View Issue Details
| ID | Project | Category | View Status | Date Submitted | Last Update |
|---|---|---|---|---|---|
| 0003503 | OpenFOAM | Bug | public | 2020-06-03 22:35 | 2020-06-05 11:04 |
| Reporter | SamMallinson | Assigned To | henry | ||
| Priority | normal | Severity | minor | Reproducibility | always |
| Status | closed | Resolution | no change required | ||
| Platform | Linux | OS | Ubuntu and Debian | OS Version | 18.04 and sid |
| Summary | 0003503: reactingParcelFoam with thermophysicalProperties.energy:sensibleEnthalpy crashes in v7, but runs ok in v6 | ||||
| Description | When updating an OpenFOAM case from version 6 to version 7, the run crashed due to issues with the thermophysical properties. We noticed the comment for the commit https://github.com/OpenFOAM/OpenFOAM-dev/commit/f9971f80d72a5318cdc81120a925ab9817b3ec62 mentions: "Changed liquid thermo from sensibleEnthalpy to sensibleInternalEnergy in tutorials. It is generally more convergent and stable to solve for internal energy if the fluid is incompressible or weakly compressible." So, we changed the case to use sensibleInternalEnergy (with requisite modifications to system/fvSolution and fvSchemes) and it ran without issue. We were also able to get the case run in version 7 by modifying OpenFOAM-7/src/thermophysicalModels/specie/equationOfState/icoPolynomial/icoPolynomialI.H, line 98, from "return p/this->rho(p, T);" to "return 0;" (that is, modifying the code to match that in version 6, https://github.com/OpenFOAM/OpenFOAM-6/blob/47517f2ebb1bdbacb8e3ce4b15110cd252953f87/src/thermophysicalModels/specie/equationOfState/icoPolynomial/icoPolynomialI.H#L98), and then recompiling; but that approach is unpalatable. I would have expected the case in version 7 to run with sensibleEnthalpy, as it did in version 6. Have the underlying thermodynamic equations changed? Is there a reference? | ||||
| Steps To Reproduce | For version 6: - download sergeyevShaw_of6.tar, un-tar it, call foam-bash-6 (. ~/pathTo/OpenFoam-6/etc/bashrc) then ./Allrun For version 7, which does not work - using the same case as above, ie sergeyevShaw_of6.tar, call foam-bash-7 (. ~/pathTo/OpenFoam-7/etc/bashrc) then ./Allrun For version 7, which does work - download sergeyevShaw_of7_sIE.tar, un-tar it, call foam-bash-7 (. ~/pathTo/OpenFoam-7/etc/bashrc) then ./Allrun | ||||
| Additional Information | Case based on the paper by Sergeyev and Shaw, http://dx.doi.org/10.1088/0957-0233/17/10/N01: droplets of 34 um diameter and velocity 7 m/s are fired horizontally and their trajectory measured. It would make a nice tutorial example for reactingParcelFoam. | ||||
| Tags | No tags attached. | ||||
|
|
|
|
|
> I would have expected the case in version 7 to run with sensibleEnthalpy, as it did in version 6. Have the underlying thermodynamic equations changed? Is there a reference? The enthalpy contribution from the equation of state is p/rho so version 7 is correct and returning 0 instead as in version 6 is an error. |
|
|
"Changed liquid thermo from sensibleEnthalpy to sensibleInternalEnergy in tutorials. It is generally more convergent and stable to solve for internal energy if the fluid is incompressible or weakly compressible." This is good advice, you should use sensibleInternalEnergy with icoPolynomial and other incompressible equations of state. |
| Date Modified | Username | Field | Change |
|---|---|---|---|
| 2020-06-03 22:35 | SamMallinson | New Issue | |
| 2020-06-03 22:35 | SamMallinson | File Added: sergeyevShaw_of6.tar | |
| 2020-06-03 22:35 | SamMallinson | File Added: sergeyevShaw_of7_sIE.tar | |
| 2020-06-03 23:39 | henry | Note Added: 0011372 | |
| 2020-06-03 23:41 | henry | Note Added: 0011373 | |
| 2020-06-05 11:04 | henry | Assigned To | => henry |
| 2020-06-05 11:04 | henry | Status | new => closed |
| 2020-06-05 11:04 | henry | Resolution | open => no change required |
