[noepfy]

Hey everyone!

I am trying to simulate a Diesel-Engine with sprayEngineFoam using Openfoam 3.0. I have a mesh that works fine with engineFoam, but sprayEngineFoam leads to a weird temperature distribution during compression. As you can see in the attachment, at -10 degree CA, the temperature in the mold of the piston is 500K higher than in the liner.

Does anybody know why this happens? As I said, mesh and BC work fine with the engineFoam- solver (no temperature gradients during compression).

Thanks in advance,
Robert



Temperature_-10CA.jpg

[noepfy]

Apparently sprayEngineFoam calculates a wrong pressure- it should be around 40bar, but actually calculates 400bar . So there must be a problem with the solver?

[NablaDyn]

Hey guys,

has anyone found an explanation for this issue yet? I experience similar behaviour when running coldEngineFoam on an axisymmetric case.
I defined the walls as adiabatic (zeroGradient) and set up an initial uniform temperature distribution of 323 K. To my surprise, the overall temperature does not increase over compression, whereas pressure and density do. Even weirder, temperature decreases above the piston top area and increases in the bowl resulting in strong gradients. I am using OpenFOAM V4.1 and I already tested many different thermophysical configurations but the problem persists. Near the top dead centre, the temperature falls below the valid lower boundary of the applied JANAF table and the velocity field shows unphysical fluctuations (I'm doing RANS). Maybe someone found a solution to this - I think - very trivial solver issue?

I attached some postviews of my case.

Regards,

Martin

[NablaDyn]

I finally solved my problem:

As it turned out, the problem was with divergence schemes. I recklessly defined a "default" scheme (bounded, 2nd order accurate) that was applied to all divergence terms that haven't been explicitly addressed. After adding the explicit definitions

div(meshPhi,p) Gauss upwind;

and

div(phi,K) Gauss upwind;

the solver computed the temperature evolution as expected. Yet, I didn't have a closer look at which of both terms caused the issue.

Regards,

Martin

[sheaker]

Hello. It is good to know it is working for You now. I got some questions for You if possible. (It is understandable that you may not want or You can not share your hard work.)
1. Is Your pressure decreased to 40bar and filled entire combustion chamber?
2. Does Your simulation includes combustion or evaporation?
3. There is "mesh.move();" so Your simulation does not include topologically changeable grid?
4. How long Your simulation takes to simulate one revolution of crankshaft?
5. Can You run Your case in parallel?
6. Is Your case based on "scania tutorial" for dieselEngineFoam? If not, could You possibly share simplest test case?

I whish you further success!
Oskar

[blttkgl]

Originally Posted by noepfy

Apparently sprayEngineFoam calculates a wrong pressure- it should be around 40bar, but actually calculates 400bar . So there must be a problem with the solver?

I ran into the same issue with my own "myEngineFoam" solver created from stock only to realize that in Make/options engineFoam was including the pEqn.H from the sprayFoam solver, not sprayDymFoam. In OpenFOAM-dev these two solvers are merged now so it shouldn't be a problem, but for any previous release this unexpectedly high pressure error is most likely happening because the pEqn.H is taken from a non-dynamic solver.


Hope this helps anyone doing the same mistake.


Bulut