# Modeling interface of fluid and porous, not with default setting

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 May 5, 2014, 05:15 Modeling interface of fluid and porous, not with default setting #1 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 Dear CFX experts, I am trying to model a blood flow inside the artery and also its wall. The model looks like this: 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). 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!

 May 5, 2014, 06:48 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 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.

May 5, 2014, 07:14
#3
Member

Ftab
Join Date: Sep 2011
Posts: 63
Rep Power: 7
Quote:
 Originally Posted by ghorrocks 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?

 May 5, 2014, 07:33 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 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.

 May 5, 2014, 08:36 #5 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 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?

 May 5, 2014, 19:06 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 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.

 May 6, 2014, 04:33 #7 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 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.

 May 6, 2014, 09:20 #8 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 I found what I claimed here, although it was an old PPT file of ANSYS. I hope it is still possible to do it some how. Last edited by ftab; May 6, 2014 at 10:56.

 May 6, 2014, 19:57 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 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.

 May 7, 2014, 08:10 #10 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 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.

 May 14, 2014, 11:00 #11 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 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: 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.

 May 14, 2014, 18:28 #12 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 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.

 May 15, 2014, 05:24 #13 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 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.

 May 15, 2014, 06:19 #14 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 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?

 May 15, 2014, 15:11 #15 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 Dear Glenn, Thanks for the reply. The very simplified model of artery without stent is just a cylinder with shell. And the result for the velocity is: and profile: 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.

 May 15, 2014, 15:15 #16 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 Could you please let me know what you mean with the CCL? I would provide any detail which could be of help for you.

 May 15, 2014, 19:00 #17 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 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?

 May 16, 2014, 05:08 #18 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 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

 May 16, 2014, 06:35 #19 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,832 Rep Power: 100 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.

 May 16, 2014, 08:30 #20 Member   Ftab Join Date: Sep 2011 Posts: 63 Rep Power: 7 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Mohsen Nazari FLUENT 4 July 23, 2016 05:10 Hitch8 CFX 19 April 20, 2015 06:24 Anna Tian CFX 1 June 16, 2013 06:28 siw FLUENT 0 December 22, 2011 08:39 rajesh kumar FLUENT 5 October 22, 2004 11:10

All times are GMT -4. The time now is 20:33.

 Contact Us - CFD Online - Top