Hi... I spent hours trying to get the definition of "Zero Gradient" when specifying "Turbulence" for "Opening" boundary condition.

Can anyone please help if you know what the term means?

The new design of the user manual is very louisy....I find it a lot harder to get what I'm looking for these days.

Thanks for help.

Hi.... Really hope that someone can clarify this term for me. What is the effect if zero gradient for turbulence is set at outlet opening boundary condition?

I run a few cases with K-e model using 5%, 10% & zero gradient for turbulence at inlet & outlet. It doesn't seem to change velocity & static pressure distribution in my problem. However, I get a message in Pre saying that zero gradient is better. Has anyone found that this advice is true?

If zero gradient means all variables are set to a constant value at outlet boundary, then it can only be true when you extend the outlet location very far away from flow domain.

'Zero Gradient' means that the variable is 'fully developed' on the inflow portion of the opening; ie, dphi/dn=0.

Thanks, Phil. In my case, it means turbulent profile will be the same after the outlet. Right? Would you mind to help explaining the reason or giving some references where this condition works better?

I still can't figure out the difference between specifying a constant turbulence intensity and using Zero gradient condition.

Sometimes the solution is insensitive to turbulence inflow BCs because the turbulence is often source-dominated (production/dissipation).

Other times the inlet levels do matter. If the flow is fully developed, the zero gradient condition makes sense; it will give a fully-developed turbulence profile. Otherwise it is probably best to specify the inlet level.

[Sudharshani]

hai Phil,
i would like to know what do u mean by fully developed turbulent flow....?
i am using ANSYS CFX to model supersonic CD nozzle and i would like to know can i use zero gradient under the turbulence section ?
bcos when i use two different options (zero gradient and mediem intensity and eddy viscosity) i got 0.01 diffrence in the mach number values . and also the shock formation inside the nozzle is also diffrent using zero gradient option.

can u expalain when and why we should use "zero gradient".option?
thanking you
sudhar

Originally Posted by Phil
;74607

Sometimes the solution is insensitive to turbulence inflow BCs because the turbulence is often source-dominated (production/dissipation).

Other times the inlet levels do matter. If the flow is fully developed, the zero gradient condition makes sense; it will give a fully-developed turbulence profile. Otherwise it is probably best to specify the inlet level.

[ghorrocks]

I think you will find Phil has long since past away, this post is over 4 years old. But no matter.

Fully developed flow is flow where the gradient of the variable in the flow direction is zero. That is the variable does not change as the flow progresses as it is "fully developed".

I don't think a zero gradient boundary is appropriate. Some level of upstream turbulence will be present and it looks like in your case it is affecting results so you need to make sure you get it right. What incoming turbulence level are you modelling? You should use this as your upstream turbulence condition.

A second possibility is if minor changes like this change your results then I recommend you move your upstream boundary further away from the region of interest.

[elisun]

Hi.

I'm doing both steady state and transient analysis for a given case. For the steady state I give constant mass flow at the inlet and pressure at the outlet, and I run it. Then I use the resulted inlet pressure as an inlet boundary for the transient case, and I run the transient case. Then I check the mass flow at the inlet. The mass flow would be oscillating.
I read in cfx manual that we choose the direction of flow to be normal to boundary when we have constant mass flux at inlet.
So my question is should I use zero gradient or normal to boundary for each steady state run and transient run, since I have constant mass flux for steady state but oscillating mass flux for transient. Would it be ok if I use normal to boundary for steady and zero gradient for transient?

Your help is highly appreciated.

[ghorrocks]

You choose boundary conditions to match the flow you are trying to simulate. That is the first consideration when choosing boundary conditions.

[elisun]

Right. Which in my case for steady state, normal to boundary and for transient, zero gradient match the flow. I just didn't want there to be any inconsistency between steady state and transient boundary conditions.

[naruto5255]

How to specify zero turbulence gradient in pressure outlet boundary condition

[ghorrocks]

The documentation states this clearly - the exit boundary condition for all convected scalars (including turbulence) is convected from inside the domain. This is a more accurate boundary condition than zero normal gradient.

[katty17]

Hi All,


I want to impose zero-gradient boundary condition at a boundary of my computational domain for the transport of a new variable in ANSYS CFX. The value of the static pressure should also be equal to a constant value at this boundary. Is there any way to define both of these boundary conditions on one boundary in CFX?


Thank you

[Opaque]

Zero gradient of which variable?

You cannot specify two conditions for the same variable at the same location for the Navier Stokes equations. Either you know
1 - the value (Dirichlet),
2 - or its gradient or flux (Neumann)
3 - or a relationship between value and flux (Robins).

[Gert-Jan]

Originally Posted by katty17

Hi All,


I want to impose zero-gradient boundary condition at a boundary of my computational domain for the transport of a new variable in ANSYS CFX. The value of the static pressure should also be equal to a constant value at this boundary. Is there any way to define both of these boundary conditions on one boundary in CFX?


Thank you

Please explain your system and what you are trying to do. There might workarounds that are less obvious.

[katty17]

Thank you for the reply,

I want to model the mass transport of an additional variable in my porous domain.
At one of the walls the boundary condition for the Navier Stokes is constant pressure of P0 and for the transport equation of the additional variable (q) is dq/dn=0 (zero gradient in the direction perpendicular to the boundary). If I use a wall boundary condition in fact I can set the value of normal velocity equal to zero and there would also be another option that allows me to set the flux of additional variable equal to zero. I am now wondering if I can have such boundary condition that instead of setting normal velocity equal to zero sets the value of pressure equal to a constant value.

[Gert-Jan]

Still don't know what system you are modelling. Is it confidential that you're not allowed to share pictures and a clear description? Now it sounds as something completely unrealistic. But ok, we'll see.

You cannot set a pressure on a wall. Only on an outlet, inlet or opening. I would opt for an outlet or inlet: at the location of your wall, you can define an outlet with a pressure higher than your local pressure. As a result, CFX will build a wall where fluid tends to flow into the domain
As an alternative, you can define an inlet with a pressure lower than your local pressure. As a result, CFX will build a wall where fluid tends to flow out the domain.

Maybe you can get away with this. But mostly, because you apply unphysical BC conditions, the solver might crash. Just give it a try.

[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).

[Gert-Jan]

Originally Posted by katty17

Dear Gert_Jan,

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).

Why don't give it a try? Use an inlet with too low pressure. Then no flow will go in. You can set the the q on that boundary. Not sure if something will diffuse into your domain, but as I said: give it a try.

[katty17]

But for the verification process I need to have pressure on this boundary be equal to let say 50mmHg.