|
[Sponsors] |
how to specify wall contact angle for compressibleInterFoam? |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
Senior Member
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 334
Rep Power: 18 ![]() |
Hi,
I used to specify contact angle the following way: channel { type constantAlphaContactAngle; theta0 90; uTheta 0; thetaA 90; thetaR 90; value uniform 0; } but now in OpenFOAM-1.7.x, I am getting the following error: Reading field alpha1 --> FOAM FATAL IO ERROR: keyword limit is undefined in dictionary "/home/phsieh/OpenFOAM/phsieh-1.7.x/run/transducerInterfaceA/0/alpha1::boundaryField::channel" file: /home/phsieh/OpenFOAM/phsieh-1.7.x/run/transducerInterfaceA/0/alpha1::boundaryField::channel from line 183257 to line 183259. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 395. FOAM exiting ------------------- what does the limit do? It looks like the limit keyword is looking for : alpha zeroGradient gradient none when to choose which one? Thanks! Pei |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 323
Rep Power: 18 ![]() |
Hi
It seems you must use dynamicAlphaContactAngle. Best regards Ata |
|
![]() |
![]() |
![]() |
![]() |
#3 |
Senior Member
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 334
Rep Power: 18 ![]() |
Hi, ata,
Thanks for the reply! I found the answer in alphaContactAngleFvPatchScalarField.H: Description Abstract base class for alphaContactAngle boundary conditions. Derived classes must implement the theta() fuction which returns the wall contact angle field. The essential entry "limit" controls the gradient of alpha1 on the wall: limit none; // Calculate the gradient from the contact-angle without // limiter limit gradient; // Limit the wall-gradient such that alpha1 remains // bounded on the wall limit alpha; // Bound the calculated alpha1 on the wall limit zeroGradient; // Set the gradient of alpha1 to 0 on the wall // i.e. reproduce previous behaviour Note that if any of the first three options are used the boundary condition on p_rgh must set to guarantee that the flux is corrected to be zero at the wall e.g. walls { type fixedFluxPressure; adjoint no; } If "limit zeroGradient;" is used the pressure BCs can be left as before. SourceFiles alphaContactAngleFvPatchScalarField.C ---------------------- Still not quite clear when to choose which one, but, for now, I added limit none; and still using constantAlphaContactAngle and the case is running. Will check if the results are reasonable. Pei |
|
![]() |
![]() |
![]() |
![]() |
#4 |
Senior Member
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 323
Rep Power: 18 ![]() |
Hi Pei
Thanks for yur explanation Good luck Best regards Ata |
|
![]() |
![]() |
![]() |
![]() |
#5 | |
Member
Join Date: May 2012
Posts: 55
Rep Power: 15 ![]() |
Quote:
Hello Pei, thank your explanation! Could you please explain, why the flux has to be zero at walls, if the limiter for alpha1 is non zeroGradient? I've tested two different pressure bc for walls. The case is the standard capillary rise tutorial. It seems that the free surface is more oscillating with zeroGradient as pressure bc at walls as with fixedFluxPressure. I've plotted the surface elevation over time: Pressure BC zeroGradient at walls: capillaryRise_zero.png Pressure BC fixedFluxPressure at wall: capillary_rise.png EDIT: I've just read that the pressure gradient is adjusts in a way that the flux on the boundary is that specified by the velocity boundary condition. (https://github.com/OpenFOAM/OpenFOAM...hScalarField.H) So it does not have to be zero. Last edited by styleworker; December 19, 2012 at 10:41. |
||
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
InterFoam contact angle | JoaoMiranda | OpenFOAM Running, Solving & CFD | 7 | October 20, 2016 06:27 |
solved: contact angle correction in interFoam | rcastilla | OpenFOAM Bugs | 24 | March 2, 2016 13:43 |
[Commercial meshers] tmerge utility creates unwanted interface/walls comes in the final mesh | Shoonya | OpenFOAM Meshing & Mesh Conversion | 11 | January 20, 2012 06:23 |
[Netgen] Import netgen mesh to OpenFOAM | hsieh | OpenFOAM Meshing & Mesh Conversion | 32 | September 13, 2011 05:50 |
Contact angle UDF | shephali shrimali | FLUENT | 0 | May 10, 2007 07:52 |