CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Running, Solving & CFD (
-   -   Venturi injector verification test (

roberto February 26, 2006 20:12

Hello I'm just to trying a

I'm just to trying a verification case, I tried to study a venturi injector for water. This is an existing part, I know the main feature from testing ( inlet pressure, outlet pressure, flow, suction flow).
I generated the mesh with gambit.
I used the turbFoam application finding reasonable velocity fields, but very low pressure fields, (1000 times or more smaller than expected) I
Running the same simulation with Fluent, with the same mesh, boundary condition and viscosity, I found very similar velocity fields but the pressure fields were much more high, matching test values.
some more information:
For openfoam setup I started from turbFoam/cavity case
I never input water density in openfoam (have to be done? how?)
I used gambitToFoam to convert the mesh

anyone have some idea?


gschaider February 27, 2006 04:50

I know, that was not what you'
I know, that was not what you're asking: if you're generating your mesh with gambit it's better to use fluentMeshToFoam to convert the mesh.

The other thing: turbFoam is an incompressible solver. In OF they don't specify a density for those, it's all done with the viscosity (dynamic vs kinematic)

hjasak February 27, 2006 05:07

Hi Bernhard, Any particular
Hi Bernhard,

Any particular reason for preferring the Fluent converter - if there are bugs I should know about, please let me know and I'll have a look. Both converters should be doing their job equally well.


mattijs February 27, 2006 05:55

Hi roberto, check turbFoam
Hi roberto,

check turbFoam for whether it solves for p or p/rho (since incompressible). The source code is in $FOAM_SOLVERS/incompressible/turbFoam. Or check the dimensions on 0/p.

gschaider February 27, 2006 06:04

Of course your right (no bugs)
Of course your right (no bugs). My reasons for recommending the fluent-converter were:

- The fluent-converter preserves boundary-information (wall, symmetry etc) where possible

- Don't know what the gambit-converter does with "internal"-boundaries (the fluent-Converter at least writes faceSets/cellSets) and one can work with that (for instance _fluent_mesh_with_internal_walls)

- if he's comparing with Fluent he can use the same .msh-file he propably imported into Fluent (I think the gambit-converter reads the Neutral-Files). I would prefer that because there are less oportunities to mess things up with just one "version" of the grid lying around (but I tend to mistrust myself -for -good reasons- so this might not apply to others)

roberto February 27, 2006 12:17

Hello and thanks to everybody!
Hello and thanks to everybody!

I checked p dimension, it's [ 0 2 -2 0 0 0 0]
Now I understand the problem, it isn't a pressure!
How can I obtain the pressure?
thanks again

gschaider February 27, 2006 12:36

Roberto: If you multiply it wi
Roberto: If you multiply it with a density it becomes a pressure

roberto February 27, 2006 13:04

Hi Bernhard Great! Now the
Hi Bernhard

Now the pressure results have lot of sense!
(and you can understand my emarrassment for not finding density input...)
Is there a way to convert p field in a pressure field in order to have parafoam rappresentations with pressure?

gschaider February 27, 2006 13:23

@embarassment: there's no need
@embarassment: there's no need. At least you were looking at the numbers (not just the colors).

For the pressure there are two ways:

- the easy way: in paraFoam use the calculator filter to multiply the p-field with a constant (the density would be the best choice ;-) ) and vizualize that

- rewrite the solver to write out an additional field pReal (or similar) that is p*density

roberto February 27, 2006 14:11

Thank you very much for everit
Thank you very much for everithing!
For almost all commercial programs this usefull and quick answers are a dream.

Embarassment was generated by the consciousness that density enter in problem equations, even with uncompressable fluid, so I didn't found phisical sense to results.
Now I know what p means for openfoam and all is very clear and full of sense.
I'm used to solve my mechanical problems by pen and paper, so I don't care too much about colors, anyway results presentation is alwais important.

If someone is interested, after simulation,sampling and testing I will share the results for validation purposes.

gschaider February 27, 2006 14:22

Roberto: one nice place to put
Roberto: one nice place to put your validation case would be: mples

All times are GMT -4. The time now is 09:42.