Modeling interface of fluid and porous, not with default setting

ghorrocks · May 17, 2014, 06:00

Something is a bit weird then. Your permeability is tiny, so your viscous loss should be very large. This should result in little axial flow and a small radial flow driven by the pressure gradient.

ftab · May 17, 2014, 06:50

It is indeed weird. I absolutely get no radial flow, and flow is completely parallel to the interface.

The idea of defining one zone with a subdomain would be troublesome as well, as the flow iside lumen is non-newtonian blood, while in porous domain I have plasma. Also to define the subdomain, I need a seperate material in tissue, which makes a boundary interface and there my problem initiates. I cannot apply the proper BC.

ghorrocks · May 17, 2014, 07:02

So I suggest you can either:
* Spend time (probably lots of it) trying to work out why this being weird. I suspect you have already spent lots of time on this so I guessing this is unlikely to be productive.
* Give up on the approach you are using and try something different. Maybe add the porous flow inertial loss factor. Maybe try a completely different porous flow model.

ftab · May 17, 2014, 09:19

Thanks Glenn for your time.
As you are correctly mentioning, I have spent so much time to figure it out and getting feedback from an expert like you reassures me that I am not doing something stupid in the process.

I will keep on playing with the parameters to reach to physically sound results.

Since I might encounter the following issues again, could you please briefly answer question 1 and 3 of Post #11? I repeat them here.

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. (from the units, I am confused what to put there, only the momentum term or the whole -C**u-u0)?. Please write the simplest example you can make, and I will follow on that, just kill the tangential 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.

With my best regards and appreciating your invaluable time,
Ftab

ghorrocks · May 18, 2014, 06:45

Blocking the z direction is easy - just use the momentum course you describe with u0=0 for the direction. I would let x and y remain unrestrained so the radial flow works. Note this will allow flow in the theta direction, but hopefully this is small enough to be OK.

Here is two ideas to get the radial direction in a solid domain:
* Make a function of xyz location. If the shape is simple you can do it analytically. If it is complex then do it on a solid modelling package and generate a 3D interpolation file (one file for each of the three directions to define the vector).
* Do a simulation with a diffusion AV where you set the inside to a value of 0 and and the outside to a value of 1. The AV will then diffused between the inside and the outside. Take the grad of the AV and hey presto you have a vector field which is normal to the surface through the solid domain.

ftab · May 19, 2014, 10:48

Dear Glenn,
Thanks for the reply and your smart idea how to calculate the vector field.

Just to clarify for me and make sure that I got the point, I quickly summarize here and ask for your confirmation.

1- to let x and y remain unrestrained, we put zero as the source term. But for the momentum source term in Z direction to set u0=0, what do we put? Do I need to define an expression equal to -1e-5 *(Z-velocity-u0)? My Naive question in the former post was also this. To set momentum source, what do we explicitely put in the table in CFX? calculated value containing the Coef? or a constant? Sorry to ask a very trivial question.

2-Thanks for this magic solution using AV. What you mean with diffusion AV is simply defining an AV (Volumetric, right?). and in the fluid domain, define it as an algebraic variable (definitely not solving transport equation or diffusion trans. Eq., right?). To define it I simply use an expression with "inside" CEL function to let the tissue side become one, and the lumen 0. And then, to define the gradient, I define a second AV as a vector, and define its x-component as =first_AV.Gradient X for instance. Is this approach the one you meant? Sorry that I am not so professional and quick to catch your brilliant idea.

ghorrocks · May 19, 2014, 18:35

1) So the source terms would be:
X = 0
Y = 0
Z = -C*(Z-z0)

Then set z0=0 [m/s] and C=1e5 [kg m-3 s-1] (NOT 1e-5!). You might also need a source term coefficient of -C.

2) The AV can be any form, volumetric is fine. No, it is not an algebraic AV. You want a diffusion transport eqn. To set the 0 and 1 thing you have a few options - The best (if it works) is to use the interface conditions on the inside and outside to set the AV to defined values as 0 and 1. If it does not like that then use a source term in the fluid and outside regions to lock it to 0 and 1.

ftab · May 20, 2014, 06:58

Dear Glenn,
I cannot thank you enough on this. I will try to apply your smart ideas and hopefully will be back with good news.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
modeling the fluid flow in porous media by Fluent	Mohsen Nazari	FLUENT	5	April 26, 2019 04:45
Radiation at interface between fluid and porous domain	Hitch8	CFX	19	April 20, 2015 06:24
Question about heat transfer coefficient setting for CFX	Anna Tian	CFX	1	June 16, 2013 06:28
Interface setup for fluid & porous zones	siw	FLUENT	0	December 22, 2011 07:39
interface between porous and fluid	rajesh kumar	FLUENT	5	October 22, 2004 11:10

May 17, 2014, 06:00		#21
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,716 Rep Power: 143	Something is a bit weird then. Your permeability is tiny, so your viscous loss should be very large. This should result in little axial flow and a small radial flow driven by the pressure gradient.

