[BlnPhoenix]

Hello,

i'm trying to model a filtration module which is submerged in my fluid domain. The fluid has to travel trough membrane to reach the pressure outlet. I wanted to use a porous region which get's a porous viscous resistance value (only need darcy's law).
The problem now ist, that the fluid enters the porous region on one face and exits the region on the same face or on opposite face which is not a realistic behavoiur. I want the fluid to remain fully within in my membrane region. How can i do that?!

[prashant810]

hi,

Can you please send the geometry then i can explain you?

thank you
Prashant

[fluid23]

This is probably an issue with your tensor definition. The most common pitfalls are:

1. You are assuming isotropic tensor (i.e. same resistances in every direction). Most filters do not behave this way. In reality your primary flow direction will have one value and then everything off-axis from that direction will have another. It is practically impossible to test the off-axis properties of most filters in a lab setting so the assumption used in industry is a 10:1 or 100:1 ratio for the orthotropy. (i.e. if you have 10 kg/m^4 on axis then off axis you should use 100 or 1000). This will encourage the local flow to follow the axis definition you define). Remember the phrase, path of least resistance? That is applicable to fluids too!

2. Your axis definitions for your tensor are improperly defined. This part is heavily determined by your geometry and you need to have some understanding of how the flow behaves inside the media. It sounds like you understand this already, but it isn't clear from the info you provided what is going on in your analysis. There are a few options that I commonly use for filter media that I will outline below. If these don't sound useful to you, perhaps elaborate on your model a bit...

a)Constant Axis: This would be useful for something like a filter in a duct or pipe where your filter is perpendicular to the flow path, is flat, and pretty boring and basic... (No pleats, nothing fancy). Here you would want to define your axis as the primar flow direction. So for a pipe flow oriented along the x axis, [1 0 0]. I personally like to use axisymmetric so that you only have to define on and off axis properties.

b) interpolateDirection/Field Function: For filters that have more difficult geometry like pleats, curved faces, or something along those lines you can create a field function that will define a vector in every cell based on the face normal of the closest cell on a face of your choice. There is an article on steve portal on how to use this approach for anisotropic thermal conductivity. The principle is the same and shows some images of you can control vectors inside a medium.

If you get stuck let me know.

[BlnPhoenix]

Originally Posted by MBdonCFD

This is probably an issue with your tensor definition. The most common pitfalls are:

1. You are assuming isotropic tensor (i.e. same resistances in every direction). Most filters do not behave this way. In reality your primary flow direction will have one value and then everything off-axis from that direction will have another. It is practically impossible to test the off-axis properties of most filters in a lab setting so the assumption used in industry is a 10:1 or 100:1 ratio for the orthotropy. (i.e. if you have 10 kg/m^4 on axis then off axis you should use 100 or 1000). This will encourage the local flow to follow the axis definition you define). Remember the phrase, path of least resistance? That is applicable to fluids too!

2. Your axis definitions for your tensor are improperly defined. This part is heavily determined by your geometry and you need to have some understanding of how the flow behaves inside the media. It sounds like you understand this already, but it isn't clear from the info you provided what is going on in your analysis. There are a few options that I commonly use for filter media that I will outline below. If these don't sound useful to you, perhaps elaborate on your model a bit...

a)Constant Axis: This would be useful for something like a filter in a duct or pipe where your filter is perpendicular to the flow path, is flat, and pretty boring and basic... (No pleats, nothing fancy). Here you would want to define your axis as the primar flow direction. So for a pipe flow oriented along the x axis, [1 0 0]. I personally like to use axisymmetric so that you only have to define on and off axis properties.

b) interpolateDirection/Field Function: For filters that have more difficult geometry like pleats, curved faces, or something along those lines you can create a field function that will define a vector in every cell based on the face normal of the closest cell on a face of your choice. There is an article on steve portal on how to use this approach for anisotropic thermal conductivity. The principle is the same and shows some images of you can control vectors inside a medium.

If you get stuck let me know.

Dear Matt,
thanks for your reply!

