Overestimated temperature values
3 Attachment(s)
Hello foamers!
I came up with a following problem: during simulation of pouring hot melt into the casting mold I got a temperature values bigger than pouring temperature! My BCs are only fixedValue at the inlet and at the walls of mold (where temperature is lower than at the inlet), and zeroGradient at nozzel boundaries, flat fixed top "freesurface" and at the outlet. Here are the snapshot, where red color indicates overheated cells. From top comes nozzel, flat top interface is with zeroGradient BC, vertical mold is with constant temperature BC: Attachment 2599 Attachment 2600 So you can see from second picture, that difference in temperature is ~30 K over pouring value, which is not appropriated. The problem arises also from other surfaces with zeroGradient BC. For example from outer wall of submerged part of the nozzle: Attachment 2601 Where can this problem come from? I don't have any sources of heat, and energy equation contains only energy dissipation parts: DT/Dt = div(alpha_eff grad(T)) My idea was that error comes from gradient schemes due to non-ortogonality of the mesh. I use following fvSchemes: Code:
/*--------------------------------*- C++ -*----------------------------------*\ |
I'd give a try with limiters on the gradients and laplacian.
The mesh is not orthogonal, but it is not skewed either from the detail you showed. Please let us know what you find. Best, |
1 Attachment(s)
Alberto,
I have followed your advice. First please check if I understood you correctly. So, I modified fvSchemes Code:
gradSchemes Attachment 2628 It represents same geometry with box slice cutted out to see what is going on You can see still overheated cell indicated, T error ~10 K. Waiting for your comments and following advices! |
1 Attachment(s)
I have found that not a diffusion, but convectional part produces wrong values.
So I splitted energy equation following way: dT1/dt + div(phi, T1) = 0 (1) dT2/dt = div(alpha_eff * grad(T2)) (2) Below are the results only transport equation (1) at the left picture, and equations (2), which accounts only for diffusion at the right picture respectively. "dT" value means temperature overestimation value (above pouring temperature). Flow is present in both cases, it's direction is shown with arrows in the picture on the right. Attachment 2768 All schemes which I used for such test are without limiting. So what are your suggestions in that case? There is nothing about limiting divergence nonorthogonality corrections in either User or Programming Guides. Here I use for equation (1) following divergence scheme: Code:
div(phi,T1) Gauss linearUpwind Gauss linear; |
Quote:
in the first fvSchemes you posted, you were using upwind interpolation, which is limited by definition, since you simply use the upwind cell center value on the face. If you use linearUpwind, you can additionally limit the gradient as shown here ( http://www.cfd-online.com/Forums/ope...earupwind.html ), using Code:
div(phi,T1) Gauss linearUpwind cellLimited Gauss linear 1; |
Alberto!
Thank you very much for such immediate response! I will try your suggestions and report here the results. |
Just one additional thought: did you try to re-mesh the part? What mesher did you use to generate the grid that gives you problems?
Best, |
It was a Gambit, so actually mesh is the third part product, I should not change it...
Btw, I have already tried Quote:
Alberto, what is your opinion regarding reasons, which can cause such problems with a simple scalar transport equation? Just for additional information, here is output of checkMesh: Code:
Mesh stats Code:
Mesh stats |
Quote:
Was this mesh working OK in FLUENT if you tried it? Best, Alberto |
FYI, similar problems on meshes with tets were described her:
http://www.cfd-online.com/Forums/ope...foam-tets.html Best, |
Alberto, thank you for reference!
I will comment there to join our effort. |
A have a following question:
Is there any reason why we solve energy equation in buoyantBoussinesqPisoFoam after momentum predictor and not after pressure and mass flux correction? Have a nice weekend! Best, Alexander |
Quote:
Best, |
All times are GMT -4. The time now is 20:56. |