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 ke,Realizable ke and SST kw turbulence models During iterations it says temperature and pressure limited to default values(ofcourse that are in limit panel), sometimes it says timestep 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 
use invisid for compressible flows

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

Quote:
Do 
@ 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 
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:

@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 
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 
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 1e6 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 
@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?? 
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 
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.

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. 
Quote:

Quote:

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 04:13. 