|
|
|
|
|
@andre: Any chance you can test with the latest OpenFOAM 2.3.1 or 2.3.x? I ask this because at least in OpenFOAM 2.3.x, there was at least one change to this tutorial, namely in commit f54ea84f6dd2dc0caa7cd7ee5ab92fe2b9201fbf, which can affect the proper set-up of the case. In addition, because this case is fairly computationally heavy (after 16714s, it has only done 1.12s of simulation in my machine, in parallel), I haven't managed to get the simulation up to the same point where you took the snapshots, namely at 2.0s. Attached is a snapshot "snapshot_at_1.1s.png" at 1.1s, executed with a recent OpenFOAM 2.3.x and it clearly seems to have heat transfer between the surfaces of the cubes and the surrounding environment. |
|
|
snapshot_at_1.1s.png (176,353 bytes) |
|
|
hotBoxes_2_3_x_latestGitPull.png (247,704 bytes) |
|
|
@wyldckat: Thank you for looking at this issue. Today I've done a git pull to get the latest version of OF2.3.x and ran hotBoxes in parallel. The hotBoxes stay cold (T=300 K) till t=0.3 s, then temperature switches to T= 350 K and stay hot. Okay so far. But in some locations on the boxes the minimum temperature is around 265 K, which isn't resonable (see attached figure). The temperatures should be in the range of [300 K , 350 K]. Using OF2.1.x the minimum temperature is 298 K. |
|
|
@andre: I didn't think 265K was very bad, since it's still very far from absolute zero :) But indeed, -8.15 degree Celsius seems fairly low for something that is initially in the range of 26.85 and 76.85 degree Celsius. I took a better look at the changes that occurred in the case set-up and the solver, and there is at least one particular big detail that was changed. In the file "constant/reactingCloud1Properties", the following entries are different: - OpenFOAM 2.1.x: flowRateProfile constant 0.1; Umag constant 3.0; - OpenFOAM 2.3.x: flowRateProfile constant 1; Umag constant 1; I'm currently running the tutorial in/from 2.1.x with "Allrun-parallel" with these values from the tutorial from 2.3.x, to try and isolate the origin of the problem... Wait... I saw just now for 0.058s that the surface film temperature is 300K on 2.3.x and 350K on 2.1.x, just as you said. This could be a mapping error between regions... I will continue to try and isolate the problem. |
|
|
OK, the good news is that tried the tutorial "lagrangian/reactingParcelFilmFoam/cylinder" and there is something weird happening with it as well... and this tutorial is substantially smaller and quicker to test! And the error is triggered after 10-15 seconds of running the solver! The not so good news is that I don't know yet where to look for the bug... all I know so far is that the Courant Number for the film shoots up at the time instance 0.56s, where output for each solver version at the end of this time instance is as follows: - OpenFOAM 2.1.x: time step continuity errors : sum local = 1.592753226e-11, global = -1.503420004e-14, cumulative = 8.290360465e-06 ExecutionTime = 14.71 s ClockTime = 14 s Courant Number mean: 0.001221796515 max: 0.008813443181 Film max Courant number: 0.05046019015 deltaT = 0.02 Time = 0.58 - OpenFOAM 2.3.x (commit 993cd4ee1298): time step continuity errors : sum local = 4.982300541e-12, global = 6.56421202e-14, cumulative = 3.267407582e-06 ExecutionTime = 11.05 s ClockTime = 11 s Courant Number mean: 0.001380531545 max: 0.009993486137 Film max Courant number: 7.030132775 deltaT = 0.001 Time = 0.561 With any luck, this bug is the same or very related to the one originally reported here. |
|
|
@wyldckat: in the hotBoxes-tutorial the boundary condition in htcConv has been changed. Could that be the cause of trouble? In the cylinder-tutorial there is no htcConv!? |
|
|
I have reverted the heat-transfer modeling in thermoSingleLayer back to how it was in OpenFOAM-2.1.x and this seems to resolve the issue report. I am not convinced either approach is correct and am running some more tests. I will push something you can try by the end of the day. |
|
|
Thanks for checking this case against older versions, this helped debugging. Resolved by commit 1f187d6f9e58c232a1363aafe4ffe46e6f20f876 thermoSingleLayer: Revert q back to the working version in OpenFOAM-2.1.x Revert changes in tutorial to correspond to the version in OpenFOAM-2.1.x Resolves bug-report http |
- Anonymous
