[mejahan]

Hello friends,

I am simulating a dynamic mass flow rate at the outlet and presser inlet BCs. The mass is changing with time by an input function file and the flow is incompressible.
But the mass flow or velocity does not follow the BC(attached file).
The only option that I was speculating might affect the simulation is "mass flow update" option on outlet Mass flow BC and I do not know the effect of this option, but for now this option was not selected by default.

I would appreciate if anyone can help me.


Mehdi

[ghorrocks]

You plotted the velocity. What does the mass flow rate look like?

[mejahan]

Hi Glenn,

As it is incompressible flow the mass differs with velocity just in a constant coefficient , density and area.
AS it shows on the figure, the BC does not follow the mass flow that I set on some points.

[ghorrocks]

Can you post your CCL?

[mejahan]

Originally Posted by ghorrocks

Can you post your CCL?

Hi Glenn,

I have plotted the CCL, as you can see it is the same as the input file that I posted before.
I am confused about the results, why the solver does not follow the BC when getting near the negative velocity?
The problem can not be from the "Mass flow update" option because by default it is "scale mass flow" which is right.
But I don't know how the solver interpolate the input data. It works fine before 0.35s but after that the input data and the solver BC are not the same.

[ghorrocks]

That is not the CCL. The CCL is the text file which sets up the CFX run. It is repeated at the top of the output file. Please read the documentation about the CCL file and post it.

[mejahan]

Hi Glenn,

I think I found the source of the problem and it is the BC.
When I set the Pressure or Mass flow BC, the solver will consider an artificial wall at the boundary to prevent the inflow at the outlet and outflow at the inlet.
And when it is getting to the negative mass flow rate, the solver does not allow such condition.
It seems that for now the only option is Velocity inlet and Opening at the outlet, but I dont see the opening BC option and more importantly I want to use pressure inlet mass flow outlet BCs.
Now my question is that is there any way to change the BC setup manually in CFX, in a way that I do not have artificial walls in Mass flow and pressure BC?
I would appreciate if you can help on this issue.

Thanks

[lmark84l]

What exactly are you trying to simulate? Is this an internal or external flow problem?

For external flow, I’ve been able to successfully implement a mass flow inlet with a pressure outlet BC provided that 1) my domain was large enough so I did not have flow trying to recirculate back through the outlet and 2) I paid careful attention to the outlet pressure specification (i.e. be mindful of how CFX uses relative and reference pressures).

Not sure if that helps at all, but figured I’d chime in.

[ghorrocks]

If you want to use a pressure inlet and a mass flow outlet then you can make the inlet a pressure opening and the outlet a velocity/mass flow condition and then both the inlet and outlet can handle reverse flow fine.

[mejahan]

Thanks,

If I set the mass flow outlet, then we have problem of artificial wall, but velocity component works. But the question is, if I set the normal component of the velocity, what is the distribution of the velocity across the outlet area? is it uniform if I do not specify a profile, or it is just the average and the solver gives the distribution according to this average value?

[ghorrocks]

Mass flow boundary conditions certainly can handle back flow - I have done it before. So you must be using different options to me. That is why I want to see your CCL to see what options you are using.

When you set velocity it uses the velocity across the entire boundary. So if you set a constant value it is constant (ie plug flow). if you want a profile then you need to define a function which sets a profile.

Have a read of the documentation about these different boundary condition types. There are lots of options available.

[mejahan]

Originally Posted by ghorrocks

Mass flow boundary conditions certainly can handle back flow - I have done it before. So you must be using different options to me. That is why I want to see your CCL to see what options you are using.

When you set velocity it uses the velocity across the entire boundary. So if you set a constant value it is constant (ie plug flow). if you want a profile then you need to define a function which sets a profile.

Have a read of the documentation about these different boundary condition types. There are lots of options available.

I have studied the documentation about the CFX BC(attached). As I have read and experienced, pressure and mass flow BCs, impose the artificial walls in reverse flow.
I have attache the CCL file about the BC and the expressions.
First I tried the Opening(Entrainment, static pressure) to have the zero gradient for the velocity and Velocity profile at the outlet. Although it follows the BC in negative velocity(simple sinusoidal BC), but completely unphysical results(compared to other studies).
Then I changed the outlet to mass flow rate, but again because of the artificial walls, it did not follow the BC setup.
I am wondering what would be the most suitable BC for my case that can give me physical results as well as flowing the BC setups.
I can not use the velocity profile because physically the profile is unknown, better to use mass flow or pressure that the profile of velocity is the part of the solution.


Thanks

[mejahan]

Hi Glenn,

I posted the CCL and looking forward to seeing your reply.

Thanks

[ghorrocks]

Can you make your boundary "Outlet" an opening set to cartesian velocity compnents? Then you can drive it with an osciallting flow.

Your boundary "Inlet" should probably be a opening as well, set to the 100mmHg pressure. I find the entrainment option numerically unstable so you might have more luck with opening pressure and direction.

As a side issue - why are you using a turbulence mode for this? I suspect the Reynolds number is pretty low (but cannot work it out as I do not know the geometry or fluid) so I suspect the flow is laminar.

[mejahan]

Hi Glenn,

Thanks for your reply.
I am trying the different possible options.
But about the SST, as the Re on the maximum flow goes beyond 7000, I am using it.

[mejahan]

Hi again,

The Opening BC gives the solver the option of having incoming and out coming flow at the boundary section.
But what is the difference between using Opening with velocity components and The Outlet with velocity components?
Both of them have to follow the velocity components across the boundary.

[ghorrocks]

Re=7000 - OK.

The opening allows flow in either direction. The outlet will only allow outwards flow.

[mejahan]

But even in velocity outlet BC, I can have the either direction defined by the profile of the velocity.
The same case for the Opening with the velocity components, the solver has to follow whatever velocity has been set at the section.

[ghorrocks]

If you specify inflow at an outlet boundary are you able specify the scalar variables with it? Things like temperature, turbulence and convection AVs? I suspect not.

[ghorrocks]

If you specify inflow at an outlet boundary are you able specify the scalar variables with it? Things like temperature, turbulence and convection AVs? I suspect not.