Hello I am trying to simulk
 

Hello

I am trying to simulkate some validat cases at:
http://www.lerc.nasa.gov/WWW/wind/valid/cdv/cdv.html
using OpenFOAM. I successfully simulated cases 1 and 3.

But I could not simulate case 2. (I used pressureInlet and pressureOutlet BCs.) If I initializef with a subsonic flow, the flow remains subsonic all the time. I also tried intilaizing the flow field with the results of case 3, but it did not help. How can I capture shock in case 2?

Also, can I use mass flow outlet for supersonic flowa! Does openFOAM has such BC?

Thanks in advance
Varun

Hi Varun Which of the compr
 

Hi Varun

Which of the compressible flow solvers are you using?
I notice that cases 1 and 3 deal with isoentropic flow.

Regds
Srinath

Hi Srinath I am using sonic
 

Hi Srinath

I am using sonicFoam. I hope I am doing the right thing!

Varun

Varun Your solver seems to
 

Varun

Your solver seems to be correct
So questions are
1)Did you create geometry in blockmesh using splines? Are you running a 2-d case or an axisymmetric one?
2)Can u post the bc's you are using for U,T?
3)Are you running it for sufficient time?


Regards
Srinath

Hi Varun I have only 1 conc
 

Hi Varun

I have only 1 concern with the bc.
At the inlet, should you be specifying p,T and U?, since the u-a characteristic points outside the domain.
Hirsch recommends not using the combo (p,U) at a subsonic inlet. So just specifying (p,T) should do, U should come from the internal flow.
Now i don't know which of the choices in FoamX, implement a bc like this.

At the outlet, i beleive only pressue should be set, so i guess setting U,T at zeroGradient is ok

Srinath

Hi Srinath "Hirsch recommen
 

Hi Srinath

"Hirsch recommends not using the combo (p,U) at a subsonic inlet. So just specifying (p,T) should do, U should come from the internal flow."

I think this is exactly the bc that I am using currently. In OpenFOAM, a pressureInlet boundary type uses following consitions:

p : fixedValue
U : pressureInletVelocity
T : fixedValue


For "pressureInletVelocity", OpenFOAM documentation says that "When p is known at inlet, U is evaluated from the flux, normal to the patch"

The U "value" that is specified for "pressureInletVelocity" bc is just used for initialization : it has no other usage.

Varun

Hi Srinath I am extremely s
 

Hi Srinath

I am extremely sorry.

The validation case on the URL concers completely inviscid flow. I found out that I was trying solutions for viscous cases as I started reducing the viscosity towards zero, I got the normal shock in case 2.

Thanks a lot for help.

Varun

Hi Srinath Another observat
 

Hi Srinath

Another observation:

Although initially the normal shock starts from approximately the position shown on URL, it slows moves towards right and as I solve for a longer time, the shock stations itself just near outlet.

Any ideas on this?

Varun

Vikas Here is a good link f
 

Vikas

Here is a good link for converging, diverging nozzles.
As you change the pressure ratio, you could observe if you get similar trends(Does the shock position change as it should)
http://www.engapplets.vt.edu/fluids/...le/cdinfo.html

Also you could place a probe at the outlet and inlet to see if pressure is being maintained at BC values.
You can do this as per the following post.
http://www.cfd-online.com/cgi-bin/Op...3520#POST23520


Srinath

Hi Varun In your previous p
 

Hi Varun

In your previous post, you say

For "pressureInletVelocity", OpenFOAM documentation says that "When p is known at inlet, U is evaluated from the flux, normal to the patch"

Which document are you referring to?

Thanks
Srinath

Hi Srinath I was referring
 

Hi Srinath

I was referring to the description given here:

http://www.opencfd.co.uk/openfoam/doc/userse22.html

Varun

Hi Varun Did you find the p
 

Hi Varun

Did you find the problem?
Can you send the case directory, without the log files and time directories?
You can e-mail it to the id obtained by clicking on my name in the newsgroup posts.
You can include the time=0 directory, as it may be useful as an initial condition.
I can run it and see what happens.

Srinath

Hi Srinath Sorry for this l
 

Hi Srinath

Sorry for this late reply. I was out for a day ;).

Your link helped me a lot. If I set Pexit = 0.75 (case 2), the shock stands just near outlet, but as I start increasing this more the shock moves inward towards the throat and keeps oscillating (only a little) around this position. So the problem is solved.

If you are still interested in the case file, please let me know, I will mail you the files.

Thanks a lot for help. But I think, I will be needing more help from you ;). I have several other problems related to supersonic flow in openFOAM.

Varun

Hi Varun Good that you solv
 

Hi Varun

Good that you solved the cd nozzle problem. Could you send me the case file anyway. It would be nice to play with the problem parameters.
No problem regarding further problems in supersonic flow.

Regards
Srinath

Hi Srinath I just mailed yo
 

Hi Srinath

I just mailed you the files.

Varun

Hi there, you should know t
 

Hi there,

you should know that sonicFoam gives erroneous results - at least on 1.3. Did some tests on the case supplied in the tutorials, and for that case the speed of the shock (as well as the jump over the shock) is wrong (when compared to the exact solution or other solvers).

/jon

Hi Jon Could you give me a
 

Hi Jon

Could you give me a reference for the exact solution? Have you tested the other solvers(compressible/incompressible)

Regds
Srinath

Hi Jon It would be great if
 

Hi Jon

It would be great if could give the reference too.

Actually I tried some simple validation cases, like oblique shocks, normal shocks, that have analytical solutions and the OpenFOAM results come quite close to these analytical ones.

Also is this the case only with sonicFoam or with other compressible solvers (rhoSonicFoam, rhopsonicFoam) also.

Regards
Varun

As for exact solution, I used
 

As for exact solution, I used the one in

www.num.math.uni-goettingen.de/knopp/teaching_vorl_num_meth_ind_aero_ss2006.html

(a program in c, which was very easy to adopt to the case in the tutorial).

Also, you may want to check

http://openfoamwiki.net/index.php/TestLucaG

I tried sonicFoam, but judging from what I saw, that solver does not give the correct jump conditions. Just run the tutorial case on 1.3, but hopefully the solver in the later versions of OF is better.

Apart from the exact solution, I also used Edge

/www.foi.se/FOI/Templates/ProjectPage____4690.aspx

which, apart from an obvious "smearing" of the shock, gave the right speed of the shock.

It would be nice if you could test a later version of OF against the exact solution.

Regards,

Jon

Thanks Jon Could you give m
 

Thanks Jon

Could you give me a link for downloading centralFoam
I can't seem to find it even in the dev version.

Cheers
Srinath

Sorry, unfortunately I have
 

Sorry,

unfortunately I haven't used centralFoam.

Maybe write an email to Luca?

/jon

Hi Varun/Shri. I am also
 

Hi Varun/Shri.

I am also Using OpenFOAM for Past few months. I guess I may help you people with Central Foam.
RhoCentralFoam may solve your case in a better way..... I think.

Vishal.

Hi, Varun/Shri, In c
 

Hi,

Varun/Shri,

In case if you still need RhoCentralFoam I can Provide you. i am also working on the same.

Vishal