Compressor Simulation using rhoPimpleDyMFoam
Hi
I am simulating compressor stage of a turbocharger with the rhoPimpleDyMFoam solver. running moveDynamicMesh -checkAMI was smooth without any errors which assures that my mesh rotates properly and i have defined my interfaces correctly , please point out if i am assuming this wrong. However running the solver my simulation crashes showing this Code:
/*---------------------------------------------------------------------------*\ Thanks |
Coming to my simulation i have to simulate compressor stage of a turbocharger
Meshing was done using ANSYS ICEM CFD , i had 3 mesh files 1. Inlet&Outlet 2.Volute 3.Rotor I imported them to openfoam using fluent3DMeshToFoam and then used mergeMeshes to make the complete domain, after that used splitMeshRegions -makeCellZones -overwrite to distinguish between the rotating zone and stationary zone. I am attaching few pictures of the domain so you could get a clear picture.Please have a look at them |
1 Attachment(s)
This is the complete domain of my simulation
|
1. How are you merging your three meshes that you have imported from fluent?
2. How did you create AMI patches? 3. Do you have 'sets' folder (with several domains) inside the constant folder? |
@vasava
As i have 3 mesh files 1.I created 3 case folders 1.Rotor 2.Volute 3.Inlet_Outlet 2. Placed the 3 mesh files into corresponding case folders and used fluent3DMeshToFoam fluent.msh -scale 0.001 for each to convert to meters 3.merged Rotor and volute , and then merged the combined mesh with Inlet_Outlet 4.used splitMeshRegions -makeCellZones -overwrite to create cell zones of different regions , 3 in my case To create the AMI patches i used the createPatchDict, I will attach it for your reference Code:
/*--------------------------------*- C++ -*----------------------------------*\ |
Hi,
Your problem seems to be in the turbulence model, I am guessing you have put epsilon equal to zero somewhere in either a boundary patch or the internalField. Change this to a sensible value for your case. Regards, Tom |
Your mesh setup seems alright. I agree with tomf, get some appropriate values for turbulence and use them in initial condition.
Also can you post your boundary file here? |
Hi ,
Sorry for the late reply and thanks for your response I have checked my epsilon file and have not put zero anywhere and ya as you have suggested i am working on my initial and boundary conditions as this might be the source of error. @vasava Here is my boundary file Code:
FoamFile |
Quote:
The boundary file looks ok but did you try any other turbulence setup?? |
1 Attachment(s)
Hi vasava,
Do you mean any of these two? I started with K-Epsilon as it was the basic turbulence model to start with. 1.K-omega SST 2.Spalart-Allmaras I am attaching my 0 folder , please take a look at my initial and boundary conditions and help me correct them. I have copied and modified the files from annularThermalMixer tutorial. |
You have provided a relative pressure of 0 Pa, you should put the absolute pressure. OpenFOAM does not use a "gauge pressure" or similar for compressible solvers. The solver now tried to solve for an absolute vacuum, which it could not do. I guess it only found out when density was required to calculated some part of the turbulence model.
For incompressible cases 0 m2/s2 is allowed since in that case the absolute pressure does not matter. Regards, Tom |
Quote:
I changed the pressure file as suggested by you creating a pressure difference between inlet and outlet but i still end up getting the same error . Alexeym has suggested this might be the cause of my error: Hi, as you've got FPE in mutkWallFunctionFvPatchScalarField::calcMut(), look at the source of the wall function: Code:
tmp<scalarField> mutkWallFunctionFvPatchScalarField::calcMut() const 1. rhow[faceI] == 0 2. muw[faceI] == 0 3. k[faceCellI] < 0 4. E_*yPlus <= 0 (this is not the case, cause yPlus > yPlusLam_) So you need to check if any of conditions 1-3 is true in your case. I am able to figure out that these conditions come from the equations to have a proper solution but unable to understand which values i should correct.Please explain me if you can interpret what the problem exactly is. Thanks |
Could you just show the p file, I was not talking about a pressure difference between inlet and outlet, I meant that you cannot have 0 Pa anywhere in the domain (internalField or any boundary condition), it should be around your absolute operating pressure (101325 Pa for standard atmosphere conditions).
I guess it should look something like this: Code:
/*--------------------------------*- C++ -*----------------------------------*\ Tom |
@tomf,
Thank you very much. Just changed my p-file as suggested by you, now my simulation started running!! :) I was always worried about the mut-file , dint expect the error was in my p-file.:confused: For now the simulation is running but too slow,have to run it in parallel and maybe some changes in my fvSchemes and fvSolution will do. il come back to you in case of any queries, thanks a lot! |
Hi ,
I am simulating compressor of a turbocharger using rhoPimpleDyMFoam with kOmegaSST turbulence model. Boundary conditons are as follows: mass flow outlet : 0.04 kg/s total pressure inlet:101325 total temperature inlet:298k compressor rpm: 300,000 Can you help me with my FvSchemes and FvSolutions as to what modifications i should be doing for better results. let me know if you need any more details about the simulation. FvSchemes Code:
/*--------------------------------*- C++ -*----------------------------------*\ Code:
/*--------------------------------*- C++ -*----------------------------------*\ |
Whats the matter with your current results? Any problems?
|
Hi RodriguezFatz,
I have started running the simulation and each timestep is taking a lot of time. Is there anything to do with my FvSolution or FvSchemes files to speed up my simulation? I am already running it on 8 cores. |
So at least there is no problem ...
|
Hi tobi,
My simulation has been running from past 1 day and still going on Here is the output Code:
Courant Number mean: 0.000114809 max: 1 |
Hi,
my simulations are running on 40 cores 2 weeks ... But you time step is very small and your density is wrong (I think) Code:
rho max/min : 2 0.5 I dont know what because you do not share many details. You should check out you time steps... maybe your pressure, velocity, k, epsilon are expoding. As I can see, you should use the correct form of the PIMPLE algorithm. Maybe it will be stabilized. Checkout my blog or also available at the wiki. |
All times are GMT -4. The time now is 03:55. |