Modeling interface of fluid and porous, not with default setting
 

Dear CFX experts,
I am trying to model a blood flow inside the artery and also its wall.
The model looks like this:
http://imageshack.com/a/img835/8348/nliz.png

As seen in the image, the boundary between the fluid domain and the tissue in reality only lets the normal component of the velocity to enter.
From my simulation with fluid domain for the lumen (inside artery) and porous tissue (inside the wall) I get only tangent velocity inside the wall, which exists only very close to the boundary (probably due to very low permeability).

http://imageshack.com/a/img836/926/w8j2.png

My question is whether there is a better way to model it and get the correct results in the interface?
- If I want to assume it as a perforated plate, how do I set the boundary?
-If I go with directional loss for the porous, how I set the streamwise direction components equal to normals on each cells?

I appreciate your valuable hints!

You could use a momentum source to set the tangential velocity component to zero. Then it is forced to only go in the normal direction.

Dear Glenn,
Thanks for your prompt reply.

Could you please explain it more. The way I understand it, I define the tissue domain as a fluid domain, then I define a subdomain there and define the momentum source. But in this case this applies to the entire porous domain (here the tissue), not only to the interface.

And regarding suppressing the tangential velocity, how do I do that? with anisotropic model and suppressing the transverse direction with lower permeability?

You define a source term which sets the value to a specific value by setting the source term to -C(v-v0) where C is a large number, v is the equation it is being applied to (eg u for U velocity) and v0 is the value you want v to be at that location. You also set the source term coefficient to -C.

So you find the tangential direction and set that to v0=0.

See the CFX documentation for more information on momentum source terms.

Thanks again, Now I can see I should go in the direction of general momentum source term and not the former ones (Isotropic loss,...). It is a great step forward for me.

I checked the theory part. I am still wandering whether
1- this approach will suppress the tangential velocity for the entire domain and not only on the interface? is it physically correct?

2- in real artery I do not know the tangential direction. The artery is tortuous. Can I use "Normal" variable to find the direction normal to each cell? Do you recommend better approach?

The momentum source acts on the region you define it to act on. So I would connect the fluid region and the porous region with an interface, then apply it to the interface. Then it will act only at the interface.

Yes, hopefully you can work out some maths to get the normal direction and apply the source term from there.

Dear Glenn,
Thanks for your invaluable comments which is of great help as always.
The method you are offering is the ultimate goal and I will dig into cfx data to make it happen.
But applying the source on an interface, I could not make it feasible in CFX. For an interface only the continuity source is available, and momentum source is only available for a domain or sub domain. Have you ever succeeded applying it to an interface boundary?

I am sorry, I am trying my best to spam you as less as possible, and write here after I really give up on something. I hope it is not a trivial problem which I am facing.

I found what I claimed here, although it was an old PPT file of ANSYS.
http://imageshack.com/a/img835/1861/ttof.png

I hope it is still possible to do it some how.

OK, I was not aware of that.

In that case I would consider defining a thin cylinder adjacent to the wall and put the momentum source on that as a volume source.

Glenn, thanks for the reply.

Then I will go with this approach. Although the cell layer is only 1 micrometer, compared to the tissue thickness of 5oo microns. Since it (what is happening in this sub domain) is not really interfering in the flow simulation, I will make it a little bit bigger and apply the momentum source.

I could not find any tutorial applying the general momentum source, and I do not exactly know what I should put as the setting. I will make myself busy for a while, and I will post it here if I do not reach a reasonable solution.

In a realistic case the artery is not a uni-axial cylinder and finding the momentum source direction normal to it will be the next challenge.

Thanks a lot anyway, for what I have reached so far was not possible without your help, Glenn.

I unfortunately had no success in applying the general momentum source in my model. The definition is clear is theory references, but when it comes to application, there is no tutorial showing an example.

I have these questions, and highly appreciate any help:

http://imageshack.com/a/img842/8829/co9e.png

1- Assuming I want to block the velocity in Z direction (just to test the effect), what should be the components in all three cartesian component blocks? Please give me the exact value, whatever you feel like as an example.

2- Since this domain is a porous domain, how the known value of permeability should be applied? Do I need to add also the isotropic source separately ( I really doubt it)? Or the component of momentum can take care of that? (viscosity / permeability *Velocity).

3-For a case which is not in any of X, Y, and Z direction, How should the components defined? Normal X,... are only defined on 2D surfaces and boundaries.

Thanks a lot.

Just a quick rewind - why do you think the flow is perpendicular to the wall anyway? And why do you think you need to constrain it to be perpendicular?

To my way of thinking, if stuff is diffusing through the wall there is no reason why it cannot diffuse along the wall versus across it. There is no physical justification to use anisotropic porous regions or momentum sources as the material is isotropic in reality (please correct me if I am wrong here). The thing which makes the flow predominantly perpendicular to the wall is that the pressure gradient generated is tangent to the wall, so this pushes the flow in a perpendicular direction. You do not need to have any constraints in the flow to do this, it will do this naturally.

So why not make use of this? Why not just use a homogeneous porous or momentum sink region and the flow will naturally go perpendicular to the wall.

