|
[Sponsors] |
March 12, 2020, 04:37 |
DLR F6 solution not converging
|
#1 |
New Member
Aqib Aziz
Join Date: Mar 2020
Posts: 15
Rep Power: 6 |
Greetings all,
I am a masters student of aerospace engineering and i am a learner of fluent. currently i am working on simulations for DLR F6 wingbody junction, a project present in drag prediction workshop. I have done structured meshing of my model and quality of mesh is okay. For the last 15 days i am working on fluent in order to get a converged solution for my model so that i can compare the lift coefficient, drag coefficient and surface pressure distribution with the experimental results present in drag prediction workshop. According to DPW i must get lift coefficient of 0.5 at Mach 0.75, but my solution goes to 0.5 value and then start to diverge to a small value and keeps on diverging. Following are the boundary conditions that i have set: Inlet: pressure farfield, Mach 0.75, angle of attack 1 degree Outlet: Pressure farfield, Mach 0.75, angle of attack of 1 degree Side: Pressure farfield, Mach 0.75, angle of attack of 1 degree Symmetry: Symmetry i have used courant number of 0.5, i have used sparalat Allmaras model of turbulance, density based solver. After some iterations, console window says negative nut value found in 2 cells after linear solve and sometimes 3 or 4. i have completed 12000 iterations but still i am not able to converge my solution to any single value. it just keep getting down and after some time starts to go up but no stable value achieved yet. If you know the solution of this problem or you have any helpful suggestion for me then reply me to overcome this problem. Thanks Regards |
|
March 12, 2020, 06:41 |
Solver at M 0.75
|
#2 |
Senior Member
|
Though density based solver can be used at any Mach number, it is recommended to use pressure based for M < 2. You can certainly work with density based solver as well, however, this would require a better initial field and may be solution steering.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. |
|
March 12, 2020, 12:39 |
solver at M 0.75
|
#3 |
New Member
Aqib Aziz
Join Date: Mar 2020
Posts: 15
Rep Power: 6 |
Okay i will try to do simulations using pressure based solver as well. is there any other thing that might be the reason why my solution is not converging. i mean any mistake in the details that i mentiined about my model?i appreciate your suggestions
|
|
March 12, 2020, 14:52 |
Case Setup
|
#4 |
Senior Member
|
Rest of the setup appears alright. Ensure that the ideal gas law is used for material density and operating pressure is set to 0. Try using fmg initialization. If the fmg initialization is successful, then the simulation should run fine. If not, then there is some issue with the setup.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. |
|
March 12, 2020, 23:52 |
Thanks
|
#5 |
New Member
Aqib Aziz
Join Date: Mar 2020
Posts: 15
Rep Power: 6 |
Thank you so much for your kind help. i will do as you told me and if i have any problems then i will reply you if you do not mind 😊
|
|
March 12, 2020, 23:58 |
initialization
|
#6 |
New Member
Aqib Aziz
Join Date: Mar 2020
Posts: 15
Rep Power: 6 |
i have used standard initialization and compute from inlet. the operating pressure is 0. is it okay?
|
|
March 13, 2020, 02:07 |
error in simulations
|
#7 |
New Member
Aqib Aziz
Join Date: Mar 2020
Posts: 15
Rep Power: 6 |
when i tried to use pressure based solver, it gives error that says floating point exception and also a warning that limited wall distance for 2361 cells to 10^-12. what should i do noe brother?
|
|
March 13, 2020, 03:28 |
Mesh
|
#8 |
Senior Member
|
Did you create an extremely fine mesh? Limiting the wall distance means you have boundaries with very small or highly skewed cells. Run a mesh check in Fluent and then may be try a case with lower Mach number.
Standard Initialization is not good for such cases. Use fmg-initialization. You have to use command to do that solve init fmg-init
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. |
|
March 13, 2020, 03:44 |
Mesh check
|
#9 |
New Member
Aqib Aziz
Join Date: Mar 2020
Posts: 15
Rep Power: 6 |
okay brother i will check the mesh quality and i will also run fmg initialization. lets see if i get my problem solved
|
|
March 13, 2020, 04:09 |
Mesh problem
|
#10 |
New Member
Aqib Aziz
Join Date: Mar 2020
Posts: 15
Rep Power: 6 |
brother i have check the orthogonality of my mesh. when i check it in icem, it shows min of 0.38 but when i convert it into unstructured mesh and import in fluent, it shows a very low min orthogonality of the order of e^-7 and gives warning the orthogonal quality is below 0.01.what is this matter brother?can you tell me why is this happening?
|
|
March 13, 2020, 04:24 |
Orthogonal Quality
|
#11 |
Senior Member
|
ICEM and Fluent have their own definitions of orthogonal quality. If Fluent observes OQ below 0.01, it would be difficult to get good results. With 1e-7, it's better to improve the mesh. Closer to 0.01, you can still work with Fluent using low URFs and/or Node based gradients. Furthermore, try to improve skewness of the mesh; skewness is more important than OQ.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. |
|
March 13, 2020, 07:05 |
Mesh problem
|
#12 |
New Member
Aqib Aziz
Join Date: Mar 2020
Posts: 15
Rep Power: 6 |
Thank you so much brother. i will work on improving skewness and orthogonality and then do my simulations. Thanks for your advice 😊
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Converging on wrong solution | gdbb89 | COMSOL | 2 | September 12, 2018 00:01 |
Solution not converging | dhands | FLUENT | 0 | April 25, 2014 14:04 |
SU2_EDU version solution not converging.. | akanoria | SU2 | 2 | March 4, 2014 05:49 |
My steady state solution converges for a while but stops converging | C.C | Fluent UDF and Scheme Programming | 0 | October 9, 2013 11:11 |
Wall functions | Abhijit Tilak | Main CFD Forum | 6 | February 5, 1999 01:16 |