CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   rocketFoam (http://www.cfd-online.com/Forums/openfoam/81469-rocketfoam.html)

 TRT October 27, 2010 16:14

rocketFoam

Hi you all

We, Terrassa Rocket Team or TRT, are a team formed by students of engineering in aeronautics involved in a project whose aim is to build a rocket capable of lifting a 1 kg payload to an altitude of, at least, 100 km if launched from a balloon launcher, which is being developed by another team of students.

One teammate and I are by now in charge of obtaining aerodynamic forces produced on our rocket model by using OpenFOAM. So far, after completing the Cavity tutorial and learning the basics, we have been able to mesh a domain with our rocket model inside it by using snappyHexMesh, and run a simulation using the simpleFoam solver.

Given this situation, now we face the following problems.

1st) We have been unable to run the case in rhoSimpleFoam (always because of a floating point exception). Although the incompressible solver may give us an approximate magnitude of the forces involved, it would be great if we could run it compressible.

2nd) We still need to find a way of computing resulting forces on the rocket, or their coefficients.

Although after a quick search several possible options arose for the second problem, we'll be soon facing our partial exams for this quarter, and thus further testing is stopped until their end on November, Friday 12, 2010.

By the meanwhile, if you could share any advice on the matter, that would be really great, we'll thank any kind of help.

Finally I'd like to show you this images from our simulation using a free stream at 200 m/s and a 10° angle. Surface color by p, streamlines color by U.

http://i167.photobucket.com/albums/u148/Ruja/TRT/1.png
http://i167.photobucket.com/albums/u148/Ruja/TRT/2.png

Note the mesh is still coarse, since we've been running only test cases.

TRT

This is our blog: http://terrassarocketteam.blogspot.com/

 colinB October 29, 2010 06:09

Hi guys,

sounds interesting what you are doing.

Concerning the floating point exception:
how is your courant-number doing? is it exceeding?
Anything above 1 for OF is exceeding. I'm not sure if there is a specific
recommended value for your solver or not but I usually try to keep it lower than
0.8. So maybe check your time steps and mesh density again.

to the second problem with the forces.
I calculate my (buoyant) forces on a ship hull with an appendix to the controlDict
file:

Code:

```maxCo          0.8; maxAlphaCo    0.8; maxDeltaT      1; // ************************************************************************* // functions (         forces         {                 type forces;                 functionObjectLibs ("libforces.so"); //Lib to load         outputControl    timeStep;         outputInterval 1;                        patches (B319_comp_patch0); // change to your patch name                 rhoInf 1000; //Reference density for fluid                 nuInf 1e-6; //Reference kinetic viscosity for fluid                 CofR (0 0 0); //Origin for moment calculations         }         forceCoeffs         {                 type forceCoeffs;                 functionObjectLibs ("libforces.so");                 outputControl  timeStep;         outputInterval 1;                 patches (B319_comp_patch0); //change to your patch name                 rhoInf 1000;                 nuInf 1e-6;                 CofR (0 0 0);                 liftDir (0 0 1);                 dragDir (-1 0 0);                 pitchAxis (0 1 0);                 magUInf -7.1;                 lRef 1;                 Aref 1;         } );```
note that the first lines are the last lines of the regular controlDict file so you know where to put these lines.
However I didn't code these lines myself and I'm not familiar with what kind of forces
you need in particular. So maybe you have to do some adjustments and/or do
something completely different. This is just a hint and not the necessarily the absolute truth ;)

I hope I could help and did not confuse you
best regards
Colin

 TRT November 16, 2010 08:15

Hi, colinB

Thanks for your advice. About the compressible solver, I believe too that the origin of the problem is the coarse mesh we are using at this point. We'll try to refine it as well as reduce time steps too, and check again if it works.

And about the forces, I had a "U, p or rho not found in database - De-activating Forces" problem until I added the following line to the script you posted, just before "rhoInf"

"rhoName rhoInf;"

I believe this happens because of using OpenFOAM version 1.7.1, but I'm not completely sure about that. After adding that line it worked like a charm.

Thanks for reading and for your help again.

TRT

 All times are GMT -4. The time now is 22:16.