dieselFoam --> Janaf Error, what are the root causes?
Hello at all,
now I've spend a lot of time to understand how I can perform my own simulation with an injection similiar to the aachenBomb. So at first I run the aachenBomb test case and modified it to a different injected mass and mass rate. For the aachenBomb geometry it works. After this I decide to change the geometry to an cylindrical tube using a tet mesh. So this works also fine. But after modifying the tube to a more complex geometry I got the problem with the Janaf temperature error which is out of the specific range of 200 - 5000 K. Using a finer mesh this will not help. The simulation stops earlier then with a worst mesh? So the question is how I can identify the root cause of the Janaf Error? Is it related to the quality of the mesh? Which procedure you can recommend me to find the problem? Thanks in advance. pajofego |
Hi,
What exactly did you change? Did you only changed the domain or did you made some changes in BC and IC also? This error comes generally when something is wrong with your BC or mesh. If you are using the same BC as in the tutorial then have a look at your mesh. Run a "checkMesh" command and see what turns out. Also specify more details regarding your case, otherwise it would be difficult to advice. |
Hi,
in fact. I should give more informations about my case. I've only change the domain. The BC are all the same. That means like the tutorial all walls. Also I've change the Injector's properties - I would like to use a common rail injector: Code:
commonRailInjectorProps Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // pajofego |
Hi,
It might be possible that problem is with your mesh. Your Max. non-orhtogonality, although OK, is a little high, in my opinion. Try to modify your mesh, if possible. Keep your maxCo to 0.1 and then try to run. Also if possible upload an image of your mesh, especially the areas where there is skewness and non-orthogonality. Also you may use first order schemes in your fvSchemes file. |
I had problems running before as well. You could try to increase the number of parcels you are injection. Okay you only have 0.something milligrams but i would still recommend at least 100 000 parcels, maybe more.
|
So, I've done improvements regarding the mesh. I tried to use a structed hex mesh in gmsh, which is not really simple. It was possible to reduce the max. skewness up to 0.35 and I was able to run a simulation for a cylindrical geometry with a hex mesh. Tet meshes doesn't work for my geometry. I will upload a picture of the meshes that I used an I will also start a simulation with an increased parcel number. What is the benefit using a increased parcel number.
Thanks pajofego |
5 Attachment(s)
Hello at all,
I came back with my problem, after done some improvements regarding the mesh. It stills will not work! That's the last iteration before I got a floating point exception, instead of an janaf error Code:
Number of parcels in system.... | 9959 Here the output of checkMesh: Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // pajofego |
This error comes from this line in dieselFoam.C
Code:
volScalarField tk = You probably have some earlier warnings about bounding the epsilon equation. what you can do is to create a new field tk2 and limit that like below to calculate tk. Code:
volScalarField tk2 = turbulence->muEff()/rho/turbulence->epsilon(); |
All times are GMT -4. The time now is 23:04. |