Dear Glenn, Thanks for your reply.

The problem is, the cell layer which I have drown in the first post, acts as a barrier, not letting the flow to enter the porous region with any tangential component. So the best way to model it would be to kill only the tangential component on the interface between flow and porous domain. That is why, I am trying to define a very thin porous region (as the momentum source is not allowed on the interface) to model it. The flow from the lumen passes the leaky junctions between the cells.

When I model it with a normal interface between fluid and porous domain, with a BC of conservation of momentum and UDS, the flow near the interface in the porous domain is parallel to the interface (see the first post and image), and the UDS is not convected perpendicular to domain at all. Is it due to very low permeability (1.43e-18)? Also the flow inside the fluid domain becomes completely plug flow without any parabolic pattern, no effect of tangential No slip is observed there.

I agree with you that the pressure gradient can take care of it, but the problem is the BC. When it is conservation of Mom and UDS, the tangential component is so dominant that affects the normal flow. If it is no slip, then there is no flow from fluid region to the tissue. Please consider that the physical flow inside the tissue is measured to be around 2e-8 m/s.

I am open to any suggestion that makes the flow look more physical, I am completely exhausted trying a lot of approaches, all of which were in vain.

If you were in my shoes, and wanted to model the drug transport in the tissue (porous domain), and wanted to see both the effects of diffusion and CONVECTION, what would be your approach? I only see the diffusion, without any convection since the flow inside the tissue is not correct. The peclet number is: L (0.0005m)*V (1e-8m/s) / D (~4e-12) = O(1). So convection is as important as diffusion in the tissue, right?

Thanks again for your invaluable time and comments.

You could use a momentum source to just set the axial flow to zero. This would allow radial and rotational flow, but unless there is something to generate rotational flow there won't be much of that. This might be close enough for you.

Something sounds very wrong with your simulation you describe. I cannot see how the fluid domain has plug flow. Can you post an image of your domain and your CCL?

Dear Glenn,
Thanks for the reply. The very simplified model of artery without stent is just a cylinder with shell.
http://imageshack.com/a/img835/5578/4tyi.png

And the result for the velocity is:
http://imageshack.com/a/img841/5048/zhfk.png
and profile:

http://imageshack.com/a/img835/9725/vhlo.png

The boundary condition is default for the interface (Conservation of mass and momentum). Making the interface Noslip solves the parabolic profile issue, but then nothing passes the interface except with diffusion.

Could you please let me know what you mean with the CCL?
I would provide any detail which could be of help for you.

The CCL is the text which describes the simulation at the top of the output file. It is also a stand-alone text file. You can export this from CFX-Pre.

You should not need an interface for this, it should be able to be modelled as a single domain with the porous region as a sub-domain. If you do this does it change anything?

Very good idea, but any way to make the subdomain, you need to define that part as a separate material in mesh, and then the wall will be generated by default. Then I encounter the same problem, but let me try it first and come back to you.

Here you go with CCL:

LIBRARY:

ADDITIONAL VARIABLE: Drug
Option = Definition
Tensor Type = SCALAR
Units = [kg m^-3 ]
Variable Type = Volumetric
END

MATERIAL: Blood
Material Group = User
Option = Pure Substance
Thermodynamic State = Liquid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 1050 [kg m^-3]
Molar Mass = 18.02 [kg kmol^-1]
Option = Value
END
DYNAMIC VISCOSITY:
Option = Non Newtonian Model
NON NEWTONIAN VISCOSITY MODEL:
High Shear Viscosity = 0.25 [Pa s]
Low Shear Viscosity = 0.0035 [Pa s]
Option = Bird Carreau
Power Law Index = 0.25
Time Constant = 25 [s]
END
END
END
END

