[murx]

Hi there,

i am simulating a 2D incompressible laminar pipe flow around an obstacle. There is a relative speed between obstacle and wall, so i applied a wall velocity. See the attached sketch for more details.

I have a problem finding a suitable outlet boundary condition. I expect the outlet velocity profile to be slightly disturbed by the obstacle, so i can't apply a parabolic velocity profile like at the inlet. An "Outlet" with pressure BC prevents flow into the solution domain, which is not suitable either because there is inflow due to the wall shear. So I choose a pressure "Opening" BC. But the resulting outlet velocity profile does not look like it makes physically sense, see attached picture. If I turn off the wall velocity and thereby switch of the backflow into the solution domain, I get the exact velocity profile that I expect.

Is there a suitable outlet BC that for this problem? Switching to openFOAM would be an acceptable option for me.
Or is the only way to solve the problem placing the outlet further downstream and applying a parabolic velocity profile? And if so... is there a rule of thumb how big the distance between obstacle and outlet has to be to assume undisturbed flow?

Thanks!

[m9819348]

Hi,

I would move the outlet backwards by ten times the diameter of the pipe and apply a uniform pressure outlet.


At the location where you want to know the pressure (according to your sketch), the parabolic velocity profile should occur.


This works in any code, open source or proprietary.


Ries Bouwman

[murx]

Thanks for the quick reply, Ries!

A uniform pressure "outlet" is not possible as this prevents backflow into the domain, which is present due to the wall velocity. A pressure "opening" with inlet Flow velocity set as "normal to boundary" is what I applied. The green/blue arrows show the awkward calculated velocity profile at the outlet. Do you think moving the opnenig further downstream will fix this?

[ghorrocks]

Boundary conditions which have both forward and backward flow on the one boundary are always going to be difficult to get right. So I agree with Ries, you have to move this further away from your region of interest so the error in the boundary can be fixed up by the time it propogates to your region of interest.

[m9819348]

If you think it is not physical to elongate the outlet, there might be other options.

I am not sure what code you are using? (I did not see it in your email and also missed in what forum we are here...).

OpenFOAM: there is an outlet boundary condition called inletOutlet which allows the behaviour you are describing.

To my knowledge, FLUENT allows for something similar.
Hence I assume other widely used codes (STAR, ...) have similar options.

Summary:
- the easy way is elongating the geometry to prevent any numerical difficulties at the outlet to occur.
- the hard way is to use more sophisticated outlet boundary conditions, with the risk they might diverge more easily...

Don't forget: if what you are trying to simulate (or expect from the simulation) is not physical, your code (no matter which) will blow up most likely! :-)

Good luck!

[ghorrocks]

Just to clarify Ries's reply - CFX does have a combined inflow/outflow boundary, it is called an opening. However, they are numerically less stable than the simpler single flow direction boundary (no matter what CFD code you are using) so that is why the simplest thing to try first is moving the outlet boundary down stream.

[murx]

I extended the domain so the distance between obstacle and outlet is now 6 times the channel diameter, which is more than the hydrodynamic entrance length according to the formula L = 0.03 * Re (=180) * D = 5.4 D.

Unfortunately, the velocity profile at the opening on the right still looks the same.

[ghorrocks]

You have missed our point. Moving the boundary downstream will not make the flow correct at the boundary. What it will do is allow enough room for the correct flow to establish between the boundary and your region of interest so the region of interest is correct.

[murx]

Ok, now i've got it
I thought that the lower extend of velocity perpendicular to the pipe axis further downstream would make the "normal to boundary" option in the opening settings more adequate and thereby help CFX to find a reasonable solution.

Since you said that this is a general numerical problem and not specifically a CFX-problem, I guess the next step for me will be to totally dismiss the pressure boundary condition and instead apply the same velocity profile as I did at the inlet. Though I know that in there is no ideal parabolic profile, it is still closer to reality than what I get with the pressure BC.

Thanks Ries and Glenn

[ghorrocks]

No, you cannot apply a velocity boundary at the inlet and outlet for a steady state simulation. This is not well-posed. Read the documentation about setting up boundary conditions. You will probably need a velocity and a pressure boundary, but which is inlet and outlet does not matter.

[m9819348]

Hi,

I agree with Glenn.

The easiest solution in my opinion would be:
- original geometry
- inlet velocity profile as needed
- outlet elongated by roughly 10x the diameter
- give new outlet (at 10xdiameter original location) pressure outlet condition
- get your post-rpocessing data at original outlet condition and you will see the backflow (or whatever phenomena you want to see).

I am not available this week, but feel free to call me anytime next week.

Ries