CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Modeling of water infiltration into a tank containing a permeable soil (http://www.cfd-online.com/Forums/cfx/92383-modeling-water-infiltration-into-tank-containing-permeable-soil.html)

idir September 13, 2011 04:32

Modeling of water infiltration into a tank containing a permeable soil
 
5 Attachment(s)
Hello all
I need to model the infiltration of water into a tank containing a permeable soil during a time t.
For this I referred to tutorials (Chapter*9:*Free Surface Flow Over a Bump) and (Chapter*12:*Flow in a Catalytic Converter) to do the modeling (see attachment 1 to 10 ):

*Analysis type : Transient.

*2 domains:
1-->Water_and_Air:(as in tuto9:free surface flow)
2-->Soil:(Porous domain as in tuto 12)

but the results obtained are not normal (incorect) (see attachment 11to 14) .
Please send your views and advice about the boundary conditions and Domains so on.
Thank you in advance.

idir September 13, 2011 04:34

5 Attachment(s)
following of the attachment

idir September 13, 2011 04:37

4 Attachment(s)
and the results of this simulation

ghorrocks September 13, 2011 08:15

What is incorrect about the results?

idir September 13, 2011 09:14

5 Attachment(s)
Hi

The problemes are:

1- the water level above land does not decrease over time

2- and when I change the properties of the soil making it more permeable (volume porosity and permeability of 0.9 to 0.2) I find very different results (see photos1 to 5) and her also the water level does not decrease

ghorrocks September 13, 2011 19:22

1 - How are your imbalances? If the Volume fraction variable has a small imbalance then it is being conserved and the top surface should be moving properly. If not then you need to converge tighter.

2 - You have a fluid region above an air region which you suddenly release. In the absence of the porous region this would result in a chaotic mixing and splashing behaviour - this looks very similar to what you are getting. Are you sure your porousity is high enough to get the effects you are looking for?

Also as you do not have a sharply defined free surface, have you turned on the free surface model? Are your time steps fine enough to resolve the motion? Do you have the correct volume fraction differencing scheme (compressive is the one you want here)?

idir September 14, 2011 06:03

Thank you for your answer

Quote:

Originally Posted by ghorrocks (Post 324019)
1 - How are your imbalances? If the Volume fraction variable has a small imbalance then it is being conserved and the top surface should be moving properly. If not then you need to converge tighter.

I do not understand what you mean by "the volume fraction imbalance variable"

But In this simulation i set the initialization of:
Water domain: Water VolumFraction = 1.0 /AirVolumFraction = 0.0
and
SoilPorous domain: Water VFraction = 0.0 / AirVFraction= 1.0

and I do not know if it's good or not?




Quote:

Originally Posted by ghorrocks (Post 324019)
Also as you do not have a sharply defined free surface, have you turned on the free surface model? Are your time steps fine enough to resolve the motion? Do you have the correct volume fraction differencing scheme (compressive is the one you want here)?

about Free Surace model it was turned off, and now I turned it on and I start the new calculation, and I will give you the results tonight.
Thank you in advance ghorrocks.

idir September 16, 2011 06:07

Now it's ok it works, you have just to turn on free surface option in Solver
thank you:p

ghorrocks September 16, 2011 06:40

Quote:

I do not understand what you mean by "the volume fraction imbalance variable"
Check out the end of the output file. It lists the variable imbalances and will have one for volume fraction. Also the solver manager will have a graph for imbalances and one of the lines will be volume fraction. You can also set convergence criterion on imbalances.

Quote:

I do not know if it's good or not?
If that is the initial condition you want then it sounds good to me.

Quote:

you have just to turn on free surface option in Solver
For a free surface problem that sounds pretty obvious to me.


All times are GMT -4. The time now is 01:57.