[Nek5000-users] Nek5000-users Digest, Vol 108, Issue 2

Fri Feb 2 22:52:05 CST 2018

The turb_outflow boundary condition accelerates the flow at the exit (like a nozzle) so that all characteristics are outward pointing.  At the outflow, the velocity becomes uout=u+Uout, where Uout is the additional velocity.   This additional velocity is generated by setting the divergence to be positive in the last layer of elements (any element with an 'O  ' BC).

turb_outflow was originally written to vascular flows (i.e., internal flows) where there is nearly a 1-to-1 relationship between the mean inlet velocity and exit velocity.   In that case Uout (and the consequent requirements for the amount of divergence required to generate Uout) could be determined automatically.   In these cases, rq > 1 suffices to set the flux-ratio (qout/qin) = rq automatically.   rq=2 ==> ratio of 2, which translates to a velocity ratio of 2 when the inlet and outlet areas are the same.    If the parameter uin := 0, the code tries to estimate the velocity near the exit and then adjust divergence so that uout/ubar = rq.   In some cases (such as a small jet in a big domain), the mean velocity (flux / area) is nowhere near what you want for a corrected velocity --- because you need to account for the high velocity at the jet.  In this case, you prescribe an input value --- uin=1.0 is reasonable.  If uin>0, the code sets ubar=uin to be your prescribed value and will set the divergence such that uout/ubar ~= rq.

What is important is that (uout-uin) > u', where u' is the magnitude of your reversed flow.

hth,

Paul

________________________________
From: Nek5000-users <nek5000-users-bounces at lists.mcs.anl.gov> on behalf of nek5000-users at lists.mcs.anl.gov <nek5000-users at lists.mcs.anl.gov>
Sent: Friday, February 2, 2018 10:33:35 PM
To: nek5000-users at lists.mcs.anl.gov
Subject: Re: [Nek5000-users] Nek5000-users Digest, Vol 108, Issue 2

Thank you Paul and Phillip for such a quick reply. I will run the jet case attached. So why was there no such problem when the first vortex from the wake of a circular cylinder was leaving the domain?

On Sat, Feb 3, 2018 at 1:49 AM, <nek5000-users-request at lists.mcs.anl.gov<mailto:nek5000-users-request at lists.mcs.anl.gov>> wrote:
Send Nek5000-users mailing list submissions to
        nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>

To subscribe or unsubscribe via the World Wide Web, visit
        https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users
or, via email, send a message with subject or body 'help' to
        nek5000-users-request at lists.mcs.anl.gov<mailto:nek5000-users-request at lists.mcs.anl.gov>

You can reach the person managing the list at
        nek5000-users-owner at lists.mcs.anl.gov<mailto:nek5000-users-owner at lists.mcs.anl.gov>

When replying, please edit your Subject line so it is more specific
than "Re: Contents of Nek5000-users digest..."

Today's Topics:

   1. Outflow Boundary Condition Clarification
      (nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>)
   2. Re: Outflow Boundary Condition Clarification
      (nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>)
   3. Re: Outflow Boundary Condition Clarification
      (nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>)

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

Message: 1
Date: Sat, 3 Feb 2018 00:40:32 +0530
From: nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>
To: nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>
Subject: [Nek5000-users] Outflow Boundary Condition Clarification
Message-ID:
        <mailman.7741.1517598636.19102.nek5000-users at lists.mcs.anl.gov<mailto:mailman.7741.1517598636.19102.nek5000-users at lists.mcs.anl.gov>>
Content-Type: text/plain; charset="utf-8"

Im trying to simulate the formation of shear layer when a jet exits a
nozzle and enters the flow domain. As the FIRST vortex leaves the outlet (
at which I have provided 'O' boundary condition using genbox) the solution
diverges. I tried to implement the 'turbulent outflow' subroutine as
suggested in the forum but now the vortex affects the upstream flow. But
when I run the flow past circular cylinder example, the vortices leave the
domain without any issue even though only 'O' boundary condition is used'.
What is the difference between the two cases and what can i do to prevent
the issue?

