[FGH]

On the dam example (http://www.openfoam.org/docs/user/damBreak.php), I run :

1. blockMesh
2. cp 0/alpha.water.org 0/alpha.water
3. setField
4. paraFoam

I can not see alpha in paraview (the only variable that is avaliable is U) : I can not get figure 2.21 from http://www.openfoam.org/docs/user/damBreak.php. I run Ubuntu 14.04 + OpenFOAM-2.3.1 (compiled from source)



I guess this is a bug



FGH

[wyldckat]

Quick answer: We are not associated to the NSA, therefore we're not able to see what you're doing in your computer

Anyway, try following these instructions: http://openfoamwiki.net/index.php/Ho...iphase_results

[meshmaster]

I couldn't see the alpha.water values either in the setup even though I had the cell array value checked for alpha.water. After I solved the simulation with interFoam I did get the results shown in the rest of the tutorial. I think it might be a bug, I am using OpenFOAM 3.0.1

[CFDMagnus]

Digging this up from two years ago, now using OpenFOAM 6.
It's been bugging me for a while and what works for me is:

After executing setFields, there's two alpha.water files:

alpha.water (the correct one, verify it by editing it, there should be a long list of 1&0s), if so setField worked correctly

alpha.water-orig (or similar) this is the original alpha.water setup file (there should be boundary conditions for your patches).

i used to rename them (or setFields does that, i don't remember) but turns out that's not enough, as the header stil says alpha.water

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

move it to a different directory and paraview should display everything correctly.
I'm curious if it's only a Paraview thing and solvers read in the correct file.

[wyldckat]

Quick question @CFDMagnus: I'm a bit confused by your description, because I haven't managed to figure out what was the problem exactly...

Any chance you can describe the steps you take that lead to the problem?

[CFDMagnus]

The problem is for 2 or more phase problems that the setFields seems to have no effect. Paraview won't show the which internal cells are water/air. It will only show the initial conditions, let's say inlet is displayed with water but walls, atmosphere etc. only air.

For a two phase problem i usually want the domain to be partly filled with water at t=0. I will execute setfields, which overrides alpha.water.

The tutorials (and many online tut videos(shout out to Jozsef Nagy) suggest to keep the original alpha.water file under a different name before executing setFields.

Every once in a while, paraview will display the initial alpha.water, instead of the desired, after setfields was excecuted. I don't think that is an OpenFOAM problem but related to Paraview. I GUESS that is because paraview checks the headings of the files, which still contains the title alpha.water and gets confused, which one to display.

It's not much of an issue but really annoying. Simply moving the originial alpha.water to a different location solves the problem.


Hope this was more clear this time

[wyldckat]

Quick answer: Mmm... ooooh! I didn't know this would happen...

So if I understood you correctly - and I'm using OpenFOAM 6 here too - the problem is because the "alpha.water.orig" field is not shown in the list of fields to be rendered, neither with ParaView's internal reader nor OpenFOAM's reader for ParaView...

At least regarding OpenFOAM 6, a feature was added in OpenFOAM to support automatic loading of the ".orig" fields if the actual fields don't exist yet. For example, if only "alpha.water" field doesn't exist yet, then it loads the field "alpha.water.orig" automatically as an alternative. This is why setFields is able to do it so without us having to copy the field as in the past.

So, yes, you'll have to either copy the file out of the folder or have it in the folder with another name. The "object" entry within the file isn't always read and it's there mostly for the user to know the last name it was written as...


As for the internal reader in ParaView, I'm not sure why exactly it ignores both the "object" entry and the file name itself... at least in ParaView 5.4...

[JVNR]

Originally Posted by CFDMagnus

Digging this up from two years ago, now using OpenFOAM 6.
It's been bugging me for a while and what works for me is:

After executing setFields, there's two alpha.water files:

alpha.water (the correct one, verify it by editing it, there should be a long list of 1&0s), if so setField worked correctly

alpha.water-orig (or similar) this is the original alpha.water setup file (there should be boundary conditions for your patches).

i used to rename them (or setFields does that, i don't remember) but turns out that's not enough, as the header stil says alpha.water

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

move it to a different directory and paraview should display everything correctly.
I'm curious if it's only a Paraview thing and solvers read in the correct file.

JUST COMMING HERE TO SAY THANK YOU. I'VE WASTED 2 HOURS OF MY TIME TRYING TO FIX THIS.

From now on I'll stick to having 0.orig and just copying the whole directory