I think i should've provided more information on my problem as you mentioned. I attached a new pic for my geometry. Firstly, it's a 3D problem. The membrane i need to model is drawn as a solid block. It's connected to side parts of the membrane which are impermeable from outside and subsequently to pipes which lead to my pressure outlet. The thing now is, that my fluid should get "sucked" from all three spatial directions into this membrane and travel through the connected parts to the outlet. I understand now that it makes total sense that the fluid can exit my porous region on the same or opposite surface as it entered. I feel 2. b) of your post is what i need to do for my porous region. Is it possible to define direction and strength of the resistance as function of location in my porous region? I would give it x,y and z for the first couple mm's of the respective surface and the set the resistance to a value that fluid can only travel in the direction of the outlet orientation (y-direction in this case). I'm not sure this totally would make sense, because how can fluid enter the region thats coming couple of mm's after entering the membrane?!
Or is it possible to define fluid flow only in positive/negative direction of a certain surface? So then my fluid could enter in say positive x-direction but not exit the same surface in negative x-direction. Is this how it could work?
regards

[fluid23]

ok, help me understand this a little better. I am thinking you are trying to over define your problem.

a) the block is a porous medium and is infact isotropic, right? I am thinking something like a block of sand. there is no doominant fibourous structure in any one direction, right?

b) why pressure outlets on the tube? do these opperate at constant p? mass flow inlets (with negative values) would be a better choice if you know flow rate.

c) what are your far-field conditions? (i.e. what are your boundary types away from the block?)

d) what exactly is your issue now? I am not 100% clear on what you want to know aside from how to define the vectors.

[BlnPhoenix]

Hey Matt,

thanks again for your post. I try to be more specific on my overall aim, maybe my problem gets clearer. See attached pic of my overall domain. I have a water tank which has an inlet pipe (bc = velocity inlet), the fluid travels along some baffles into an area with two rotating discs (bc = rotational velocity) sitting on a shaft. these discs should act as an degassing outlet for microbubbles. I hope to model this correctly using the euler-euler-approach. however i fear velocity inlets for the degassing discs can not have a rotational velocity at the same time, is that correct? the fluid travels further in the area where the membrane sits (brown rectangular in pic). Here it gets filtered, i dont need to model the air getting filtered but i need an accurate prediction of this filter, that it "sucks" in the water. What i see however from a first single-phase simulation is what i tried to show in my first post. The fluid enters the porous domain but does not remain within the membrane region, it leaves the domain on several faces. this is not what i have in reality, in reality the vaccum pressure makes sure that no water can leave the membrane domain onces it has entered. so i had no luck solving this problem so far.

to your specific questions.

1) i'm not sure if its isotropic but i can surely assume that, if only my mentioned problem with exiting fluid would be resolved correctly.

2) hm, i understood this is common in cfd to give the pressure outlet condition as an outlet bc. i tried negative mass inlet with an according value to my inlet velocity and i saw no good flow prediction. i have to say with pressure outlet it converges best. it's only single phase atm though..

3) in addition to my mentioned bc's i have assigned the non slip-condition to some of my walls, to predict correctly symmetry walls and the open tank top.

4) my main problem atm is the one with the membrane, that fluid exits porous region on same surface, after it has entered the porous domain. i need something like a filtration part, that only sucks the water which will definilty stay in the porous region and travel to the outlet pipes/pipe instead of partly leaving the domain. the problem is, that the filtration part has influence on my studied flow behaviour and subsequently of my air bubble distribution in the tank. i would be delighted if this could be modeled correctly. i have two values for flow vs. pressure drop for this membrane btw. has this something to do with tensor setup?? i tried also isotropic, axissymetric and principal tensors, i don't see different flow behaviour in the porous region.
second problem would be the rotating degassing boundaries. but that comes later...

thanks for your thoughts!

[BlnPhoenix]

I still wasn't able to solve my membrane problem. How can i implement surface resistance as in Autodesk's Simulation CFD? Thanks a lot for your thoughts.

[fluid23]

can you be more specific than 'unable to solve my membrane problem'? Is it not converging? Not solving at all? Results don't make sense?

As for Autodesk's implementation of 'surface resistance', its fairly unsophisticated. From what I have read, it is only used to reduce model complexity and the assumptions it makes are probably not valid for what you want to model.

I am thinking that I sent you down a rabbit hole now though. Let's return to this question:

a) the block is a porous medium and is infact isotropic, right? I am thinking something like a block of sand. there is no doominant fibourous structure in any one direction, right?

You didn't really correct this assumtiion so I was assuming that your filter was a block (not a sheet) and that you were using the word membrane improprely. Is your filter infact a sheet and not a block? Not sure why you would want to use surface resistance if its a block...

If its a sheet, then your model is setup wrong... You need a porous region that is the correct thickness for your membrane and then a separate body of fluid inside of block.