MATERIAL: plasma
Material Description = Water (liquid)
Material Group = User
Option = Pure Substance
Thermodynamic State = Liquid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 1000 [kg m^-3]
Molar Mass = 18.02 [kg kmol^-1]
Option = Value
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 0.001 [kg m^-1 s^-1]
Option = Value
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 1.0 [m^-1]
Option = Value
END
SCATTERING COEFFICIENT:
Option = Value
Scattering Coefficient = 0.0 [m^-1]
END
REFRACTIVE INDEX:
Option = Value
Refractive Index = 1.0 [m m^-1]
END
END
END
END
FLOW: Flow Analysis 1
SOLUTION UNITS:
Angle Units = [rad]
Length Units = [m]
Mass Units = [kg]
Solid Angle Units = [sr]
Temperature Units = [K]
Time Units = [s]
END
ANALYSIS TYPE:
Option = Steady State
EXTERNAL SOLVER COUPLING:
Option = None
END
END
DOMAIN: lumen
Coord Frame = Coord 0
Domain Type = Fluid
Location = CREATED_MATERIAL_5
BOUNDARY: inlet_lumen
Boundary Type = INLET
Location = LUMEN_INLET
BOUNDARY CONDITIONS:
ADDITIONAL VARIABLE: Drug
Additional Variable Value = 1 [kg m^-3]
Option = Value
END
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Mass Flow Rate = 0.0009975 [kg s^-1]
Option = Mass Flow Rate
END
END
END
BOUNDARY: lumen_out
Boundary Type = OUTLET
Location = LUMEN_OUTLET
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Average Static Pressure
Pressure Profile Blend = 0.05
Relative Pressure = 70 [mm Hg]
END
PRESSURE AVERAGING:
Option = Average Over Whole Outlet
END
END
END
BOUNDARY: luminal_interface Side 1
Boundary Type = INTERFACE
Location = LUMINAL
BOUNDARY CONDITIONS:
ADDITIONAL VARIABLE: Drug
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 1 [atm]
END
END
FLUID DEFINITION: Fluid 1
Material = Blood
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
ADDITIONAL VARIABLE: Drug
Kinematic Diffusivity = 3.89e-11 [m^2 s^-1]
Option = Transport Equation
END
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = Laminar
END
END
END
DOMAIN: tissue
Coord Frame = Coord 0
Domain Type = Fluid
Location = TISSUE_MATERIAL
BOUNDARY: in_tissue
Boundary Type = INLET
Location = TISSUE_IN
BOUNDARY CONDITIONS:
ADDITIONAL VARIABLE: Drug
Additional Variable Value = 0 [kg m^-3]
Option = Value
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Normal Speed = 0 [m s^-1]
Option = Normal Speed
END
END
END
BOUNDARY: luminal_interface Side 2
Boundary Type = INTERFACE
Location = LUMINAL_INTF_TISSUE
BOUNDARY CONDITIONS:
ADDITIONAL VARIABLE: Drug
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: out_tissue
Boundary Type = OUTLET
Location = TISSUE_OUT
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Normal Speed = 0 [m s^-1]
Option = Normal Speed
END
END
END
BOUNDARY: perivascular
Boundary Type = OUTLET
Location = PERIVASCULAR
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Average Static Pressure
Pressure Profile Blend = 0.05
Relative Pressure = 17.5 [mm Hg]
END
PRESSURE AVERAGING:
Option = Average Over Whole Outlet
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 1 [atm]
END
END
FLUID DEFINITION: Fluid 1
Material = plasma
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
ADDITIONAL VARIABLE: Drug
Kinematic Diffusivity = 3.65e-12 [m^2 s^-1]
Option = Transport Equation
END
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = Laminar
END
END
SUBDOMAIN: Subdomain 1
Coord Frame = Coord 0
Location = TISSUE_MATERIAL
SOURCES:
MOMENTUM SOURCE:
LOSS MODEL:
Option = Isotropic Loss
ISOTROPIC LOSS MODEL:
Option = Permeability and Loss Coefficient
Permeability = 1.43e-18 [m^2]
END
END
END
END
END
END
DOMAIN INTERFACE: luminal_interface
Boundary List1 = luminal_interface Side 1
Boundary List2 = luminal_interface Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = None
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
PITCH CHANGE:
Option = None
END
END
MESH CONNECTION:
Option = GGI
END
END
OUTPUT CONTROL:
RESULTS:
File Compression Level = Default
Option = Standard
END
END
SOLVER CONTROL:
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Length Scale Option = Conservative
Maximum Number of Iterations = 25000
Minimum Number of Iterations = 1
Timescale Control = Auto Timescale
Timescale Factor = 1
END
CONVERGENCE CRITERIA:
Residual Target = 0.00000001
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
EQUATION CLASS: av
CONVERGENCE CONTROL:
Length Scale Option = Conservative
Timescale Control = Auto Timescale
Timescale Factor = 1
END
END
END
EXPERT PARAMETERS:
solve fluids = t
solve scalar = t
END
END
COMMAND FILE:
Version = 14.0
END
SIMULATION CONTROL:
EXECUTION CONTROL:
EXECUTABLE SELECTION:
Double Precision = No
END
INTERPOLATOR STEP CONTROL:
Runtime Priority = Standard
END
PARTITIONER STEP CONTROL:
Multidomain Option = Independent Partitioning
Runtime Priority = Standard
PARTITIONING TYPE:
MeTiS Type = k-way
Option = MeTiS
Partition Size Rule = Automatic
END
END
RUN DEFINITION:
Run Mode = Full
Solver Input File = Z:/Cylinder_test/No stent/New \
Folder/no_stent_peri_out_mass_NOflux_drug_inlet_conservat ive_intf_.def
END
SOLVER STEP CONTROL:
Runtime Priority = Standard
PARALLEL ENVIRONMENT:
Start Method = Serial
END
END
END
END

You do not seem to have a loss coefficient in your porous model. Is it missing something? A zero loss porous region would explain what you are seeing.

We could have two different loss coefficients as far as I know:
-Viscous loss, which is first order (similar to darcy law), equal to Viscosity* velocity/Permeability (miu*V/K).
-Nonlinear term for the Inertia loss, soething I have ignored (similar to my reference paper) : Coeff. * Density/2 *|Velocity| * Velocity_Vector

I have ignored the second, as it is in this open source paper that I have referenced, you can see the whole models and boundary conditions there if needed:
http://www.plosone.org/article/info%...l.pone.0008105