--
Nitish Kovalam
Aerospace Engineering
Indian Institute of Space Science and Technology
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20180203/87028828/attachment-0001.html>

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

Message: 2
Date: Fri, 2 Feb 2018 20:27:50 +0100
From: nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>
To: nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>
Subject: Re: [Nek5000-users] Outflow Boundary Condition Clarification
Message-ID:
        <mailman.7745.1517601585.19102.nek5000-users at lists.mcs.anl.gov<mailto:mailman.7745.1517601585.19102.nek5000-users at lists.mcs.anl.gov>>
Content-Type: text/plain; charset=utf-8; format=flowed

I think you should try the stabilised O condition, as described in a
paper by Dong (2014). We have an implementation of that, we should
probably provide it as a module in the repository.

best regards,
Philipp

On 2018-02-02 20:10, nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov> wrote:
> Im trying to simulate the formation of shear layer when a jet exits a
> nozzle and enters the flow domain. As the FIRST vortex leaves the outlet
> ( at which I have provided 'O' boundary condition using genbox) the
> solution diverges. I tried to implement the 'turbulent outflow'
> subroutine as suggested in the forum but now the vortex affects the
> upstream flow. But when I run the flow past circular cylinder example,
> the vortices leave the domain without any issue even though only 'O'
> boundary condition is used'. What is the difference between the two
> cases and what can i do to prevent the issue?
>
> --
> Nitish Kovalam
> Aerospace Engineering
> Indian Institute of Space Science and Technology
>
>
> _______________________________________________
> Nek5000-users mailing list
> Nek5000-users at lists.mcs.anl.gov<mailto:Nek5000-users at lists.mcs.anl.gov>
> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users
>

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

Message: 3
Date: Fri, 2 Feb 2018 20:19:54 +0000
From: nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>
To: "nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>"
        <nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>>
Subject: Re: [Nek5000-users] Outflow Boundary Condition Clarification
Message-ID:
        <mailman.7749.1517602797.19102.nek5000-users at lists.mcs.anl.gov<mailto:mailman.7749.1517602797.19102.nek5000-users at lists.mcs.anl.gov>>
Content-Type: text/plain; charset="us-ascii"

Attached is a .usr with turb_outflow that works for this case---there is

no difficulty if you use the prescribed input values, as shown in the attached

files.

Here is a movie of the result - you can see that turb_outflow is turned on prior to the jet reaching the top of the domain.

http://mcs.anl.gov/~obabko/jet_vm.mpeg

This mesh is a bit under-resolved in the z-direction.

The files for a new case, with more axial resolution, are posted here

www.mcs.anl.gov/~fischer/jet2.tgz<http://www.mcs.anl.gov/~fischer/jet2.tgz><http://www.mcs.anl.gov/~fischer/jet2.tgz>

I'll be posting an example with a script on how to build this geometry to nekexamples soon.

Paul

________________________________
From: Nek5000-users <nek5000-users-bounces at lists.mcs.anl.gov<mailto:nek5000-users-bounces at lists.mcs.anl.gov>> on behalf of nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov> <nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>>
Sent: Friday, February 2, 2018 1:10:32 PM
To: nek5000-users at lists.mcs.anl.gov<mailto:nek5000-users at lists.mcs.anl.gov>
Subject: [Nek5000-users] Outflow Boundary Condition Clarification

Im trying to simulate the formation of shear layer when a jet exits a nozzle and enters the flow domain. As the FIRST vortex leaves the outlet ( at which I have provided 'O' boundary condition using genbox) the solution diverges. I tried to implement the 'turbulent outflow' subroutine as suggested in the forum but now the vortex affects the upstream flow. But when I run the flow past circular cylinder example, the vortices leave the domain without any issue even though only 'O' boundary condition is used'. What is the difference between the two cases and what can i do to prevent the issue?

--
Nitish Kovalam
Aerospace Engineering
Indian Institute of Space Science and Technology
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20180202/7cbaf33d/attachment.html>
-------------- next part --------------
A non-text attachment was scrubbed...
Name: jet2.usr
Type: application/octet-stream
Size: 18256 bytes
Desc: jet2.usr
URL: <http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20180202/7cbaf33d/attachment.obj>

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

Subject: Digest Footer

_______________________________________________
Nek5000-users mailing list
Nek5000-users at lists.mcs.anl.gov<mailto:Nek5000-users at lists.mcs.anl.gov>
https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users

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

End of Nek5000-users Digest, Vol 108, Issue 2
*********************************************

--
Nitish Kovalam
Aerospace Engineering
Indian Institute of Space Science and Technology
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20180203/a188b369/attachment-0001.html>