CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   calculation of additional variable in multiple domain (

cosine May 3, 2011 05:27

calculation of additional variable in multiple domain
1 Attachment(s)

I need to model mass transport in arteries. I have two domain e.g. one is a fluid domain (blood) and one is porous domain (arterial wall) as shown in the figures.

I create an interface between the fluid and porous domain. In the fluid, i create an additional variable (concentration) which is transferred in the domain. I want to transfer the variable from the fluid domain to the porous domain through the interface.
Do i need to add a subdomain and sources? I what cases a subdomain is necessary?
I have enable the beta features.
Should i enable the additional variable in porous domain also? Otherwise the concentration is not calculated.

Thank you very much for your time

stumpy May 3, 2011 09:23

The AV should be enabled in both domains. If you're just solving a transport equation then I would expect the domain interface to have a "Conservative Interface Flux" option for the AV, and this is probably the default. This just means the AV is transported with the fluid, so any fluid that passes across the interface will carry the AV with it. Is there any fluid flow across that interface? I assume you also want a flux across the interface based on the concentration gradient of the AV. If you set a diffusivity for the AV then this may provide the correct interface flux. If the equation for the interface AV flux is more complicated than a simple diffusivity (e.g. there's some resistance too), then set up the domain interface with a Zero Flux option for the AV then add your own source and sink terms on the two sides of the interface. No need for a subdomain, they are just used for volumetric sources. You would need a boundary source which is created on the side 1 and side 2 interface boundaries.

cosine May 3, 2011 09:35

Thank you Stumby,

Actually, in my case i cannot use a consevative interface flux, because the transport across the interface is based on an CEL expression which defines a transfer coefficient. (I also have diffusivity). The expression is dependent to wall shear stress.
Until now i use that way of boundary conditions, but i observe too large values of concentration in the porous domain. I will try the zero flux and source/sink terms as you suggest.
Correct me if i am wrong, i will define sink in the fluid domain and source at the porous domain? The sink term should be negative?

stumpy May 3, 2011 12:02

Yes, sink in the fluid and source in the porous, and the sink should be negative. However, if you are using wall shear stress, then I assume there's no interface between the domains since you need a wall in the fluid domain. So you can make the AV sink in the fluid domain a function of the local wall shear easy enough, but I don't know how you can make it a function of the porous AV concentration since that value won't exist in the fluid domain. Similarly, in the porous domain you can't get the local wall shear stress or the AV value from the fluid side. Come to think of it, even if you did have an interface a similar problem would exist.

cosine May 3, 2011 14:21

I am considering your idea, but i have some questions.
1) Even if i have interface, i think i can calculate wall shear stress at this region from the side of the fluid domain (at least i can show it in CFX-post).
2) I don't know what i am doing wrong but using negative sink value, i observe negative concentration at the interface from fluid side. Is that wrong? Or the negative shows the direction out of the domain?

stumpy May 3, 2011 15:44

Yes, you can set the wall shear on the fluid side of the interface, but then if you add a source term on the other side of the interface I don't think it can be a function of the wall shear from the other side of the interface.
Regarding the negative concentration, make sure the sink (negative source term) goes to zero as the concentration goes to zero. It sounds like you'll pulling out too much AV making the concentration negative.

ghorrocks May 3, 2011 19:10

Why are you modelling the artery as a porous domain? Does the fluid (blood plasma?) go through the artery wall? If not then modelling the artery as a solid domain might be easier.

cosine May 4, 2011 04:01

Yes, i assume that plasma also flows in arterial wall. So, i need the porous domain.

cosine May 5, 2011 03:46

Thank you both for your advice.
I think that i am in a good way. I correct also the negative values. You are right stumpy!

Can you help me, if i can transform the transport equation for the AV in the porous domain to a convection-diffusion-reaction equation? In fact, if the terms of diffusion+convection are equal to 0, in the convection-diffusion-reaction equation the terms of diffusion+convection are equal to r*c, where r is a reaction rate and c the concentration.

ghorrocks May 5, 2011 07:27

If you set the AV to convection diffusion model, then you can turn diffusion on and off by setting the diffusion coefficient, you can turn convection on and off by using a solid domain and you can turn reactions on and off with either a source term (for simple chemistry) or a full chemistry model for more complex chemistry.

cosine May 6, 2011 04:30

Thanks for your reply.
I do not know what i am doing wrong but i observe too high values of concentration in the porous domain. I expect to have about 4 mol/m3 and i take the values multiplied x10^8.
At the sink, should i use negative values both in flux and in transfer coefficient?

bitak January 27, 2013 13:38

I have a problem like you.:)
I want to reproduce an article but I don't know how Should put a boundary condition for wall!!!!!!!!!!!:confused:
my geometry is a tube( d=7mm and L=15.4 cm ).

Boundary conditions for concentration of LDL at the inlet, outlet and wall, sequentially, are as follows:
C(0, y) = C0 ( inlet concentration)

@ outlet flux = 0

on the wal : CwVw (wall concentration * infilteration velocity)
I really be happy and will be thanks if you answer to me.

All times are GMT -4. The time now is 11:04.