[AS_Aero]

Hi All

I did a simple Pipe flow simulation with a diffuser at the end and I did a RANS computation using CFX with
Inlet as massflow boundary condition
Outlet as the Avg static pressure =0 atm
Ref Pressure as 1 atm
Flow is incompressible

And I got a warning in the out file even though it ran completely

OUTER LOOP ITERATION = 768 CPU SECONDS = 2.478E+05
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom | 0.99 | 1.5E-04 | 1.0E-02 | 1.3E-01 ok|
| V-Mom | 0.97 | 1.2E-04 | 8.1E-03 | 9.2E-02 OK|
| W-Mom | 0.96 | 1.2E-04 | 1.2E-02 | 8.8E-02 OK|
| P-Mass | 0.90 | 2.1E-05 | 3.3E-03 | 14.2 3.9E-01 ok|
+----------------------+------+---------+---------+------------------+
+--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 48.9% of the faces, 24.6% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: Outlet. |
| The fluid name is: Fluid 1. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+--------------------------------------------------------------------+
| K-TurbKE | 1.22 | 1.4E-03 | 5.1E-02 | 10.3 6.5E-02 OK|
| E-Diss.K | 1.28 | 7.3E-03 | 1.1E+00 | 10.8 1.4E-03 OK|

This Warning at the OUTLET is always there but with different % . What could be the reason. Have anyone faced this and does it affect our simulation !

Also is there any other Boundary condition that I could specify. I cant extend the outlet as I need to measure the pressure and velocity exactly at the Area of outlet.


Thanks in advance.

[ghorrocks]

FAQ: https://www.cfd-online.com/Wiki/Ansy...f_an_OUTLET.22

[AS_Aero]

Hi Glenn

Yes its a good assumption and as I mentioned already, that I cant extend my outlet as for me its important to have that pressure value from that surface and velocity profile etc to continue the simulation further.

The third option :
If the outlet and the wall is not significantly affecting your results you can ignore it and accept the solution with the back flow warning.
But how to decide this whether its affecting or not ? And how to see that reversed flow happening or not ? This happens only when I give average static pressure as the outlet. (which I gave as zero ) as mentioned previously.

[ghorrocks]

Draw velocity vectors on the outlet. Then you can see what the flow is doing there.

To see if it is significant, compare it to a simulation with the outlet moved downstream.

[AS_Aero]

Cool !! I tried the Velocity vector and it looks like a messed up the vectors are coming out of the geometry domain and its spread in all direction; as its a diffuser at the end and before that there is a swirl chamber.
But just a note :
This warning came when I gave the Outlet
Pressure: Avg Static Pressure =0 bar
Pres Profile Blend 0.05
Pressure Avg: Over whole outlet
But with the other one like
Outlet BC: Pressure: Static Pressure =0 bar
There is no warning !! So it has something to do with this outlet definition.
So now am not sure if I should give the average over the outlet area or just the Static pressure as Zero !!

But thanks a lot for your description.

[ghorrocks]

You should apply a boundary condition which matches the flow conditions you know exist at that location. If you do not know the flow conditions at that location you must move to another location where you do know the conditions. That is why they are called boundary conditions.

[AS_Aero]

That's the problem. I dont have information about the outlet. Its like a pipe flow with a nozzle at the outlet. So I know the inlet pressure and flow rate and the outlet is exposed to the atmosphere, thats the reason I gave the outlet BC'n as Pressure with Static Pressure as Zero and Reference pressure as the 1 Atmospheric pressure. What else can I give ? Or I could apply opening boundary condition and then I have to give the static pressure value as well. So instead I thought this is better. Whats your opinion ?

[ghorrocks]

If you don't know what is happening at your outlet then you cannot put a boundary condition there.

But you do know it vents to atmosphere, so you know the pressure there. The most accurate way of modelling this is to have a large volume at the end of the pipe to allow the jet to expand out and reach a low velocity - then you can apply a simple static pressure boundary as an opening.

If you want a simple simulation but not as accurate you can put the outlet at the exit plane of the pipe. This is usually pretty close to atmospheric pressure for many cases. This approach is less accurate but easier to implement.

[AS_Aero]

Hi Glenn

Yes you are right I gave the pressure at the boundary I have provided the link below regarding to that : I wanted to confirm the BC'n what I gave is correct

Pressure Boundary at Outlet

And actually its a spray so if I give a big doomain at the outlet then I will have to go to multiphase flow and doing that with the geomety completly will be very expensive . That is the reason I split the simulation into two part. One is completely single phase flow that is the pipe internal flow and then take the velocity profile and turbulence data from the outlet and feed it to the multiphase simulation domain. Because of this reason I cant extend my domain or something. If you can provide me your email I can send you more details !!

So here the problem is the experements are conducted at lets say 10bar and they have a flow rate of 5L/min ; so when Idid the simulation I gave the flow rate at the inlet and when I cross check its not showing that 10 bar pressure. so normally it should show that right ?? And as you mentioned I was already giving reference pressure as 1 atm adn staatic pressure at the outlet as 0 bar.

[ghorrocks]

It sounds like a case of either an incorrectly set up simulation (your boundary condition approach should especially problematic) or inaccurate simulation numerics. This is exactly what I said on the other post which you have linked to.

[AS_Aero]

The flow and everything seems normal to me but I dont know where am I going wrong. !! afterall its just an internal pipe flow.

[ghorrocks]

Please post an image of what you are modelling, your mesh, your output file and an image of the flow you are currently getting.

[AS_Aero]

Hi Gelnn

Am attaching you the details with the image

Kindly have a look and let me know. I am not able to attach the output file since its really big.

[AS_Aero]

Here is the Output file , I deleted the iterations inbetween..so it got small !!
Thanks

[ghorrocks]

I see lots of problems.

1) Single precision solver - change to double precision
2) Auto time scale control - read the FAQ and/or the CFX documentation on time step size. You can normally do a lot better than the auto mode.
3) Your outlet looks really close to some edges and separations - but having said that your 10000th iteration does not show any backflow. But I would be very careful about this - you might have some regions of backflow in reality which are actually air penetrating into the nozzle. This will affect the result.

[AS_Aero]

Dear Glenn

Yes I will change it to double and also I havent tried with this time scale control.
Regarding the outlet yes its close to the diffuser kind of part (as you can see) but the warning goes off at 65th iteration itself.so from then nothing is there.And what do you think about my Physiscs setup ? ('I used k-Epsilon Scalable wall function' ) The reference pressure and outlet static pressure thing ? Also regarding the TimeScale factor where I have given 1.

Also just a small doubt regarding the Solver Control
I was using Equation Class Settings / Equation Class : Continuity Equation
But dint give the further options like Advection Scheme and High Resolution etc…
Do I have to select them for this case ? Whats your opinion on that ?

[ghorrocks]

If the warning goes off that suggests it is OK.

Scalable wall functions - do a sensitivity analysis and figure out if it is significant in your case.

Reference Pressure - do a sensitivity analysis and figure out if it is significant in your case.

Outlet static pressure - ditto.

If you are not sure if some choices you made are right then try some alternatives and see if it makes a difference. If no difference then it does not matter (so choose the easiest one to work with). If it makes a difference then you know this is something you need to do some work on to get an accurate simulation.

[AS_Aero]

Also I couldnt find the option for Double Precision in CFX Pre !! Where can I find it ( I am running my job in Cluster)

[ghorrocks]

In the execution options. You can also set it by CCL or in the solver manager. Use the documentation to find the exact locations.