[tara behmanesh]

Hello,
I have some questions that are really simple and may seem ridiculous but i am struggling with them.


First the most general one : i know it's common to have velocity at the inlet and pressure at the outlet. Since i should dfine the velocity at the outlet how should i do that ?

Some ideas that i have are:
1)assume that pressure drop in this section is not significant. So put velocity equal to the value of Previous row.

2)due to conservation of mass and incompressiblity of the fluid (water) ,assume that inlet and outlet flow rates should be equal and then Vin*Ain=Vout*Aout and if we assume that outle and inlet areas are the same and the pore distribution in media is homogeneous it can be concluded that Vin=Vout (which my mind kinda refuses to accept but do not have any reason against it )

While i do not have solid reason against 1 and 2 but i think that 3 may be more logical and make more sense.

3)since i have pressure at outlet then i can define Vout as blowusing just darcy formula and neglecting fluid-fluid intraction or /the deffusion term)

Vout= - (Pout-P(at previous row))/dy*k/mu
Where
dy : is vertical distance between nodes
k: is permeability
mu : is dynamic viscosity of the fluid

Additional information
(I'm trying to solve a flow in porous media (a cylinder) in staggered grids using artificial compressibilty method)
Thanks sincerely

[andy_]

For an incompressible flow it is common to specify the velocity at the inlet, zero gradient velocity at exit and then scaled so the outflow exactly matches the inflow, zero gradient on the pressure on all boundaries. This ensures the pressure correction equation has a solution (to within a constant so specify a pressure value somewhere convenient within the solution to prevent the arbitrary pressure level drifting) which it won't if the mass sources don't sum to zero exactly.

There are variations which involve setting combinations of static pressures, total pressures, pressure drops, shear stresses on the walls,... but I would suggest getting the basic approach to work first. Check the mass sources always sum to exactly zero (hence the scaling of the exit velocity) or else the Poisson equation will have no solution and the scheme won't converge.

[tara behmanesh]

Thanks a lot. For the first part i think i get what you said :at the out let the velocity should be the same in each node so there is no gradient and at the same time it should be adjusted in a way that conservation of mass holds true (what comes in goes out) that's ok .
However for pressure i can understand that any gradient on boundaries causes non convergence but for a physical point of view isn't pressure difference what drives the flow in side porous media ? So if pressure along inlet boundary is constant does having parabolic profile at inlet make sense? I mean i used parabolic pressure drop (which i had no idea how it would be generated in experiment!) as an explanation for having parabolic velocity profile .

[andy_]

Originally Posted by tara behmanesh

Thanks a lot. For the first part i think i get what you said :at the out let the velocity should be the same in each node so there is no gradient and at the same time it should be adjusted in a way that conservation of mass holds true (what comes in goes out) that's ok .
However for pressure i can understand that any gradient on boundaries causes non convergence but for a physical point of view isn't pressure difference what drives the flow in side porous media ? So if pressure along inlet boundary is constant does having parabolic profile at inlet make sense? I mean i used parabolic pressure drop (which i had no idea how it would be generated in experiment!) as an explanation for having parabolic velocity profile .

Your code assumes the fluid is incompressible and the assumptions involved mean that what is being called pressure is not the thermodynamic pressure. What is a consistent set of boundary conditions is not straightforward with CFD and it can vary with the assumptions within the code (e.g. incompressible vs compressible fluid) and how the pressure-related quantity is evaluated and even in some cases the details of how roundoff quantities vary from time step to time step. However, CFD codes have been around for 50 odd years and so knowledge about how to use all the various versions is about.

Does your current CFD code include all the physics you need or will you have to add some coding? Does it have a user community?

[FMDenaro]

Originally Posted by tara behmanesh

Hello,
I have some questions that are really simple and may seem ridiculous but i am struggling with them.


First the most general one : i know it's common to have velocity at the inlet and pressure at the outlet. Since i should dfine the velocity at the outlet how should i do that ?

Some ideas that i have are:
1)assume that pressure drop in this section is not significant. So put velocity equal to the value of Previous row.

2)due to conservation of mass and incompressiblity of the fluid (water) ,assume that inlet and outlet flow rates should be equal and then Vin*Ain=Vout*Aout and if we assume that outle and inlet areas are the same and the pore distribution in media is homogeneous it can be concluded that Vin=Vout (which my mind kinda refuses to accept but do not have any reason against it )

While i do not have solid reason against 1 and 2 but i think that 3 may be more logical and make more sense.

3)since i have pressure at outlet then i can define Vout as blowusing just darcy formula and neglecting fluid-fluid intraction or /the deffusion term)

Vout= - (Pout-P(at previous row))/dy*k/mu
Where
dy : is vertical distance between nodes
k: is permeability
mu : is dynamic viscosity of the fluid

Additional information
(I'm trying to solve a flow in porous media (a cylinder) in staggered grids using artificial compressibilty method)
Thanks sincerely

I strongly suggest to do an intermediate step before coding the porous flow problem.


Consider the flow in a channel with a constant velocity profile in inlet, low Reynolds number and let the flow develop towards the parabolic profile in outflow with the zero normal derivative.
You need to understand that the pressure has a mathematical, not a thermodynamic meaning and the BCs. for the pressure must ensure the divergence-free velocity constraint.

[Dr Youssef Hafez]

I agree with Dr. Denaro and Dr. Andy that the pressure has a mathematical, not a thermodynamic meaning. In fact, from a CFD or mathematical prospective the pressure is just a constraint to enforce the incompressibility constraint or the velocity divergence free condition. Therefore it makes less sense that some CFD codes requires specification of some pressure values which may lead to over-constraint of the solution and causes mass imbalance problems.
For that reason there are codes that expresses the pressure using the penalty approach as:
- p/k = (Div. V) ; or p = - K (Div. V)
where K is a penalty parameter that is supposed to have a very large values (ideally infinity) so at such very large values Div (V) =0.0 .
A better formulation is the iterative penalty method which I used in my codes which is:
p (at iteration i+1) = p (at iteration i) - K (Div. V)
In the iterative penalty method smaller values could be taken for k, eg. k maybe 100 to avoid using very large numbers.
When using the pressure penalty approach, no need to solve the continuity equation on the global scale and in fact the pressure is substituted for using the above mentioned equations and the pressure is no longer an unknown which reduces the number of unknown to only the velocities. However, the pressure can be recovered by solving on the element or cell scale using the penalty equation and the obtained values are true within an additive constant. Knowing one value of pressure, the pressure values obtained could be easily scaled.