![]() |
1 Attachment(s)
Quote:
Hi tobi, My density is calculated based on inlet pressure and inlet temperature and it is 1.1845kg/m3. I have taken the FvSchemes and FvSolution files from the annularThermalMixer Tutorial under rhoPimpleDyMFoam as i am using the same solver and modified them. Can you please explain what values i should be giving for rho max/min: for my case. My time step is calculated using courant no. formula co=delT*U/delX I have set co max=1, my maximum velocity =78m/sec calculated using v = w*r w=31415 rad/sec , radius of impeller r = 5cm. min cell volume from my mesh is 5.37e-16 so delX is approx =8e-06, delT i found is 5.2e-09.Is this the right approach??? I have invested a lot of time in setting up my boundary conditions in the 0 folder. Attached is my 0 folder , please take a look and correct me if there is anything wrong. You can also find detailed explaination of my simulation in this thread http://http://www.cfd-online.com/For...ledymfoam.html Thanks |
Quote:
@Bruno - please move all posts refered to Jetfire question to the given thread. @Jetfire - double posts are not wished I will answer you in your thread! PS your link is wrong |
|
Hi,
Since Tobias uses this solver he will probably be the better contact, but here are some general things:
|
Hello,
some hints and question:
Code:
// Recalculate density from the relaxed pressure Code:
rhoEqn max/min : 2.15688 0.182153 . Code:
rhoMin rhoMin [ 1 -3 0 0 0 ] 0.5; As I told you befor, you should use the correct PIMPLE ALGO with underrelaxation. I refer (again) to my blog or to the wiki. There you will get how to set up these parameters: Code:
PIMPLE Code:
AMI: Creating addressing and weights between 1900 source faces and 32076 target faces Did you ever checked out if your mesh is okay? Code:
checkMesh -constant Code:
moveDynamicMesh -checkAMI
|
Hi Tobi,
Thanks for your reply Meshing was done using ANSYS ICEM CFD and the simulation was already run on CFX which gave good results.My task is to simulate the same on OpenFOAM. Code:
Did you ever checked out if your mesh is okay? I have even checked whether my AMI Interfaces were correct using moveDynamicMesh -checkAMI and it had run without any errors. Checked the compressor rotation on ParaView and the rotation was fine. Coming to my AMI Interfaces , i too have noticed that weights are not 1:1 but that is due to one interface on compressor being meshed with hex and it's neighbour interface on volute being meshed with tet elements. But as long as there is some weight matching the weight on target faces it is fine. This is not a problem as i have checked with moveDynamicMesh -checkAMI and it ran perfectly , otherwise i would have got errors there itself. Please look at the mesh domain i have posted earlier in this thread.There is only one rotating zone but there are 3 interfaces. 1. inlet and rotor 2.rotor and volute 3.connection between volute and outlet |
Quote:
-> red Line is wrong (SEE BELOW) Quote:
|
Hi,
good to know, well done. So then its clear that you have different faces. But you are not using PIMPLE as I told you 2 times befor. Have a look into the blog, wiki. Code:
Create mesh for time = 0 |
Quote:
Quote:
|
Quote:
|
Hi tobi,
I do not know what min or max rho for which calculation be done So according to you do i have to remove these lines from the pEqn.H file??? Code:
rho = thermo.rho(); Code:
rhoMin rhoMin [ 1 -3 0 0 0 ] 0.5; |
Hi Phillip,
sorry my fault (: I mixed the things up!
I wanted to say to use that one: Code:
Gauss linear limited 1 = Gauss linear uncorrected
|
Quote:
First you calculate your density: Code:
rho = thermo.rho() Code:
rho = min(rho, rhoMax) rho = 0.43 » 0.5 rho = 2.13 » 2.0 If the values are correct you have to change the cutted parameter in the fvSolution! At least - please read the blog or wiki for PIMPLE! |
Hi,
I have nowhere mentioned PISO algorithm, i dont understand why it is running it in PISO.Can you help me understand what changes i have to make to run it on PIMPLE. |
It's the "nOuterCorrectors". If set to "1", this is the same as running PISO algorithm. If set >1, it actually runs in real PIMPLE mode.
Solver PIMPLE solves multiple iterations of solver PISO during each time-step. So, if you just solve a single iteration of PISO (nOuterCorrectors=1) each time-step this comes up to PISO. |
I am not able to open your blog , i get this :(
Your host needs to use PHP 5.3.10 or higher to run this version of Joomla! |
Quote:
If you want to use PIMPLE and how it is working - go to my blog. I think you are too lazy to click on my blog on the left of that post :D so I be kind: BLOG WIKI I hope you will check it out now. There is everything mentioned - also like Philipp told you! You do not use the PIMPLE loop due to your settings in your fvSolution. Blog is on cfd-online :p |
Checking it now :)
I really thank you both for taking out your precious time and helping me out. Thanks a lot! |
Does the omega-bounding vanish, if you use the laplacian-setting I suggested?
|
Hi,
Sorry for the late reply , i was not at the work station for the rhomin/max , with reference to the air properties at atmospheric pressure in the link http://www.engineeringtoolbox.com/ai...ies-d_156.html I think my rhomin/max should not exceed the limits 0.524/2.793. But looking at the output there are timeSteps deviating from this for example. Code:
rhoEqn max/min : 2.15688 0.182153 . . GAMG: Solving for p, Initial residual = 1.49854e-09, Final residual = 1.49854e-09, No Iterations 0 rho max/min : 2 0.5 |
All times are GMT -4. The time now is 04:44. |