View Issue Details

IDProjectCategoryView StatusLast Update
0003480OpenFOAMBugpublic2020-11-04 09:47
Reporterzhangxusjtu Assigned Towill  
Status resolvedResolutionfixed 
Product Versiondev 
Summary0003480: Error in a fomula of the lagrangian library at /PhaseChangeModel/LiquidEvaporation/LiquidEvaporation.C
DescriptionAt line 197 to calculate the vapor concentration at surface: const scalar Cs = pSat/(RR*Ts);. Here, `Cs` is supposed to be the surface vapor concentration of component i.

According to Raoult's law, the partial pressure of each component of an ideal mixture of liquids is equal to the vapour pressure of the pure component multiplied by its mole fraction in the mixture. The partial vapor pressure of component i can be calculated with `ps = X[lid]*pSat`, and the corresponding vapor concentration should be `Cs = X[lid] * pSat/(RR*Ts)`.
TagsNo tags attached.



2020-04-16 11:59

manager   ~0011292

Last edited: 2020-04-16 11:59

Just looking at the code, I agree with you. However, the code is not straightforward, and I can't be 100% sure. I need some evidence that the current implementation is wrong and that your proposal is correct. This is a commonly used model; we can't just change it on a hunch. Do you have any evidence?

It seems to me that you could prove the correct-ness of this model in the presence of multiple species by creating two cases that simulate the evaporation of a single drop (potentially in a single cell). The drop in the first case would be 100% water. The second would be 50% water and 50% some other species with identical properties to water. If the results were the same, then the handling of Raoult's law would be proven consistent. Can you construct such a test?


2020-04-16 12:51

reporter   ~0011294

I agree with you, and the proposed test case is convincing. I will try it later.


2020-11-04 02:36

reporter   ~0011658

I have carried out a test with mixed water parcel in a box, with 50% H2O and 50% anotherH2O (with the same liquid properties). The results are different though, with different particle diameter at time=0.5. This indicates that they are evaporating with different rates. I am working with OpenFOAM-6. The orig case was from the $FOAM_TUTORIALS.
waterParcelInBox.tar (1,699,840 bytes)


2020-11-04 09:47

manager   ~0011661

Thanks for confirming it.

More importantly than the evaporation rates being different, if we apply your proposed fix then the evaporation rates become the same. See the attached graphs for before and after.

This has been fixed in dev and version 8 by the following commits.
beforeAndAfter.png (47,940 bytes)   
beforeAndAfter.png (47,940 bytes)   

Issue History

Date Modified Username Field Change
2020-04-14 13:14 zhangxusjtu New Issue
2020-04-16 11:59 will Note Added: 0011292
2020-04-16 11:59 will Note Edited: 0011292
2020-04-16 12:51 zhangxusjtu Note Added: 0011294
2020-11-04 02:36 zhangxusjtu File Added: waterParcelInBox.tar
2020-11-04 02:36 zhangxusjtu Note Added: 0011658
2020-11-04 09:47 will File Added: beforeAndAfter.png
2020-11-04 09:47 will Note Added: 0011661
2020-11-04 09:47 will Assigned To => will
2020-11-04 09:47 will Status new => resolved
2020-11-04 09:47 will Resolution open => fixed
2020-11-04 09:47 will Fixed in Version => 8