 2011 22:06

A few suggestions:

1. First check your mesh and be sure all the boundary conditions are correctly defined.
2. Try again with the 3 turbulence models you've used, however switch from Roe to AUSM for the numerical flux calculation (sometimes for high speed flows Roe will give non physical results).
3. Try also the Spalart Allmaras turbulence model.

If nothing works upload your cas and dat files, maybe someone will take a few minutes to check if all your settings are OK. It is difficult to give advices when you don't see exactly the problem specification (I mean mesh and Fluent settings).

Do

cfd seeker March 2, 2011 02:00

@ smartnatu
thanx mate for replying, ok i will try your suggestions and then let you know.

cfd seeker March 2, 2011 02:13

@ DoHander
thanx mate for your suggestions
here i will like to add something as you are talking about mesh and boundary conditions

1. My flow domain is 3 body lengths forwrad, 3 body lengths upwards, 3 body lengths downwards and 6 body lengths backwards (body length is 500mm)

2. I have kept mesh very fine near the walls( i.e body) and courser towards the boundries.

3. I have used Pressure farfield boundary conditions for inlet,top and bottom boundries and Pressure outlet for outlet boundary

4. Operating pressure is 101325 Pa and Guage pressure is 0(zero) in Pressure farfield and Pressure outlet boundries.

I hope my problem settings are very much clear to you
Your suggestions are very good and i hope you will give some more good suggestions after reading this post.

chengdi March 2, 2011 05:51

Check the limits value in solver settings

usually, I set the interval of pressure as [90% of inlet static pressure, 110% of inlet total pressure]

so as the interval of temperature: [90% of inlet static temperature, 110% of inlet total temperature], (assuming there is no combustion, heat transfer or serious seperation)

These values is easy to acquire if you follow the physics.

And keep other limits default.

Quote:

Originally Posted by cfd seeker (Post 297506)
hi all

i am trying to model hypersonic flow over 2D cone of length 0.5m, diameter 0.15838m and half cone angle of 9 degrees.

M.No=6.77
density based,implicit and steady solver
i have used Standard k-e,Realizable k-e and SST k-w turbulence models

During iterations it says temperature and pressure limited to default values(ofcourse that are in limit panel), sometimes it says time-step reduced in some cells due to excessive temperature change. After some iterations solution diverges and iterations stop by saying that floating point exception

I dont know where i am going wrong. Please give some suggestions as i am really stuckup.

I have to find CL,CD,CM values for 0 and 60 degrees angle of attack


DoHander March 2, 2011 09:31

Quote:

Originally Posted by cfd seeker (Post 297584)
@ DoHander
thanx mate for your suggestions
here i will like to add something as you are talking about mesh and boundary conditions

1. My flow domain is 3 body lengths forwrad, 3 body lengths upwards, 3 body lengths downwards and 6 body lengths backwards (body length is 500mm)

2. I have kept mesh very fine near the walls( i.e body) and courser towards the boundries.

3. I have used Pressure farfield boundary conditions for inlet,top and bottom boundries and Pressure outlet for outlet boundary

4. Operating pressure is 101325 Pa and Guage pressure is 0(zero) in Pressure farfield and Pressure outlet boundries.

I hope my problem settings are very much clear to you
Your suggestions are very good and i hope you will give some more good suggestions after reading this post.

Try to use pressure far field for all boundaries, also the operating pressure should be 0 (a non-zero value is useful in low speed flows, read the Fluent help page about operating pressure and the tutorial about compressible flow).

Do

cfd seeker March 2, 2011 10:28

@ DoHander
ok mate i will also try with 0(zero) Operating Pressure and also Pressure farfield at the outlet.

here i will like to ask one more thing, in your previous post you mentioned about switching from Roe to AUSM, can you shotly explain th effect of this as i have to calculate CL,CD,CM values for the body at 0 and 60 degrees angle of attacks

chengdi March 2, 2011 12:15

the Mach No. of your case is too large for fluent...

Considering your flow field is supersonic, you can use a <| shape calculating domain and make sure every boundary is pure inlet or outlet.

Quote:

Originally Posted by cfd seeker (Post 297584)
@ DoHander
thanx mate for your suggestions
here i will like to add something as you are talking about mesh and boundary conditions

1. My flow domain is 3 body lengths forwrad, 3 body lengths upwards, 3 body lengths downwards and 6 body lengths backwards (body length is 500mm)

2. I have kept mesh very fine near the walls( i.e body) and courser towards the boundries.

3. I have used Pressure farfield boundary conditions for inlet,top and bottom boundries and Pressure outlet for outlet boundary

4. Operating pressure is 101325 Pa and Guage pressure is 0(zero) in Pressure farfield and Pressure outlet boundries.

I hope my problem settings are very much clear to you
Your suggestions are very good and i hope you will give some more good suggestions after reading this post.


