[Opaque]

If you expect the flow to leave the domain on that boundary (right most boundary in Domain 2), the flow must be extremely slow to impose a Dirichlet condition.

If the mass flow is leaving the domain, what in the physics can force the outlet value? I do not think the boundary conditions on that boundary, pressure specified with outflow plus fixed additional variable is an ill-posed problem unless the Reynolds number is very small, say ~1

If that is the case, I would use an outlet boundary condition, and manually add the BC you want for the Additional Variable, the UI will warn you but you can try and see if the solver accepts the setup. Then, verify the solution makes sense for you.

ADDITIONAL VARIABLE: MyVar
Option = Value
Additional Variable Value = <real>
END

[Gert-Jan]

Originally Posted by katty17

Dear Gert_Jan,
No, the problem is not confidential. I am trying to model mass transport in living tissues. Below are the links to my problem's boundary conditions as well as the governing equations.
https://pasteboard.co/IPdoaVBg.png
https://pasteboard.co/IPdFfTs.png.

And sorry for the confusion. The reason for mentioning wall in my previous post was to show that it is possible to set a boundary condition for the Navier-Stokes and another one for the mass transport equation on exactly the same wall. I don't want to use the wall boundary condition. As is shown in the attached figure, at the outlet boundary condition of domain#1, I should set the value of pressure to a constant value and also have zero gradient for the transport of the additional variable "q". Is there any way to do this using the available CFX boundary conditions?

Although using the outlet/inlet/opening boundary conditions, it is possible to set the value of pressure as well as that of the "q" on a boundary condition, it would be fine if I could set the value of the gradient of the q (dq/dx=Constant) rather than its value (q=constant).

Given the uncommon physics, I would opt for somehting like Comsol, which is better equipped for this than CFX.

[katty17]

Dear Opaque,


Thanks for letting me know about this approach. Although it works in some cases, there are cases that using this approach will end up with an error "segmentation violation".


Now I have three questions:


1- There must be a reason that ANSYS did not consider "zero flux" option for the additional variable in the "opening" boundary conditions. May I ask you to please share your thoughts on this.


2- When I use "Outlet" boundary condition, CFX just requires the outlet pressure and do not ask any information regarding the value of additional variable for this boundary condition. Based on my knowledge there must a boundary condition defined on this boundary otherwise we would not be able to solve the transport equation numerically. How the "Outlet" boundary condition handle the additional variable?


3- I know we can force the values of velocity vector components to be equal to a specific value at a location using the general momentum source term. Is it possible to do the same with the pressure value? I mean can we set the value of pressure to be a specific value at a specific location inside our computational domain?



Many thanks in advance.

[Opaque]

1- There must be a reason that ANSYS did not consider "zero flux" option for the additional variable in the "opening" boundary conditions. May I ask you to please share your thoughts on this.

What would be your definition of flux at an opening? Here are possible alternatives:

1 - Flux = mdot * Additional Variable

2 - Flux = - DiffCoeff * grad (Additional Variable).Normal

3 - Flux = mdot * Additional Variable + DifCoeff * grad (Additional Variable).Normal

I am not certain which of three would you expect, nor which one will make sense for you.

[QUOTE]
2- When I use "Outlet" boundary condition, CFX just requires the outlet pressure and do not ask any information regarding the value of additional variable for this boundary condition. Based on my knowledge there must a boundary condition defined on this boundary otherwise we would not be able to solve the transport equation numerically. How the "Outlet" boundary condition handle the additional variable?
[\QUOTE]

I agree with you on the need for a boundary condition at every boundary. However, the software provides us with a built-in treatment for outlets where no user input is required. Which treatment is used?

The software assumes that diffusion is negligible; therefore, is advection dominated at the outlet (recall is also subsonic); therefore, the solution at the boundary MUST come from the interior.

[QUOTE]
3- I know we can force the values of velocity vector components to be equal to a specific value at a location using the general momentum source term. Is it possible to do the same with the pressure value? I mean can we set the value of pressure to be a specific value at a specific location inside our computational domain?
[\QUOTE]

Though the software may allow you to force a value anywhere, it is not necessarily correct to do so. The Navier-Stokes equations, and the advection transport equations do not support multi-value boundary conditions at the same boundary. Either you know the value exactly, the gradient, or combination of both (Robins condition), but not both separately.


Many thanks in advance.

[katty17]

Thanks for the reply.

What would be your definition of flux at an opening? Here are possible alternatives:

1 - Flux = mdot * Additional Variable

2 - Flux = - DiffCoeff * grad (Additional Variable).Normal

3 - Flux = mdot * Additional Variable + DifCoeff * grad (Additional Variable).Normal

Option #2. In other words, I just wanted to set the gradient equal to zero (i.e., grad (Additional Variable).Normal=0 ) at this BC. So option #2 works here.

The software assumes that diffusion is negligible; therefore, is advection dominated at the outlet (recall is also subsonic); therefore, the solution at the boundary MUST come from the interior.

Great. So when we extend the outlet so that it represents a far-field BC, can we feel confident that the gradients there are all equal to zero? Based on your information, if I set the outlet BC where the boundary is located near the inlet, I should face convergence issues. Am I correct?

Though the software may allow you to force a value anywhere, it is not necessarily correct to do so. The Navier-Stokes equations, and the advection transport equations do not support multi-value boundary conditions at the same boundary. Either you know the value exactly, the gradient, or combination of both (Robins condition), but not both separately.

Actually, I wanted to use a symmetry BC at the outlet to enforce the normal gradient of the additional variable to be equal to zero. However, using the symmetry BC we can not set the value of pressure. To solve this issue, I wanted to create a thin subdomain close to the outlet BC and set the value of pressure to the desired value in the subdomain using the general momentum source terms. However, I am not sure whether this is a valid approach.

[ghorrocks]

Many boundary conditions can be validly applied to the inlets and outlets of domains. If you do a sensitivity study of how close the boundary can be to the region of interest you will find that boundary conditions which more closely match the actual conditions can be placed a lot closer than ones which do not match well. In other words, the error from the boundary condition fades out over distance; and boundaries with more error take longer to fade out.

This means that the CFX applied boundary condition where the boundary value is convected from the flow is a better boundary than the zero flux boundary for cases where the flow is dominated by convection. So a sensitivity analysis will show that the CFX default convected boundary will be OK closer to the area of interest than the zero flux boundary. This means the simulation will be smaller for a given accuracy with the convected boundary compared to the zero flux boundary.

Regarding your last paragraph - If you think this was a good approach don't you think it would already be in the software by default? CFX does not do your described approach as it is not a recommended method.