Porosity:Unable to get desired pressure drop

[sagarcfd]

Hello,
I am solving for head loss from porous region in a square duct using code saturne 4.2. Square duct is of length 10m with cross section of 0.5m * 0.5m i.e. 0.5*0.5*10 (X*Y*Z). It has porous region of length 1 m at middle i.e. from Z=4.5m to Z=5.5m.Pressure drop is obtained from equation given in code saturne user manual, i.e.-
rho*du/dt=-0.5*rho*alpha*|u|u
Where rho is density
u is velocity
Alpha is loss coefficient (per meter)
For steady flow simulation I have used following properties:
Density =1.225 kg/m^3
Viscosity = 1.7894 Pa.s
Reference pressure = 101325 Pa
Turbulence model = k-epsilon scalable two scales model
Head loss coefficient,Alpha=103.082
Inlet velocity=8 m/s
Turbulence - Calculation by turbulence intensity
Intensity=5%
Hydraulic Diameter=0.5 m
Gradient calculation method - Least square method over extended neighbourhood
Velocity-pressure coupling-SIMPLE
No. of iteration=500
Using formula for head loss as stated above I should get pressure drop of 4040.8144 Pa across porous region. But I am getting 2223.17 Pa pressure drop as measured at Points at start (Z=4.5m) and end (Z=5.5m) of porous zone.
Please tell me why I am unable to get desired pressure drop?
.xml File and pictures of mesh are attached below

[Yvan Fournier]

Hello,

How many cells do you have in the head loss region ? If you do not have many cells, using the "improved pressure interpolation in stratified flow" global numerical parameter might help.

Also, if the profile is not flat, measuring the head loss might be tricky (in version 4.3, an automatic computation of the head loss for a volume region was added, making this easier; in version 5.0-alpha, this may be activated using the GUI).

Regards,

Yvan

[sagarcfd]

Hello Sir,
Thank you for your prompt reply.

I have used 36784 elements in porous region and 344608 elements in non porous region. Total elements in whole domain are thus 425316 with 400950 nodes.

I have carried out simulation using "improved pressure interpolation in stratified flow" as per your suggestion. Now I am getting pressure drop of 4083.8 Pa. But as It can be seen in attached figures flow starts swirling near start of porous region so pressure contour on planes at Z=4.5 m and Z=5.5 m (i.e. beginning and end of porous region) are not symmetric. For simple square duct pressure and velocity contours should be symmetrical. Please suggest possible reason for swirling of flow.

Thanks and Regards,
Sagar More

[Yvan Fournier]

Hello,

What type of mesh do you have ? Your initial images seemed to show a hexahedral mesh, but your results here would be expected more of a less symmetric mesh, such as tetrahedra. This might also be a side-effect of the "improved pressure interpolation in stratified flow" option, in which case I'll need to pass this along to colleagues who know this part of the algorithm better than I do.

Regards,

Yvan Fournier

[sagarcfd]

Hello sir,

I have used hexahedral mesh in whole domain. It is symmetric as it can be seen from mesh images which I have attached with my previous reply.

I would like to know if you want some more files (viz. Data,RESU etc.)?

Also please suggest me as a best practice how many nodes I should use for simulating porous region (0.5m*0.5m*1m dimension) if I want to simulate without using "improved interpolation in stratified flow" option? Or Is it mandatory to use that option for porosity simulation?

Thanks and regards,
Sagar More

[Yvan Fournier]

Hello,

The option is no mandatory (to my knowledge), but there is an interpolation error at the first and last layers, so having at least 10 to 20 cells in the porous region would be recommended.

I'll check with colleagues to see if they need your setup (though I can always test it on my side, of the mesh is not tool large).

Regards,

Yvan