[Bodo1993]

Dear All,

I was wondering if the inletOutlet bounday condition is applicable for cases where the density of the fluid changes.

I was reading through the ANSYS manual and found that Outflow boundary condition cannot be used for transient simulations with variable density.

I use twoLiquidMixingFoam and have one inlet and two outlets. Fluid 1 inters the domain at which Fluid 2 is there. The two fluids mix (since miscible) and exits the domain. I get some issues at the outlet when the mixed phase reaches the outlet.

I would greatly appreciate your support.

Thanks.

[peterhess]

Hello Bodo!

In this toturial:

tutorials/compressible/rhoSimpleFoam/squareBend/

The fluid is perfect gas and the velocity is inletOutlet at the outlet!

Well, I think that the combination you are using is possible.

Regards

Peter

[Bodo1993]

Dear Peter,

Thanks a lot for your reply. Then, it seems that it should not have a problem.

In my simulations with twoLiquidMixingFoam multiphase solver, I have a single inlet and two outlets as shown in the attachment. The two fluids are expected to mix and exit through the outlets. I am wondering, what would be the appropriate outlet boundary conditions for the velocity, pressure and alpha phase in this case?

I use: pressureInletOutletVelocity for velocity, totalPressure for pressure and zeroGradient or inletOutlet for phase fraction.
The settings I use work fine if only single phase exists at the outlet boundary. However, when the mixed phase reaches the outlet boundary, I get some vortices as shown in the attachment.

I am wondering, what causes the vortices to develop at the outlet once the mixed phase reaches there and how would I resolve this issue. Please note that I am using a coarse mesh; however, I refined the mesh once and the issue persists.


Thank you for your time and cooperation, and I look forward to hearing from you.

[peterhess]

Hello Bodo!
Well, I dont realy understand which two fluids you are supposing here...

You have one inlet. i.e. one fluid.

Please clarify that.

------------------------------------

I suppose the simulation is turbulent, cause from the shape, I could difficult imagine that your simulation is laminar, unless the viscosity of the fluid is such high, that the turbulence desipation could destroy the turbulence.

The assumption of turbulent flow is the basis for the following discussion.

Now!

From the shape of the flow I could imagine that the flow is not leaving the geometry along the whole width of the outlet(s).

In this case a back flow could happening here factly.

And in this case you are not able to define a velocity boundary at the outlet like this:

outlet
{
type inletOutlet;
value uniform (0 0 0);
inletValue uniform (0 0 0);
}

This would be wrong cause you need to define a back flow velocity via inletValue!

A zero inletValue is not correct.

And in this case you need to specifi k & epsilon (supposing you are using those) for the defined inletValue velocity.

If you take a look to the tutorial I mentioned earlier, you will see the that k & epsilon at the outlet are also inletOutlet and with specified values.

Like that a vortex will happend at the outlet, actualy two of them in every outlet, one for fluid leaving the domain and one for the fluid entering.

--------------------------------------------------

Which pressure conditions? well it depends ubon what you are targeting to simulate...

As example:

Pressure:

inlet --> zeroGradient and outlet(s) --> fixedValue

Or any other combinations...

It realy depends ubon what are you simulating.

Velocity:

inlet --> fixedValue and outlet(s)--> inletOutlet or as you mentined pressureIletOutletVelocity

Or flowRateInletVelocity for the inlet...

alphat:

take it from the tutorial I mentioned above...

I hope it helps.

I dont use the solver you are using, that why I am not aware about some possible limitaions could exsist for this solver, just as a small note.

Regards

Peter


PS: good source for boundary conditions

http://www.nextfoam.co.kr/lib/downlo...bb43ccfe025b25

[Bodo1993]

Dear Peter,

Thanks for the detailed response.

Initially, there is another fluid (i.e. fluid 2) is occupying the channel. Therefore, the when fluid 1 is injected, the two fluids mix and exit the outlets.

In fact, the simulations are laminar. However, I was wondering, how would I know the back flow velocity that I have to specify for the inletValue priori?

Also, as you said, the fluid exist the outlets through the central cells of the outlet (does not exit from all cells). Kindly, what do you think are the main reasons for that? Would refining the mesh near the walls solve this issue?

Thanks and I look forward to hearing from you.

[peterhess]

Hello Bodo!
The schape u r simulating has 180° curve at every channel left and right.
Like that the flow momentum will push the flow to the outer wall of those channels.
And as a result, a sparated boundary layer is happening at (both) the corner.
The flow after traveling along the channel, will expand to "fill" the channel.
If the length of the channel is long enough, then the vortex caused via the separated boundary layer will vanich.
Simply increase the length of the channels at both side for a "suffcient length" to get an outflow from the channels that is expanded along the width.
In this case no inleValue for the velocity is needed...
In all cases, your flow must be turbulent calculated, cause the separated boundary layer will produce turbulence.
Unless the velocity is very low or/and the fluid very viscus...

Regards

Peter

[Bodo1993]

Hello Peter,
Thanks a lot for your time and elaboration.