May 17, 2014, 06:50		#22
ftab Member Ftab Join Date: Sep 2011 Posts: 87 Rep Power: 14	It is indeed weird. I absolutely get no radial flow, and flow is completely parallel to the interface. The idea of defining one zone with a subdomain would be troublesome as well, as the flow iside lumen is non-newtonian blood, while in porous domain I have plasma. Also to define the subdomain, I need a seperate material in tissue, which makes a boundary interface and there my problem initiates. I cannot apply the proper BC.

May 17, 2014, 07:02		#23
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,716 Rep Power: 143	So I suggest you can either: * Spend time (probably lots of it) trying to work out why this being weird. I suspect you have already spent lots of time on this so I guessing this is unlikely to be productive. * Give up on the approach you are using and try something different. Maybe add the porous flow inertial loss factor. Maybe try a completely different porous flow model.

May 17, 2014, 09:19		#24
ftab Member Ftab Join Date: Sep 2011 Posts: 87 Rep Power: 14	Thanks Glenn for your time. As you are correctly mentioning, I have spent so much time to figure it out and getting feedback from an expert like you reassures me that I am not doing something stupid in the process. I will keep on playing with the parameters to reach to physically sound results. Since I might encounter the following issues again, could you please briefly answer question 1 and 3 of Post #11? I repeat them here. 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. (from the units, I am confused what to put there, only the momentum term or the whole -C**u-u0)?. Please write the simplest example you can make, and I will follow on that, just kill the tangential 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. With my best regards and appreciating your invaluable time, Ftab

May 18, 2014, 06:45		#25
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,716 Rep Power: 143	Blocking the z direction is easy - just use the momentum course you describe with u0=0 for the direction. I would let x and y remain unrestrained so the radial flow works. Note this will allow flow in the theta direction, but hopefully this is small enough to be OK. Here is two ideas to get the radial direction in a solid domain: * Make a function of xyz location. If the shape is simple you can do it analytically. If it is complex then do it on a solid modelling package and generate a 3D interpolation file (one file for each of the three directions to define the vector). * Do a simulation with a diffusion AV where you set the inside to a value of 0 and and the outside to a value of 1. The AV will then diffused between the inside and the outside. Take the grad of the AV and hey presto you have a vector field which is normal to the surface through the solid domain.

May 19, 2014, 10:48		#26
ftab Member Ftab Join Date: Sep 2011 Posts: 87 Rep Power: 14	Dear Glenn, Thanks for the reply and your smart idea how to calculate the vector field. Just to clarify for me and make sure that I got the point, I quickly summarize here and ask for your confirmation. 1- to let x and y remain unrestrained, we put zero as the source term. But for the momentum source term in Z direction to set u0=0, what do we put? Do I need to define an expression equal to -1e-5 *(Z-velocity-u0)? My Naive question in the former post was also this. To set momentum source, what do we explicitely put in the table in CFX? calculated value containing the Coef? or a constant? Sorry to ask a very trivial question. 2-Thanks for this magic solution using AV. What you mean with diffusion AV is simply defining an AV (Volumetric, right?). and in the fluid domain, define it as an algebraic variable (definitely not solving transport equation or diffusion trans. Eq., right?). To define it I simply use an expression with "inside" CEL function to let the tissue side become one, and the lumen 0. And then, to define the gradient, I define a second AV as a vector, and define its x-component as =first_AV.Gradient X for instance. Is this approach the one you meant? Sorry that I am not so professional and quick to catch your brilliant idea.

May 19, 2014, 18:35		#27
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,716 Rep Power: 143	1) So the source terms would be: X = 0 Y = 0 Z = -C*(Z-z0) Then set z0=0 [m/s] and C=1e5 [kg m-3 s-1] (NOT 1e-5!). You might also need a source term coefficient of -C. 2) The AV can be any form, volumetric is fine. No, it is not an algebraic AV. You want a diffusion transport eqn. To set the 0 and 1 thing you have a few options - The best (if it works) is to use the interface conditions on the inside and outside to set the AV to defined values as 0 and 1. If it does not like that then use a source term in the fluid and outside regions to lock it to 0 and 1.

May 20, 2014, 06:58		#28
ftab Member Ftab Join Date: Sep 2011 Posts: 87 Rep Power: 14	Dear Glenn, I cannot thank you enough on this. I will try to apply your smart ideas and hopefully will be back with good news.