[AS_Aero]

Hi All

I am doing a Rotor- Stator crossflow fan simulaton !

Inorder to study the effects of geometry etc, I am trying a quasi 2D RANS simulation and then use these data for intializing the URANS computations.

But I am facing a problem or I am not sure why this is happening :

With one simulation RANS, I kept Iterations 3000 and Physical Timescale as 0.5s

With another one RANS, 3000 Iterations, Physical TImescale as 2 seconds

And when I check the value of Power the value differs, The one with 2 second is producing 0.85W and the one with 0.5s is producing 0.76W

Its a RANS computation and Frozen Rotor case. Can someone tell my why this difference ? What is the influence of Physical TImescale ?
And what is the best value for Physical Timescale for a rotor stator configuration with Rotor 400RPM and free velocity of 10m/s and 21 blades

[ghorrocks]

For steady state simulations the time step size is not important. What is important is whether you are adequately converged or not. The fact that two simulations of the same thing with different numerical conditions says that you are not adequately converged.

Run both 0.5s and 2s time step simulation for longer to get tighter convergence and they should give the same results (when they are adequately converged).

[AS_Aero]

Hi Glenn

I have attached the image of the streamlines for two cases
Here one is the geometry is small at the outflow region and the other is bigger.

The thing is for smaller domain I am getting Power of 0.846 W and for the bigger domain 0.747 W.
But normally for bigger domain the recirculation should not be affecting the flow of the rotor right ? So that I should have more power than the smaller domain where there will be recirculation ! (correct m if I am wrong)

And then the other issue is as I said before
For same domain I am changing the Physical timescale from
2seconds Power = 0.8498W
0.5seconds) Power =0.76355 W
0.0238seconds (based on one over omega rule for rotor) Power = 0.846 W
All ran for 3000 Iterations !
You can see the convergence plot as well for one case in the image.
Should I run it longer as you said ? All the cases and see or ?

[ghorrocks]

You are clearly getting a big effect on the domain size. So obviously your domain needs to be a lot longer than it is. I recall Gert-Jan and myself saying that on another thread - well, you have now proven it so you know you need to make it longer.

Your convergence is poor and there is no point continuing as it is not converging. Read this FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

But your convergence will improve a lot when you move your outlet boundary further downstream.

[AS_Aero]

Hi Glenn

Thanks a lot for your reply. But my main concern here is the block is 2m high and the outflow domain is alredy 6m and now i did with 11m distance and again the recirculation region is increasing till the outlet. So am confused if its something wrong with my boundary condition ?
I am giving Opening boundary with Avg static pressure and dir and relative pressure as 0 atm since reference pressure is 1atm.

Then in the residual plot it ran for 10000 iterations and my RMS P-Mass is not going further, dont know why . Images attached.
If I go on extending the domain at the outflow it will basically increase the recirculation length. But in theory there is some findings right for flow around a block the recirculation length is fixed there right ? Kindly correct me if am wrong

[ghorrocks]

You don't want an outlet boundary in a recirculation. Keep pushing it downstream. Yes, recirculations can be quite big.

[AS_Aero]

Is there any rule of thumb to calculate the length of recirculation , based on our flow and height of the block ?

[ghorrocks]

I am not aware of a rule of thumb. Recirculations get very large - the recirculation behind a building or a truck go for a long way.

If you want to find out how big your recirculation is just model a really, really long downstream section. Then you should be able to see its length.