cfd seeker March 3, 2011 02:16

@DoHander
when i performed analysis for 0(zero) degree angle of attack my result came out to be v good but problems arises when i started analysis at 60 degree angle of attack

then my friend suggested that i should start with some subsonic M.No and i choose M.No=0.6. The results at this mach also came out to be very good for 0(zero) degree angle of attack but i am facing problems at 60 degree angle as drag and lift curves are oscillating between very high values(illogical values)

Does this mean that very high angle of 60 degrees is affecting the physics of this problems???

suggestions from any body will be highly welcomed as i am really stuckup with it. thanks

cfd seeker March 3, 2011 03:28

i also want to ask 1 more simple question about Reference values for the calculation of coefficients

diameter of geometry is 0.15838m and its length is 0.5m

in Reference values panel i set the Area=pi*d^2/4=0.0197
Length=0.5m

i want to ask what should i set for Depth value in my case?? shouldi i set Diameter as depth in my case

Shamoon Jamshed March 5, 2011 13:38

Dear cfd seeker

Your problem is not very difficult. Do this step by step

1) IS your problem a wedge or a cone? If its a wedge specify the front bottom near the nose tip as wall
IF its a cone specify it as axis

2) Try to setup air as ideal gas , Sutherland and thermal conductivity calc using kinetic theory.
3) Start with low Courant number
4) In meshing do not use very high clustering near the wall 1e-6 m is enough
5) First try to solve inviscid. At least till the flow develops.
6) If Roe FDS doesn't work shift to AUSM
7) Reference value of area should be the pi r*r.

Hope this will help

cfd seeker March 7, 2011 03:07

@Shamoon Jamshed
thanx for your suggestions. ok i will try these and let you know my progress. but how does very fine grid is not good near the walls??

cfd seeker March 29, 2011 10:50

today i feel i should come back here and post something about my solution for the benefit of others.
By decreasing Courant Number and Under Relaxation Factors has solved all my problems

Shamoon Jamshed March 29, 2011 12:10

congratualtions
 
OK fine very good. Regarding your question about near wall refinement. I have seen that if the mesh is very fine near wall but the lateral lenght of the cell is very big for example y+=1 but del x+ =1000 this has very high aspect ratio and that creates residuals to fluctuate so you have to compromise in between i.e not very big cells length wise nor very loose mesh near wall. Fingers crossed for your case.

cfd seeker April 1, 2011 02:05

thanx Jamshed
actually in my case solution variables were varying so much from one iteration to the other that fluent was unable to cope with it and so fluent was giving floating point exception. so by decreasing the courant no. and under relaxation factors helped the fluent to solve the problems in small steps and consequently the solution gets stable.

now Jamshed i also want to learn in detail about all turbulence models, their wall y+ requirements(how wall y+ is managed) and about near wall functions and treatments. so can u help me by providing me your some personal experiences,notes or any thing from where i can learn about these things.

Centurion2011 September 13, 2011 04:48

Quote:

Originally Posted by DoHander (Post 297564)
A few suggestions:

1. First check your mesh and be sure all the boundary conditions are correctly defined.
2. Try again with the 3 turbulence models you've used, however switch from Roe to AUSM for the numerical flux calculation (sometimes for high speed flows Roe will give non physical results).
3. Try also the Spalart Allmaras turbulence model.

If nothing works upload your cas and dat files, maybe someone will take a few minutes to check if all your settings are OK. It is difficult to give advices when you don't see exactly the problem specification (I mean mesh and Fluent settings).

Do

I agree with that. I made simulation for supersonic flow (4 Mach) for irregular shape body, used AUSM, Green-Gaus cell based setup and after some 6000 iteration solution converged.

Shamoon Jamshed September 13, 2011 21:31

Quote:

Originally Posted by cfd seeker (Post 301776)
thanx Jamshed
actually in my case solution variables were varying so much from one iteration to the other that fluent was unable to cope with it and so fluent was giving floating point exception. so by decreasing the courant no. and under relaxation factors helped the fluent to solve the problems in small steps and consequently the solution gets stable.

now Jamshed i also want to learn in detail about all turbulence models, their wall y+ requirements(how wall y+ is managed) and about near wall functions and treatments. so can u help me by providing me your some personal experiences,notes or any thing from where i can learn about these things.

I suggest that as far as I have seen that y+ for each and every turbulence model should be equal to one. Try to get it as much as possible closer to one and then if you don't get then go for the limits of y+ set up for each turbulence model.

christina1990 April 21, 2014 01:28

hypersonic fluent
 
hi .....
Shamoon Jamshed, DoHander...
I want to simulate hypersonic flow with Fluent with this condition(Pstat=2000pa,Tstat=60k, M=6)......for this condition Fluent can simulate and correct solution???
with out UDF???

Please help me.....thanks


All times are GMT -4. The time now is 03:48.