View Issue Details
| ID | Project | Category | View Status | Date Submitted | Last Update |
|---|---|---|---|---|---|
| 0003457 | OpenFOAM | Bug | public | 2020-02-19 20:08 | 2020-02-25 20:56 |
| Reporter | sjohn2 | Assigned To | henry | ||
| Priority | normal | Severity | minor | Reproducibility | sometimes |
| Status | resolved | Resolution | fixed | ||
| Platform | GNU/Linux | OS | Ubuntu | OS Version | 15.04 |
| Product Version | dev | ||||
| Fixed in Version | dev | ||||
| Summary | 0003457: Error in boundary condition prghTotalPressure | ||||
| Description | The field varible 'p' picks up a uniform value of p0 specified in prghTotalPressure boundary condition in field p_rgh. At the inlet p_rgh is a non uniform scalar field while p is a uniform field. This leads to abnormality in the internalField. | ||||
| Steps To Reproduce | re-run case files attached | ||||
| Tags | No tags attached. | ||||
|
|
|
|
|
solver is reactingTwoPhaseEulerFoam |
|
|
In a p_rgh solver p should have calculated BCs so that it is calculated from the current p_rgh and rho distributions. It is not clear why you the field varible 'p' picks up a uniform value of p0 if the 'p' BCs are calculated. |
|
|
Please check the boundary field 'p' after 0.01 seconds It is picking up INLET { type calculated; value uniform 514174; } instead of values based p_rgh. On a seperate note, in the p_rgh file after 0.01 seconds, if I uncomment lines // phi phi.liquid; // rho thermo:rho.liquid; in the inlet field at initial time, I found that p_rgh also picked up value uniform 514174; which is basically p0 at the inlet after 0.01 secs. Note : there is not volume fractions of gas phase in the inlet |
|
|
In what way are the p values not based on p_rgh? Can you provide a patch which changes the BC how you want it to be for us to consider? |
|
|
I did not mean to say that the p values are not based on p_rgh. Can you run the original case till 0.001 secs and check the boundary field p. They are taking a uniform value of 'p0' and please compare it with the boundary field of p_rgh at the same time. |
|
|
I am not aware of any problem in either the prghTotalPressure BC or the evaluation of p. See if you can reproduce the problem in one of the tutorial cases with uses the prghTotalPressure BC. Alternatively can you provide a patch which corrects the problem for your case which we can study? |
|
|
I have checked all tutorials for multiphase solvers and all of them use prghPressure at the outlet, which is different from my case, so I am not sure how I can reporduce my problem from it. I will detail my problem: I am trying to simulate phase change in a nozzle using reactingTwoPhaseEulerFoam using pressure based boundary conditions. I have used prghTotalPressure at the inlet and prghPressure at outlet and pressure based boundary conditions for the velocity field. Rest BC are standard. I have set a total pressure p0 514174 at the inlet and 454700 at the outlet. The p BC's are set to be calculated based in internal field. In this particular case, As p =p_rgh - rho g x At the inlet p = p_rgh as x=0; IF you check the attached file in the note here: you can find in the boundary field 0.001/p INLET { type calculated; value uniform 514174; <----- is the value of total pressure I have given in the problem. } while in the 0.001/p_rgh file we can se that INLET { type prghTotalPressure; U U.liquid; rho rho; psi none; gamma 1; p0 uniform 514174; value nonuniform List<scalar> 24 ( 514173.201842 514173.201842 514173.201842 514173.201842 514173.201842 514173.201842 514173.201841 514173.201841 514173.201841 514173.201841 514173.201841 514173.201841 514173.20184 514173.20184 514173.20184 514173.20184 514173.201839 514173.201839 514173.201839 514173.201839 514173.201838 514173.201838 514173.201965 514173.20699 ) ; } Shouldn't be p =p_rgh? and how can p have a value of total pressure when there is some value of velocity pressure in the inlet face. |
|
|
correction in this first line: I have checked all tutorials for multiphase solvers and all of them use "prghTotalPressure" at the outlet, which is different from my case, so I am not sure how I can reporduce my problem from it. |
|
|
The issue does not relate to the boundary condition prghTotalPressure but the use of pressureInletOutletVelocity for inlet velocity which was not explicitly supported for multiphase. I have now generalised support for derived fixedValue BCs using the assignable() member function which should resolve this problem and potential problems with other derived fixedValue BCs. Resolved by commit 5b4e84c97bf272104f432406b22fc8728d751da2 |
|
|
i think this issue has been resolved, works correctly for 3D cases. |
|
|
Resolved by commit 5b4e84c97bf272104f432406b22fc8728d751da2 |
| Date Modified | Username | Field | Change |
|---|---|---|---|
| 2020-02-19 20:08 | sjohn2 | New Issue | |
| 2020-02-19 20:09 | sjohn2 | File Added: CD_NOZ_3D_rtpef_BNL_291_lam_cse8_TP_oldcase_pWAL_dev_bc_test.zip | |
| 2020-02-20 21:47 | sjohn2 | Note Added: 0011199 | |
| 2020-02-21 12:48 | henry | Note Added: 0011200 | |
| 2020-02-21 14:56 | sjohn2 | File Added: CD_NOZ_3D_rtpef_BNL_291_lam_cse8_TP_oldcase_pWAL_dev_bc_test-2.zip | |
| 2020-02-21 14:56 | sjohn2 | Note Added: 0011201 | |
| 2020-02-21 15:11 | henry | Note Added: 0011202 | |
| 2020-02-21 15:29 | sjohn2 | Note Added: 0011203 | |
| 2020-02-21 15:32 | henry | Note Added: 0011204 | |
| 2020-02-21 15:33 | henry | Note Edited: 0011204 | |
| 2020-02-21 16:25 | sjohn2 | File Added: CD_NOZ_3D_rtpef_BNL_291_lam_cse8_TP_oldcase_pWAL_dev_bc_test-3.zip | |
| 2020-02-21 16:25 | sjohn2 | Note Added: 0011206 | |
| 2020-02-21 16:28 | sjohn2 | Note Added: 0011207 | |
| 2020-02-23 22:24 | henry | Note Added: 0011209 | |
| 2020-02-25 20:21 | sjohn2 | Note Added: 0011211 | |
| 2020-02-25 20:56 | henry | Assigned To | => henry |
| 2020-02-25 20:56 | henry | Status | new => resolved |
| 2020-02-25 20:56 | henry | Resolution | open => fixed |
| 2020-02-25 20:56 | henry | Fixed in Version | => dev |
| 2020-02-25 20:56 | henry | Note Added: 0011212 |
