[frossi]

Hi all,

I came across a source that stated "Velocity specified inlets are intended for incompressible flows. Using velocity inlets in compressible flows can lead to non-physical results. Pressure and mass flow inlets are suitable for compressible and incompressible flows


1. Does the above quote refers to FLUENT only, or CFX as well? In fact I am using CFX, and when I select the boundary conditions I can only choose between inlet, outlet, opening, wall, and symmetry. So Could someone please clarify it?

2. Also, when is it preferable to use the "opening boundary condition" and what does opening actually mean? I usually use it for the fluid domains which are more distant from the body (and are not inlet or outlet) like the domain highlighted in the picture.

Thank you friends.

[ghorrocks]

This is all covered in the CFX Modelling guide, in the section titled Boundary condition modelling - sections 2.2 and 2.3.

[frossi]

thank you ghorrocks for the useful link. While that clearly answered my first question, it didn't really clarify the one about the "opening" boundary condition. The modelling guide defines opening as

"Define a region as an “opening” when the full prescription of information at that location is not readily available; for example, if the value of pressure is known, but the direction of flow is unknown. It is also important to note how ANSYS CFX treats the value of pressure that you specify at an opening. If, during the course of the solution, flow is directed out of the domain, then the value is treated as static pressure. If, instead, the flow is entering the domain, the value is taken to be total pressure, from which the static pressure is calculated."

What confuses me is the part that says that CFX will interpret the pressure as static or total depending on whether the flow leaves or enters the system.

So my questions are:

1. Flow in that region (highlighted in the picture) should continue straight, as a "continuation" of the inlet. Thus, it's neither entering nor leaving the system. So what is happening?

2. If I assign to such region a pressure value, but I have no idea of the direction of the flow, my results could be dramatically altered depending on whether CFX treats the pressure as static or absolute. So in this case, "opening" doesn't seem like a reliable option. Any suggestions?

Thank you very much

[ghorrocks]

You can set an opening to be static pressure in both directions if you want.

Q1: There will be small cross currents which will push air out the domain or pull air in. For this flow the opening boundary will be applied.

Note that openings and outlets can have numerical stability problems when the flow is parallel to the boundary or is in both directions (forwards and backwards). So if this causes stability problems you might need to change boundary condition types.

Q2:

my results could be dramatically altered depending on whether CFX treats the pressure as static or absolute

You are confused between static and total pressure versus gauge and absolute pressure.

As I said, if the different approach to forward and backward flow is not appropriate for your flow then turn it off.

[frossi]

thanks ghorrocks for your clarification and yeah, I am struggling to understand the pressure nomenclature in CFX.

So, I know that
ABSOLUTE PRESSURE = (ATMOSPHERIC PRESSURE) + (GAUGE PRESSURE)

my questions are:

1. Does gauge pressure includes any type of pressure other than the atmospheric one?
If yes, is it correct to assume that in the case of air flow over a wing, gauge pressure is the dynamic pressure caused by the airflow?

2. In the main domain tab in CFX there is "Reference Pressure". What does this pressure refers too? I understand it as ambient pressure and usually set it to 1 atm.

3. For "inlet" or "opening" boundary conditions I have to specify a "Relative Pressure". What does this pressure refers too? I usually set it to 0 because I don't know what to do.

Thank you, hope you can clear my doubt.

[Opaque]

You should refer to the documentation for an initial description,

For reference pressure,

CFX-Solver Modeling Guide | Chapter 1: Basic Capabilities Modeling | 1.2. Physical Models | 1.2.8 Setting a Reference Pressure

For absolute pressure,

CFX-Solver Theory Guide | Chapter 1: Basic Solver Capability Theory | Buoyancy

Therefore, Relative Pressure = Absolute Pressure - Reference Pressure - Hydrostatic Pressure (if Buoyancy active)

Hope the above helps,

[frossi]

thank you Opaque. I did read those sections on the CFX modelling guide but I still don't understand the following:

1. Does gauge pressure includes any type of pressure other than the atmospheric one?
If yes, is it correct to assume that in the case of air flow over a wing, gauge pressure is the dynamic pressure caused by the airflow?

2. What is reference pressure and what is its physical meaning? I didn't understand the manual definition.

3. For inlet boundary condition, I can either specify "static pressure" or "total pressure". I believe "static pressure" is the atmosphere pressure and "total pressure" is the sum of atmospheric plus dynamic dynamic pressure. Am i correct?

Could someone please give a specific answer for these doubts I have? thank you very much everybody

[Opaque]

Not sure why you continue mentioning the atmospheric pressure. It has not bearing anywhere.

The variable Pressure is a "convenient pressure" to minimize round off errors. If you read the documentation carefully, you should select a reference pressure such the "convenient pressure" represents variation about the selected reference pressure, i.e. least round off.

For cases with buoyancy, there is also the possibility to remove further contributions (read the documentation for the details) to make the "convenient pressure".

Whenever the software asks for Relative Pressure, it is asking for the "convenient pressure", and it is up you to account for the transformations.

Regarding Total Pressure = Static Pressure + 0.5 * density * velocity ^ 2 (incompressible flow). For compressible flow the definition is a function of the equation of state.

If you do not have buoyancy active, you can set the Reference Pressure to 0 [Pa], run in double precision, and all your worries will be gone since all the pressures are absolute from there on.

Hope the above helps somehow,

[-Maxim-]

If you search this forum, you will also find more discussions and definitions of the "different pressures" CFX is using

[frossi]

Opaque,

Thanks again for your answer. I am new to CFX and I am still struggling with the CFX pressures, but I want to clearly understand how to use them. So, I am simulating flow over a 3D wing at Mach 0.4.

I want to simulate exactly the flow conditions encountered at 5,000 m of altitude. So, in order to tell CFX that I am at such altitude, I have to input somewhere the pressure that exists at 5,000 m.

My questions are:
1. what would you set as the reference pressure and why?

2. What would you set as the relative pressure and why?


Thank you for your patience